CAMWorks Nesting User Guide and Tutorials

CAMWorks Nesting User Guide and Tutorials
Cover Page
CAMWorks Nesting
2015
User Guide
&
Tutorials
Disclaimer
Geometric Americas Inc. makes no warranties, either expressed or implied with
respect to this manual. Geometric Americas Inc. reserves the right to revise and
improve products as it sees fit, and to revise the specifications and information
contained herein without prior notice. Due to continuing product development,
specifications and capabilities described in this manual are subject to change without
notice.
Trademarks
The following and other product names and corporate references herein are registered
or proprietary trademarks of their respective owners.
CAMWorks Nesting is a registered trademark of Geometric Americas Inc.
SOLIDWORKS® is a registered trademark of Dassault Systèmes SolidWorks Corp.
Microsoft®, Windows®, Windows Vista®, Window 7® and Access® are registered
trademarks of Microsoft Corporation in the United States and/or other countries.
All other brands and names are the property of their respective owners.
Copyright © 2013-2015 Geometric Ltd. (A division of Geometric Americas, Inc.)
All Rights Reserved.
Geometric Ltd. is a subsidiary of Geometric Americas, Inc.
Product Name:
CAMWorks Nesting
Version:
2015 SP 0.0
License Version Date: September 15, 2014
CAMWorks Nesting Tutorial
TABLE OF CONTENTS
CAMWORKS NESTING: INTRODUCTION.................................................................. 11
What is CAMWorks Nesting? .................................................................................................11
Procuring CAMWorks Nesting ...............................................................................................11
Why CAMWorks Nesting should be your preferred nesting program .................................11
Receiving latest updates & Update Support Plan (USP) ......................................................12
Update Support Plan ...........................................................................................................12
Technical Support ...................................................................................................................13
CAMWorks Nesting Installation & License Activation .........................................................13
CAMWorks Nesting Tutorials .................................................................................................13
ABOUT THESE TUTORIALS ...................................................................................... 14
UNDERSTANDING THE CAMWORKS NESTING FUNDAMENTALS ....................... 17
Basic Procedure of Nesting ...................................................................................................17
Flowchart on Basic Procedure to Implement Nesting ..........................................................20
The Part Model/Assembly.......................................................................................................22
Defining Part Parameters .......................................................................................................23
The Part data Tab ...............................................................................................................23
Part List ...............................................................................................................................23
Thickness ............................................................................................................................24
Material ...............................................................................................................................24
Rotation Angle.....................................................................................................................25
Grain Direction ....................................................................................................................26
Normal Face .......................................................................................................................27
Quantity...............................................................................................................................28
Defining Sheet Parameters.....................................................................................................29
The Sheet data Tab.............................................................................................................29
Sheet List ............................................................................................................................30
Thickness ............................................................................................................................30
Material ...............................................................................................................................31
Quantity...............................................................................................................................31
Grain Direction ....................................................................................................................31
Assigning Grain directions ............................................................................................................. 31
Add Sheet & Remove Sheet buttons ...................................................................................32
Sheet Size ...........................................................................................................................32
Defining Standard Sheet ................................................................................................................ 33
Defining Custom Size Sheet .......................................................................................................... 34
Defining Sheet DXF ....................................................................................................................... 34
Defining Multi Head Options Parameters ..............................................................................35
How the functionality of nesting with multiple tool heads works ...........................................36
The Default Settings in the Multi Head Options tab .............................................................36
SingleTHMachine (Single Tool Head Machine) ............................................................................. 36
Enabling Multi Tool Head Machining ...................................................................................37
Table of Contents
i
CAMWorks Nesting Tutorial
Parameters and Data fields in the Multi Head Options tab ..................................................37
Sheet List ....................................................................................................................................... 38
Machine (machine name)............................................................................................................... 38
Number of Tool Heads ................................................................................................................... 39
Multi-tool head nesting type ........................................................................................................... 39
Rail direction .................................................................................................................................. 39
Tool head distance ......................................................................................................................... 40
Editing the default settings for the Multi Head Options tab ..................................................40
Define Nesting Data Parameters ............................................................................................40
Part to Part Distance ...........................................................................................................41
Part to Sheet Distance ........................................................................................................41
Output Assembly file ...........................................................................................................41
Assembly Template Path ....................................................................................................42
Save output as dxf ..............................................................................................................42
Automatically Select Sheet ..................................................................................................42
Setting the Forecaster Method in DefaultValues.ini ....................................................................... 43
Create Separate Assembly..................................................................................................43
Nesting Type .......................................................................................................................43
Max Nesting time ................................................................................................................43
Generating the Nested Layout ...............................................................................................44
How the Nested layouts generated are saved within SOLIDWORKS ..................................44
TUTORIAL 1 - NESTING AN ASSEMBLY ................................................................... 45
Step 1: Open the Assembly ....................................................................................................45
Step 2: Assign Nesting Parameters .......................................................................................45
Part Data Tab ......................................................................................................................45
Sheet Data Tab ...................................................................................................................45
Nesting Parameters.............................................................................................................46
Step 3: Generating the Nested Layout ...................................................................................46
Summary Text .....................................................................................................................46
Nested Assembly ................................................................................................................47
INITIALIZATION FILES OF CAMWORKS NESTING .................................................. 49
Location of the CAMWorks Nesting Initialization files .........................................................49
Backing up the Initialization Files ..........................................................................................49
Configuration settings available in Initialization files ..........................................................49
StandardsSheets-INCH.ini & StandardsSheets-MM.ini .......................................................51
Viewing the StandardSheets-INCH.ini/ StandardsSheets-MM.ini file: ..................................51
Adding sheets to the StandardSheets-INCH.ini/ StandardsSheets-MM.ini file: ....................51
Editing parameters in StandardSheets-INCH.ini/ StandardsSheets-MM.ini file ....................52
Material.ini ...............................................................................................................................53
Location ..............................................................................................................................53
Viewing/Editing the Material dropdown list ..........................................................................53
DefaultValues.ini .....................................................................................................................54
Location ..............................................................................................................................54
Assigning default Part Quantity ...........................................................................................54
Steps to edit default part quantity in the DefaultValues.ini file ....................................................... 54
ii
Table of Contents
CAMWorks Nesting Tutorial
Defining default Sheet Thickness and Quantity ...................................................................54
Steps to edit default sheet thickness and quantity in DefaultValues.ini file ................................... 54
Defining default dimensions for Custom Sheet ....................................................................55
Editing the Default Custom Size Dimensions in the DefaultValues.ini file ..................................... 55
Assigning default Part to Part Distance & Part to Sheet Distance ........................................56
Editing the Part to Part distance and Part to Sheet Distance ........................................................ 56
Enabling/Disabling the Preferential Hole Filling Functionality ..............................................57
Assigning default state for the Create Separate Assembly option........................................57
Assigning default state for the Automatically Select sheet option ........................................58
Enabling/Disabling the option of Flattening Sheet Metal Parts .............................................58
Enabling/Disabling the option of utilizing „Fix Component‟ or „Mate-Lock‟ feature ................59
Assigning the default Inventory Forecasting method ...........................................................60
Assigning default state for the „Save Output as dxf‟ option ..................................................60
Enabling/disabling the functionality to add nested Parts to CAMWorks Part Manager .........61
Enabling/disabling the Display of the Message shown before linking CAMWorks Nesting
with CAMWorks...................................................................................................................61
Enabling/disabling the feature of „Assigning Assembly Quantities‟ ......................................62
Settings for the Stamp Feature Unfold Option .....................................................................62
Machine.ini ..............................................................................................................................64
Configuration settings in the Machine.ini file ........................................................................64
Location ..............................................................................................................................64
Enabling/Disabling the option of Nesting with Multiple Tool heads ......................................65
Enabling/disabling the display of the Multi Head Options tab in the Create Nesting Job
dialog box............................................................................................................................66
Defining the Machines which support nesting with multiple tools .........................................67
Assigning the Machine Count, machine names and default machine ........................................... 67
The Default Machine Configuration .....................................................................................68
Defining default parameter values for Machines which support nesting with multiple tools ..69
Adding a new machine in the Machine.ini file ......................................................................70
TUTORIAL 2- SINGLE PART, SINGLE SHEET NESTING FOR A SOLID PART ...... 73
Introduction .............................................................................................................................73
STEP 1: Open the Part ............................................................................................................73
STEP 2: Define the Part Parameters ......................................................................................74
STEP 3: Define the Sheet Parameters & adding a standard sheet ......................................75
STEP 4: Selecting a machine with Single Tool Head for the Nesting Process ...................77
STEP 5: Define Nesting Parameters ......................................................................................77
STEP 6: Generating the Nested Layout .................................................................................78
Result A ..............................................................................................................................79
Result B ..............................................................................................................................79
Result C ..............................................................................................................................80
TUTORIAL 3 – SINGLE PART, SINGLE SHEET NESTING FOR SHEET METAL
PART ............................................................................................................................. 82
Introduction .............................................................................................................................82
STEP 1: Open the Part ............................................................................................................82
STEP 2: Change in Configuration File settings ....................................................................83
Table of Contents
iii
CAMWorks Nesting Tutorial
Enabling the option to Flatten Sheet Metal Part...................................................................83
Enabling the Fix Component Feature of SOLIDWORKS .....................................................83
STEP 3: Define the Part Parameters ......................................................................................83
STEP 4: Defining a „Custom‟ size sheet ................................................................................84
STEP 5: Selecting a machine with Single Tool Head for the Nesting Process ...................85
STEP 6: Define Nesting Parameters ......................................................................................85
STEP 7: Generating the Nested Layout .................................................................................85
TUTORIAL 4 – NESTING OF MULTIPLE PARTS BASED ON THICKNESS ............. 87
Introduction .............................................................................................................................87
STEP 1: Using „Nest by Folder‟ to open the Assembly .......................................................87
STEP 2: Define the Part Parameters ......................................................................................88
Selectively Nesting Parts .....................................................................................................88
Material ...............................................................................................................................89
Normal Face .......................................................................................................................89
Grain Direction ....................................................................................................................89
Step Angle ..........................................................................................................................89
Quantity...............................................................................................................................89
STEP 3: Adding a sheet of using „DXF‟ file. ..........................................................................90
STEP 4: Selecting a machine with Single Tool Head for the Nesting Process ...................91
STEP 5: Define Nesting Parameters ......................................................................................91
STEP 6: Nesting all the Parts in the Assembly .....................................................................92
Adding a standard sheet .....................................................................................................93
Nesting of multi-body parts....................................................................................................95
Steps to nest a Multi-body Part ...........................................................................................95
Nesting of assemblies containing multi-body parts .............................................................96
Steps to nest an Assembly containing Multi-body Parts ......................................................96
TUTORIAL 5 – NEST BY MATERIAL, NEST BY THICKNESS .................................. 98
Introduction .............................................................................................................................98
Preferential Hole Filling .......................................................................................................98
STEP 1: Enabling „Preferential Hole Filling‟ functionality ....................................................98
STEP 2: Using „Nest by Folder‟ to open the Assembly .......................................................98
STEP 3: Define the Part Parameters ......................................................................................99
Thickness & Material of the parts ........................................................................................99
Normal Face .....................................................................................................................100
Grain Direction ..................................................................................................................100
Step Angle & Quantity .......................................................................................................100
STEP 4: Defining sheet parameters .....................................................................................101
Adding Standard Sheet .....................................................................................................101
Adding Standard Sheet 2 ..................................................................................................102
STEP 5: Selecting a machine with Single Tool Head for the Nesting Process .................103
STEP 6: Define Nesting Parameters ....................................................................................103
Step 7: Generating the Nested Layout .................................................................................103
Saving Files in the .dxf format ...........................................................................................103
iv
Table of Contents
CAMWorks Nesting Tutorial
Summary File ....................................................................................................................103
Viewing the Nested Layouts ..............................................................................................104
TUTORIAL 6 – NESTING WITH MULTIPLE TOOL HEADS ..................................... 106
Introduction ...........................................................................................................................106
STEP 1: Open the Assembly ................................................................................................106
STEP 2: Enabling the option of flattening the sheet metal parts .......................................107
STEP 3: Define the Part Parameters ....................................................................................107
STEP 4: Define the Sheet Parameters .................................................................................108
STEP 5: Define the Multi head options parameters ............................................................108
STEP 6: Define Nesting Parameters ....................................................................................110
Step 7: Generating the Nested Layout .................................................................................110
TUTORIAL 7 – NESTING IMPORTED SHEET METAL COMPONENTS WITH BENDS
..................................................................................................................................... 112
Introduction ...........................................................................................................................112
The functionality of Unfolding Sheet Metal Parts ...............................................................112
The „Unfold Imported Bodies‟ dialog box ...........................................................................112
Commands to Invoke „Unfold Imported Bodies‟ dialog box ..............................................113
1. The „Enable Auto Unfold‟ Option ................................................................................113
2. The „Intelligent Unfold‟ Command ..............................................................................114
Function ....................................................................................................................................... 114
Command Execution .................................................................................................................... 114
How it works ................................................................................................................................. 114
Next Step ..................................................................................................................................... 115
3.
The „Unfold All Parts‟ Command ................................................................................115
Function ....................................................................................................................................... 115
Command Execution .................................................................................................................... 116
How it works ................................................................................................................................. 116
Next Step ..................................................................................................................................... 117
STEP 1: Open the Assembly ................................................................................................117
STEP 2: Unfolding the Parts with bends .............................................................................118
STEP 3: Defining the Part, Sheet & Nesting Parameters ....................................................120
Part Data Tab ....................................................................................................................120
Sheet Data Tab .................................................................................................................120
Nesting Parameters...........................................................................................................121
Step 4: Generating the Nested Layout .................................................................................122
TUTORIAL 8 – UNFOLDING IMPORTED 3D SHEET METAL COMPONENTS WITH
FAULTY SURFACES ................................................................................................. 123
Introduction ...........................................................................................................................123
STEP 1: Open the Assembly ................................................................................................123
STEP 2: Executing the „Intelligent Unfold‟ command .........................................................124
STEP 3: Selective unfolding of imported parts ...................................................................124
STEP 4: Executing the Nesting Job .....................................................................................130
Table of Contents
v
CAMWorks Nesting Tutorial
Part Data Tab ....................................................................................................................130
Sheet Data Tab .................................................................................................................130
Nesting Parameters...........................................................................................................131
Step 5: Generating the Nested Layout .................................................................................131
TUTORIAL 9 – ASSIGNING ASSEMBLY QUANTITIES ........................................... 133
Introduction ...........................................................................................................................133
STEP 1: Open the Assembly ................................................................................................133
Components of the Parent Assembly ................................................................................134
STEP 2: Enabling the option of flattening the sheet metal parts ...................................137
STEP 3: Enabling the feature for Assigning Assembly Quantities ....................................137
STEP 4: Open the „Create Nesting Job‟ Dialog box ............................................................137
Assembly Column .............................................................................................................138
Part name column .............................................................................................................138
Quantity Column ...............................................................................................................138
Step 5: Changing the quantity of the Parent assembly ......................................................139
Analysis.............................................................................................................................139
STEP 6: Changing the Quantity of a sub-assembly............................................................140
Analysis.............................................................................................................................141
STEP 7: Changing the Quantity of Parent Assembly .........................................................142
Step 8: Overwriting automatically assigned Quantity values for Parts with user-defined
values ....................................................................................................................................143
Step 9: Deactivating the feature of assigning assembly quantities ..................................144
Deactivating the feature only for the current nesting job ....................................................144
Deactivating the feature for all nesting jobs .......................................................................145
TUTORIAL 10 – UNFOLDING SHEET METAL COMPONENTS USING
„INTERACTIVE UNFOLD‟ COMMAND ...................................................................... 146
Introduction ...........................................................................................................................146
The „Interactive Unfold‟ Command ....................................................................................146
Difference between the various Unfold commands ............................................................146
Legend: ........................................................................................................................................ 146
The „Chain Faces‟ option for Unfold commands ................................................................147
STEP 1: Open the Assembly ................................................................................................147
STEP 2: Executing the „Interactive Unfold‟ command ........................................................148
STEP 3: Selective Unfolding of Parts when „Chain Faces‟ option is enabled...................149
Deselecting/ Selecting the faces to be unfolded ................................................................151
The following illustrations explain how to select/deselect faces to be unfolded. ....... 151
Illustration 1: ................................................................................................................................. 151
Illustration 2: ................................................................................................................................. 152
Illustration 3: ................................................................................................................................. 152
Changing the Reference Face ...........................................................................................154
Deselecting the Reference Face .................................................................................................. 154
Selecting a Reference Face ......................................................................................................... 155
STEP 4: Selective Unfolding of Parts when „Chain Faces‟ option is disabled ..................156
Disabling the Chain Faces option ......................................................................................156
vi
Table of Contents
CAMWorks Nesting Tutorial
Selecting faces to unfold when Chain Faces option is disabled .........................................157
Example: ...................................................................................................................................... 157
Changing Reference face when Chain Faces option is disabled .......................................158
Illustration: .................................................................................................................................... 158
TUTORIAL 11 – THE STAMP FEATURE UNFOLD OPTION ................................... 162
Introduction ...........................................................................................................................162
Assigning Stamp Feature Unfold Option settings in DefaultValues.ini ........................................ 162
Stamp Feature Unfold Option settings for Native parts & Imported Parts ................................... 163
Part 1:
Stamp Feature Unfold Options for Native Sheet Metal Parts ............................164
Step 1: Open the Part........................................................................................................164
Step 2: Executing the Unfold Command ............................................................................164
1.
The „Unfold All Parts‟ command
2.
The „Interactive Unfold‟ command
................................................................................ 164
3.
The „Create Nest Job‟ command
.................................................................................. 164
.................................................................................... 164
Step 3: Retaining the stamp feature ..................................................................................165
Step 4: Patching the stamp feature ...................................................................................165
Step 5: Ignoring the stamp feature ....................................................................................166
Step 6: Behaviour in native parts without bends ................................................................167
Part 2:
Stamp Feature Unfold Option for Imported Sheet Metal Parts ..........................168
Step 1: Open the Part........................................................................................................168
Step 2: Executing the Unfold Command ............................................................................168
1.
The „Intelligent Unfold‟ command
.................................................................................. 168
2.
The „Unfold All Parts‟ command
.................................................................................... 168
3.
The „Interactive Unfold‟ command
................................................................................ 168
4.
The „Create Nest Job‟ command
.................................................................................. 168
Step 3: Retaining the stamp feature ..................................................................................169
Step 4: Patching the stamp feature ...................................................................................169
Step 5: Ignoring the stamp feature ....................................................................................169
Step 6: Behaviour in imported parts without bends ............................................................170
TUTORIAL 12 – GENERATING NC CODES FOR NESTED LAYOUTS USING
CAMWORKS (I) .......................................................................................................... 172
How the Nested layouts generated are saved within SOLIDWORKS ................................172
Relation between CAMWorks Nesting and CAMWorks .....................................................172
Steps to generate NC codes for Nested layouts .................................................................173
Generating the nested layout assembly ..............................................................................174
Step 1: Define the Fixture Coordinates ...............................................................................175
Steps to set the Fixture Coordinates System .....................................................................175
Step 2: Define the Machine...................................................................................................176
Step 3: Addition of nested Parts to Part Manager ..............................................................177
Step 4: Define the Stock ......................................................................................................179
Table of Contents
vii
CAMWorks Nesting Tutorial
Step 5: Defining Machinable Features ................................................................................180
Extracting Machinable Feature using AFR ........................................................................180
Interactively Inserting Features .........................................................................................181
Step 6: Sorting Part Instances ............................................................................................182
Step 7: Generating the Operation Plan ...............................................................................184
Step 8: Adjusting Operation Parameters .............................................................................185
Step 9: Defining G-code Program Zero Location ................................................................187
Step 10: Generating Toolpaths and Sorting Operations ....................................................188
Step 11: Simulate Toolpaths ................................................................................................191
Step 12: Post Processing Toolpaths ...................................................................................192
TUTORIAL 13 – GENERATING NC CODES FOR NESTED LAYOUTS USING
CAMWORKS (II) ......................................................................................................... 195
Functionality to link CAMWorks Nesting with CAMWorks .................................................195
Pre-requisites for using this functionality ...........................................................................195
Advantages of this functionality .........................................................................................196
Enabling the functionality ..................................................................................................196
How the functionality works ...............................................................................................196
Automatic Definition of Stock in CAMWorks Stock Manager ....................................................... 197
Tutorial illustrating Generating of NC codes for Nested Layouts .....................................197
Section I: Generating Nested layouts ................................................................................198
Section II: Generating NC codes using CAMWorks ...........................................................200
Step 1: Defining the Fixture Coordinate System for the Machine ............................................... 200
Step 2: Defining the Machine ..................................................................................................... 201
Step 3: Verifying the Addition of Parts in the CAMWorks Part Manager .................................... 202
Step 4: Automatic Stock Definition .............................................................................................. 203
Step 5: Defining Machinable Features and Interactively Inserting Features ............................... 204
Step 6: Sorting Part Instances to Determine Machining Order .................................................... 208
Step 7: Generating the Operation Plan and Adjusting Operation Parameters ............................ 209
Step 8: Defining G-code Program Zero Location ......................................................................... 211
Step 9: Generating Toolpaths ..................................................................................................... 212
Step 10: Simulate Toolpaths ........................................................................................................ 213
Step 11: Generate the NC code ................................................................................................... 214
viii
Table of Contents
CAMWorks Nesting Tutorial
CAMWORKS NESTING: INTRODUCTION
What is CAMWorks Nesting?
CAMWorks Nesting, developed by Geometric Americas, Inc., is an
automatic, true-shape nesting program that easily creates fast and efficient
nested layouts. It is seamlessly integrated within SOLIDWORKS®/CAMWorks
Solids and allows nesting of flat or 3D solid or sheet metal parts and
assemblies.
CAMWorks Nesting can be used to create efficient layouts of metal, wood or
composite based materials, producing the maximum number of parts from a
single piece of raw material within minutes.
Procuring CAMWorks Nesting
Geometric Americas, Inc. sells CAMWorks Nesting and related program
modules through a worldwide network of Value Added Resellers.
 If you are an existing user of our other product named CAMWorks, you
can contact your Reseller for CAMWorks Nesting.
 If you are a first-time user of CAMWorks Nesting, you can find your
local CAMWorks Reseller on www.camworks.com
Note: CAMWorks Nesting can be purchased only through CAMWorks
Resellers. Though the CAMWorks Nesting installer can be downloaded
from the CAMWorks website, the license required to run the CAMWorks
Nesting application can be purchased only from an authorized Reseller.
Why CAMWorks Nesting should be your preferred
nesting program
CAMWorks Nesting has the following advantages that make it the ideal
choice when it comes to choosing the nesting application to suit your needs:
 Ease of Use: Parts imported from other CAD applications or created in
SOLIDWORKS as well as assemblies can be directly used as an input
without the need to convert them to flat patterns.
 Full Associativity with SOLIDWORKS: Updates are tracked and
flagged whenever the component is changed. Refresh rebuild the nest to
reflect the updated designs.
 SOLIDWORKS Compatible Output: Provides the nested output as a
new SOLIDWORKS assembly and retains the original part and assembly
model files. The SOLIDWORKS nested assembly can then be used for
further processing, such as toolpath and NC Code generation with
CAMWorks or any other CAM software, if required.
CAMWorks Nesting: Introduction
11
CAMWorks Nesting Tutorial





Part Requirements automatically assigned: Automatically nests
multiple parts, based on material and thickness, within an assembly in a
single run.
This feature helps users eliminate manual efforts in segregating individual
parts with the same material and thickness for a nesting operation.
Material Optimization: The advanced true-shape automatic nesting
algorithms reduce raw material consumption by providing optimized and
compact layouts.
Nesting with multiple tool heads: An optional feature to nest two or
more identical nesting layouts using multiple tool heads is provided. This
feature is useful for flame cutting applications.
Save Nested layout Output as DXF file: An optional feature that
allows users to save the nested layouts in the internationally accepted
CAD data file format known as „Drawing Exchange Format‟ (.dxf), in
addition to the existing assembly file format (.sldasm).
Unfold Imported Sheet Metal Bodies: Supports nesting of imported
sheet metal part models containing bends. Using this „Unfold Imported
Bodies‟ dialog box, such sheet metal parts can be unfolded before
executing the nesting job.
Receiving latest updates & Update Support Plan (USP)
Update Support Plan
Update Support Plan (USP): When you purchase CAMWorks Nesting
through a Reseller, you will receive a permanent license required to run the
CAMWorks Nesting application. In addition to this, you will also be enrolled
in a CAMWorks Nesting Update Support Plan (USP) for a specific duration.
Your Reseller will brief you about the USP when you purchase CAMWorks
Nesting.
Being enrolled in the CAMWorks Nesting Update Support Plan has the
following benefits:
 Receiving updates: It allows you to keep your CAMWorks Nesting
application up-to-date with the new features and performance
improvements of CAMWorks Nesting released in the form of Service
Packs.
 Technical Support: You receive technical support for all your queries
and doubts regarding CAMWorks Nesting.
Once your USP expires, you will no longer receive updates or support.
Ensure that you repurchase an appropriate Update Support Plan from your
CAMWorks Reseller to continue receiving technical support and updates.
12
CAMWorks Nesting: Introduction
CAMWorks Nesting Tutorial
Note: The CAMWorks Nesting license you purchase from your Reseller will be
perpetual in nature. However, the Update Support Plan has a fixed duration.
You need to repurchase an Update Support Plan after your current plan
expires.
Technical Support
This manual has been designed to be as informative as possible. In case you
still face problems related to installation, license activation or using CAMWorks
Nesting, you can write back to us at:
support@camworks.com
We will get back to you with the solution to your query within two working
days.
CAMWorks Nesting Installation & License Activation
A separate manual has been provided to acquaint you with the details of
installation and License activation for CAMWorks Nesting.
This manual is available on the CAMWorks website in the Downloads section
for CAMWorks Nesting-related downloads.
After you install CAMWorks Nesting, this manual can be accessed from
Start>>All Programs>>CAMWorksNesting 201x>>Installation & License Activation
Guide.
CAMWorks Nesting Tutorials
The last section of this manual contains illustrated tutorials which will help you
understand all the aspects of using CAMWorks Nesting for practical purposes.
Refer: CAMWorks Nesting Tutorials section.
CAMWorks Nesting: Introduction
13
CAMWorks Nesting Tutorial
ABOUT
THESE TUTORIALS
Section 1: The first section „Understanding the CAMWorks Nesting
Fundamentals‟ introduces the CAMWorks Nesting User Interface, working
environment and the various Nesting parameters.
Section 2: The second section „Initialization files of CAMWorks Nesting‟
explains how to use the initialization files present in CAMWorks Nesting to
define and edit default values, settings and populate the dropdown fields. It
is highly recommended that you read this section in order to gain an
understanding of how to customize the CAMWorks Nesting settings to meet
your facility‟s requirements.
Section 3: An understanding of these basic elements is required before
proceeding to the tutorials. The 12 tutorials given in this document will help
you to learn how to use CAMWorks Nesting through a step by step hands-on
tour of its features and functions. The tutorials are presented in order of
increasing complexity, each building upon the knowledge gained from the
previous tutorial.
Tutorial
14
Topic covered in the Tutorial
Tutorial 1 – Assembly Nesting
Nesting a Sheet Metal assembly.
Tutorial 2 – Single part, Single sheet Nesting
Nesting a Solid part.
Tutorial 3 – Single Part, Single sheet Nesting
Nesting a Sheet Metal Part.
Tutorial 4 – Nesting by Thickness
Nesting Parts of different thickness.
Tutorial 5 – Nest by material, Nest by
Thickness
Nesting Parts of different material &
thickness.
Tutorial 6 – Nesting with Multiple tool heads
Nesting Parts of identical material and
thickness intended to be machined
using a Machine with Multiple Tool
Heads.
Tutorial 7 – Nesting of Imported Sheet Metal
Parts
Nesting of Imported sheet metal parts
with bends.
Tutorial 8 – Nesting of Imported Sheet Metal
Parts with faulty surfaces
Nesting of Imported sheet metal parts.
Tutorial 9 – Assigning Assembly Quantities
Nesting an Assembly comprising subassemblies and parts.
About these Tutorials
CAMWorksNesting Tutorial
Tutorial
Topic covered in the Tutorial
Tutorial 10 – Unfolding Sheet Metal
Components Using „Interactive
Unfold‟ Command
Using „Interactive Unfold” command to
unfold sheet metal parts.
Tutorial 11 – The Stamp Feature Unfold
Option
Using „Stamp Feature Unfold‟
Command.
Tutorial 12 – Generating NC codes for Nested
layouts using CAMWorks (I)
Generating NC codes using
CAMWorks application for Nested
layouts.
Generating NC codes using
CAMWorks application for Nested
layouts using functionality to link
CAMWorks Nesting with CAMWorks.
Tutorial 13 – Generating NC codes for Nested
layouts using CAMWorks (II)
Additional information is available in the CAMWorks Nesting Context
Based Help. It is highly recommended that you read theses tutorials to gain
a deeper and practical understanding of CAMWorks Nesting features and
capabilities.
About these Tutorials
15
SECTION ONE
CAMWorks Nesting
Fundamentals
CAMWorks Nesting Tutorial
UNDERSTANDING THE CAMWORKS NESTING
FUNDAMENTALS
Basic Procedure of Nesting
Follow these general procedures to
generate nested layouts using CAMWorks
Nesting.
1. Open SOLIDWORKS/CAMWorks
CAMWorks
Solids. Click on the dropdown
Options icon
button of the CAMWorks Options
in the CAMWorks Menu Bar and select Add-Ins.
Selecting CAMWorks
Add-Ins
2. Load the CAMWorks Nesting Add-In.
Selecting the CAMWorksNesting Add-In
3. The CAMWorks Nesting Menu will be added to the
SOLIDWORKS/CAMWorks Solids menu bar.
CAMWorksNesting Menu added to CAMWorks Menu bar
4. For Single-part nesting:
a. Model or open a sheet metal part/ solid part model in
SOLIDWORKS. For example, open the part ‘Tutorial_1a’ located in
the following folder.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples/Tutorials\Assemblies\Tutorial1
b. Select Create Nesting Job from the CAMWorksNesting menu bar.
OR
Click on the Create Nest Job button on the CAMWorks Nesting
Ribbon Bar.
Understanding the CAMWorks Nesting Fundamentals
17
CAMWorks Nesting Tutorial
CAMWorks Nesting Ribbon
Bar
CAMWorksNesting Menu
c. The Create Nesting Job dialog box is displayed.
Part
Model
The CAMWorks Nesting „Create Nesting Job‟ dialog box
18
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
5. For Assembly Nesting:
a. Model or open a sheet metal/solid part/solid assembly in
SOLIDWORKS.
b. Select Create Nesting Job from the CAMWorksNesting menu bar.
c. The Create Nesting Job dialog box is displayed.
6. For Multi-part Nesting  Use Nest by Folder
a. If an assembly model is not available already and if the parts to be
nested are available in a folder then select Nest by Folder from the
CAMWorksNesting menu.
b. Browse to the folder containing the parts to be nested. Click OK.
c. The parts to be nested will be displayed in the SOLIDWORKS
Graphical User Interface.
d. The Create Nesting Job dialog box is displayed. All the parts are
listed under the Part Data tab of this dialog box along with the part
parameters.
7.
In all the three cases viz. Single Part Nesting, Assembly Nesting and
Multi-part Nesting, if the part or assembly contains an imported
sheet metal part with bends, then the Unfold Imported Bodies
dialog box will be displayed prior to the Create Nesting Job dialog
box. Use this dialog box to select the imported sheet metal parts to
be unfolded and to assign parameters related to unfolding. Once you
make the required selection and assign parameters, click OK. The
Create Nesting Job dialog box will be displayed.
8.
In the Create Nesting Job dialog box, under the Part Data tab, modify
or assign the Part controller parameters for the part(s) as required.
These parameters include thickness, material, grain direction,
quantity, Step angle, Normal Face Selection as required. These
parameters are discussed in detail in the section Part Parameters.
9.
Under the Sheet data tab, select the required sheet size(s). Modify or
assign the sheet parameters such as sheet name, sheet thickness,
sheet material, sheet quantity, grain direction, sheet length and
width. These parameters are discussed in detail in the section Sheet
Parameters.
10. If you wish to nest the part(s)/assembly using multiple tool heads,
use the Multi head options tab to assign the associated parameters
such as the machine name, number of tool heads, to be used, rail
direction, tool head distance and multi-tool head nesting type. These
parameters are discussed in detail in the section Multi Head
Options parameters.
11. In the Nesting Data group box:
a. Assign appropriate values to the parameters of Part-to-Part
distance and Part-to-Sheet distance.
Understanding the CAMWorks Nesting Fundamentals
19
CAMWorks Nesting Tutorial
b. Use the browse button
to assign a new location for the output
file rather than the default location given in the Output Assembly
File field.
c. CAMWorks Nesting always saves the nested layouts generated after
the execution of a nesting job in the assembly file format (.sldasm).
To optionally save the nested layouts in the .dxf format, check the
Save output as dxf checkbox. Use the browse button
to assign
the folder location where the .dxf files are to be saved.
d. Fast Nesting and Optimal Nesting indicate the two different sets of
algorithms used to implement Nesting. Select the option that best
suits your requirements. Time Constraint can be applied to Optimal
Nesting if required.
The parameters in the Nesting Data group box are discussed in
detail in the section Nesting Data Parameters.
12. After all the parameters are set, click OK to execute the Nesting Job.
This sets into motion the process to generate a nested layout.
Generating the layout might take some time depending on the
complexity of the part.
Two files will be generated during the nesting process, namely a text
file and an assembly file.
After the Nesting process is completed, CAMWorks Nesting will display
a message indicating the location of the text file containing the
summary of the Nest Results. Click OK to close the message. The
Text file will be displayed.
The Nested layout assembly will be displayed in the Graphics area.
Both these files are saved in the location indicated by Output Assembly
File path stated in the Apply Nesting dialog box.
Note: The assembly file format (.sldasm) is the standard file format in which the
nested layouts are generated. If the Save output as dxf option is used, then the
nested layouts will be generated in two file formats: .sldasm & .dxf and saved
in the specified folder locations.
Flowchart on Basic Procedure to Implement Nesting
A flow chart of the basic procedure to implement nesting using
CAMWorks Nesting is given on the next page.
20
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
START
Load CAMWorks Nesting
Add-In in SolidWorks
Multi-Part Nesting
Single Part Nesting
Open the Part to be nested
The ‘Unfold Imported Bodies’
dialog is displayed
Select the bodies to be
unfolded and modify
associated parameters
Yes
Open the Assembly to be nested
Select the ‘Nest by folder’ menu
option
Select the ‘Create Nesting Job’
menu option
Browse to open the folder
containing the parts to be nested
Do Parts to
be nested include
imported sheet
metal bodies with
Bends?
No
The ‘Create Nesting Job’ dialog is displayed
Assign/ Modify part parameters of each part to be nested
Assign/Modify sheet parameters
of each sheet used for nesting
Multi-tool
nesting
Assign/ modify parameters
for nesting with multiple tools
Assign/Modify Nesting parameters
Execute Nesting Job
Nested Layout generated. Save Output file.
END
Steps to generate Nesting Layout in CAMWorks Nesting
Understanding the CAMWorks Nesting Fundamentals
21
CAMWorks Nesting Tutorial
The Part Model/Assembly
In CAMWorks Nesting, your part model is a solid created with SOLIDWORKS
or imported into SOLIDWORKS from another CAD system via an IGES, STEP,
Parasolid, SAT or other neutral translators. A part can contain multiple
bodies.
Similarly, an assembly is a group of parts created with SOLIDWORKS or
imported into SOLIDWORKS from another CAD system. An assembly can
contain multi-body parts. Assemblies with parts having multiple
configurations are supported.
The tutorials in this manual use existing SOLIDWORKS Parts installed with
CAMWorks Nesting.
For example, open the assembly Tutorial_1.sldasm located in the following
folder of your CAMWorks Nesting installation folder.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial1
Select Create Nesting Job from the CAMWorksNesting menu.
The CAMWorks Nesting Graphical User Interface
Create Nesting Job
Dialog Model
22
Part Model
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Defining Part Parameters
The Create Nesting Job dialog box is used to set the part, sheet and nesting
parameters for Single Part nesting as well as Multi-Part nesting.
The Part data Tab
Use the Part Data tab of the Create Nesting Job dialog box to view and edit
the part related parameters.
The Part Data tab is the default tab displayed when the Create Nesting Job
dialog box is displayed.
The below data fields are available and can be edited in the Part Data tab:
 Part List
 Thickness
 Material
 Rotation Angle
 Grain Direction
 Normal Face Selection
 Quantity
Part name and
parameters of the
part to be nested
are displayed in
Part List
The
preview
of the
part to be
nested is
displayed
here
The Part Data Tab
Part List
The part parameters of Part name, Thickness, Quantity, Material, Rotation
Type, Rotation Angle, Grain direction are displayed in the Part List. The Part
Understanding the CAMWorks Nesting Fundamentals
23
CAMWorks Nesting Tutorial
parameters of thickness and material are extracted from the solid model
part and displayed in the Part List.
All the above parameters except the Part name can be edited directly in the
Part List. Alternatively, use the various Part parameter fields given below the
Part List grid to edit the parameters.
To edit the part parameter fields, highlight the part to be edited in the part
list and double-click on the required field. Edit the values as required.
Thickness
CAMWorks Nesting extracts
the part parameter of
Thickness from the Solid Part
and displays it in the
Thickness field as default
thickness for the part.
To assign a desired thickness,
enter the thickness value in
the Thickness field.
The Thickness field in the Part
List as well as Thickness field
below the Part List grid can be
used to edit the value.
Assigning thickness value to a part
Material
CAMWorks Nesting extracts Material related information from the solid part
in the SOLIDWORKS environment and displays it in the „Material‟ field as
default material for
the part.
If the material value is
not extracted from the
3D model then,
CAMWorks Nesting
assigns a default
value. This default
value will be the first
material listed in the
material dropdown
list.
To assign a material
from the material
dropdown list, select
the desired material
24
Assigning Material from dropdown list in Material Column
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
from the dropdown list in the material column of the Part list. Alternatively,
use the Material dropdown list given below the Part List grid.
A user-defined
material (a
material which
is not part of
the material
dropdown list)
can also be
assigned to a
part.
However,
such a userdefined
Enter user-defined material name in the field given below the Part list.
material
It will then update the Material Column of Part List
cannot be
assigned to a part using the Part List.
To assign a user defined material, following are the steps:
a) Select the Part (for which material is to be changed) in the Part List.
b) Enter the Material name into the Material combo box given below the
Part List.
c) Shift the focus from this field by pressing the tab button. Observe that
the new material assigned is reflected the Part List.
Note: You must customize the material dropdown list to populate it with the materials
used at your facility. For details, read: Viewing/ Editing the Material dropdown list.
Rotation Angle
CAMWorks Nesting provides two options for applying the rotation control for
a part:
Step Angle:
Angle List:
This is the angle that specifies the step in which the part is
tried for nesting.
For example, if the Step angle provided for the part is 90
degrees, then that part will be tried in 90, 180, 270 and
360 degrees. The default step angle is 10.
If step angle is 150, then nesting of the part will be tried in
15, 30, 45, 60, 75, 90, 105, 120, 135, 150, 165 …… up to
360 degrees.
This is the second way in which the rotation control can be
applied on a part. The set of angles need to be input in a
list. CAMWorks Nesting will then try nesting the parts only
for the specified set of angles. To specify an Angle List in
Understanding the CAMWorks Nesting Fundamentals
25
CAMWorks Nesting Tutorial
the Create Nesting Job dialog box, separate the angles by
a comma. For example, to specify angles of 10, 20, 30, 60
and 90 degrees, you must enter '10, 20, 30, 60, 90' in the
Part Angle List field.
The Rotation type and the subsequent Part angle can be set in the Part List.
Alternatively, you can highlight the part(s) in Part List for which this
parameter is to be changed. Then change the Rotation Type and part angle
for the highlighted part in the Rotation Angle group box below the Part list
grid.
Change the
parameters
directly in the
Part List
Change the
parameters for the
selected part here
Assigning Rotation angle to the part
Grain Direction
To ensure accuracy and avoid defects during the subsequent mechanical
operations like bending, it is necessary to cut critical parts, such that they
have pre-defined and proper grain direction.
The Grain direction field is a drop down list from which you must choose any
one option. The options are:



X direction
Y direction
None (default option for both part and sheet)
The Grain Direction for a part can be set directly in the Part list.
Alternatively, you can highlight the part(s) in Part list for which this
parameter is to be changed. Then change the Grain direction for the
highlighted part using the Grain direction dropdown list below the Part list
grid.
26
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Assigning the grain direction for the part to be nested
Normal Face
The Normal Face selection is used to select the part face to be used as a
normal plane for generating silhouette profile of the part to be nested.
By default, CAMWorks Nesting uses the part face with the maximum number
of features as a normal plane to generate a silhouette profile. However, for
certain solid/imported parts, a need may arise to select another face of the
part for various reasons such as ease of machining, single setup machining
etc. For such situations, CAMWorks Nesting provides the option to manually
define the Normal face.
The Normal Face selection cannot be executed in the Part List grid.
To change the Normal face direction of a part:



Highlight the required part in the Part List grid.
The sheet metal/solid part to be nested is highlighted in the Graphical
User Interface of SOLIDWORKS. In this interface, click on the face of
the part that you wish to assign as the normal face.
The Normal face field will now list the selected face.

Click
to reverse the normal direction.
Understanding the CAMWorks Nesting Fundamentals
27
CAMWorks Nesting Tutorial
Highlight the
part for which
normal face is to
be changed
Flip to reverse the
normal direction
Normal Face Selection
Quantity
The Part Quantity field indicates the number of instances of the part to be
nested. CAMWorks Nesting assigns a default quantity to all parts listed in the
Part List.
Use the Quantity field to assign the number of instances of the part to be
nested.
The quantity for a part can be set directly in the Part List.
Alternatively, you can highlight the part(s) in Part List for which this
parameter is to be changed. Then change the quantity for the highlighted
part using the Quantity field below the Part list grid. You can use spin control
to increase or decrease the Quantity value. Spin control increases the value
in steps of +1 and decreases it in steps of -1.
Note:
For assemblies, default quantity assigned for a part is equal to the number of instances
of the part in the assembly. For single part nesting, the default value assigned is based
on the value defined in the DefaultValues.ini file. You can edit the default Quantity to be
assigned for parts. For details, read: Defining default Part quantity.
28
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Assigning Quantity to the parts to be nested
Note: If the feature for assigning assembly quantities is enabled, then the Quantity
column will also display values in the Quantity column for the assembly to be
nested as well as its constituent sub-assemblies, if any. Editing the quantity of
the assembly or its constituent sub-assemblies updates the quantity of its
constituent parts automatically. For more detail, refer: Tutorial 9
Defining Sheet Parameters
The Create Nesting Job dialog box is used to set the part, sheet and nesting
parameters for Single Part nesting as well as Multi-Part nesting.
The Sheet data Tab
Use the Sheet Data tab of the Create Nesting Job dialog box to add sheet(s)
and set the parameters for sheet(s) in which parts will be nested.
The Part Data tab is the default tab displayed when the Create Nesting Job
dialog box is displayed. Click on the Sheet Data tab to view Sheet related
data fields.
The below data fields are available and can be edited in the Sheet Data tab:








Sheet List
Thickness
Material
Quantity
Grain Direction
Sheet Size
Length
Width
Understanding the CAMWorks Nesting Fundamentals
29
CAMWorks Nesting Tutorial
Sheet Data tab of „Create Nesting Job‟ dialog box
Sheet List
The Sheet List is populated by adding sheets using the Add Sheet button.
Parts defined in the Part Data tab will be nested only on the sheet(s)
listed in the Sheet List.
The sheet parameters of Sheet name, Length, Width, Thickness, Quantity,
Material and Grain direction are displayed in the Sheet List.
Of these parameters, Thickness, Quantity, Material and Grain direction
parameters can be edited directly in the Sheet List grid after insertion. This
is true for all sheet sizes. The parameters of Sheet Name, Length and Width
can be edited only for Sheet of type Custom Size.
To edit the sheet parameter fields, highlight the sheet to be edited in the
Sheet List and double-click on the required field to edit the values.
Thickness
Some intelligence is added in CAMWorks Nesting such that it ensures all
sheets with relevant materials and thicknesses are available for nesting
all the parts in the assembly. CAMWorks Nesting automatically extracts the
thickness and material of the first part in the part list and assigns these as
the default value of the first sheet. CAMWorks Nesting automatically checks
for different material and thickness if any in the part list and assigns these
as the default value of the second sheet and so on till all required sheets
with relevant material and thickness are added.
For a sheet inserted in the Sheet List, the thickness field displays the sheet‟s
thickness.
30
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Use the thickness field given below the sheet list to set the thickness value
before adding the sheet to the Sheet List. Once the sheet is added to the
Sheet List, the thickness value can be edited directly within the Sheet List in
the respective field.
Material
For a sheet inserted in the Sheet list grid, the Material field displays the
material the sheet is made of.
Use the Material field given below the sheet list to set the Material type
before adding the sheet to the Sheet List. Once the sheet is added to the
Sheet List, the material type can be edited directly within the Sheet List in
the respective field.
Quantity
The Quantity field indicates the number of sheets available. Use the Quantity
field given below the sheet list to set the Quantity value before adding the
sheet to the Sheet List. Once the sheet is added to the Sheet List, the
Quantity field can be edited directly within the Sheet List in the respective
field.
The default quantity assigned is based on the value defined in the
DefaultValues.ini file. You can edit the default Quantity to be assigned for
sheets. For details, read: Defining default Sheet Quantity.
Grain Direction
Grain direction can be set for a sheet just like it is set for parts. This field is
a drop down list from which you must choose an option. The options are:



X direction
Y direction
None (default option for both part and sheet)
Use the Grain Direction field given below the sheet list to set the Grain
Direction before adding the sheet to the Sheet List. Once the sheet is added
to the Sheet List, the Grain Direction field can be edited directly within the
Sheet List in the respective field.
Assigning Grain directions
The Grain Direction which you can assign to a particular sheet is dependent
on the Grain Direction of the Parts which will be nested within that sheet.
The allowed relationship between the Grain Direction of the part(s) and
sheet is given in the following table:
Understanding the CAMWorks Nesting Fundamentals
31
CAMWorks Nesting Tutorial
Grain Direction
of Part
Allowed Grain
Direction for Sheet
Description
X or Y but not None
If a part has grain direction “X”, then at
least one of its corresponding sheets
should have either “X” or “Y” but not “None”
as its grain.
Y
X or Y but not None
If a part has grain direction “Y”, then at
least one of its corresponding sheets
should have either “X” or “Y” but not “None”
as its grain.
None
X or Y or None
If a part has grain direction “None”, then the
corresponding sheets can have either “X”
or “Y” or “None” as its grain direction.
X
Add Sheet & Remove Sheet buttons
Use the Add Sheet button to add a sheet to the Sheet List after setting its
parameters.
To remove a sheet from the Sheet List, select the sheet to be deleted in the
Sheet List and click Remove Sheet.
Sheet Size
The Sheet List grid will initially be empty when you click on the Sheet Data
tab of the Create Nesting Job dialog box. The size of the sheet in which the
part(s) will be nested needs to be defined and then added to the Sheet List.
CAMWorks Nesting provides three options with respect to sheet size:
Standard Size: The Standard Size dropdown box lists all the standard sheet
sizes listed in the StandardSheets.ini file. This option is best
exercised if you have defined the standard sheet sizes used
at your facility in the StandardSheets-INCH.ini or
StandardSheets-MM.ini file.
32
Custom Size:
The Custom Size option is best used when adding a nonstandard size rectangular sheet or adding a custom sheet
size.
The default dimensions (length and breadth) for the
Custom sheet can be defined in the DefaultValues.ini file.
These default values will be displayed in the Sheet Data tab
when you select the Custom Size option to execute a new
nesting job.
Sheet DXF:
Only rectangular sheets can be defined using Standard Size
and Custom Size. The Sheet DXF option is best used when
you want to use a non- rectangular sheet or remnant sheet.
In order to nest parts using such a non-rectangular or
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
remnant sheet, the sheet should be saved in CAD graphic
image file format called Drawing Exchange format (.dxf).
Defining Standard Sheet
To add a standard size sheet, following are the steps:

In the Sheet data tab, the row indicating Select to add sheet in the
Sheet list would have been selected by default, if it is not selected
then click on the row indicating Select to add sheet in the Sheet list.

To define the sheet size, select the option Standard Size.

In the Standard Size dropdown list, select the required sheet size.

Set the parameters of thickness, quantity, material and grain
direction as required.

Click on the Add Sheet button.

The sheet is now added to the sheet list.
Standard Sheet is added to
Sheet List after executing
‘Add Sheet’
Select the Standard size
from the dropdown list.
Adding Standard Size Sheet to Sheet List
Understanding the CAMWorks Nesting Fundamentals
33
CAMWorks Nesting Tutorial
Defining Custom Size Sheet
To define a Custom size sheet, following are the steps:

In the Sheet data tab, the row indicating Select to add sheet in the
Sheet list would have been selected by default, if it is not selected
then click on the row indicating Select to add sheet in the Sheet list.

In the Sheet data tab, select the option Custom Size.

The Length and Width fields are activated on selecting this
option. Default values are displayed in these fields. (These values
are defined in the DefaultValues.ini file.) Edit the Length and Width
fields to assign the required values. You can use spin control to
increase or decrease the Length and Width values.

Set Thickness, Material and Grain Direction values.

Set the Quantity of the Sheet.

Click on the Add Sheet button.

The sheet is now added to the sheet list.
The preview of the sheet
highlighted in the Sheet
List is displayed here
Adding Custom Size Sheet to Sheet List
Defining Sheet DXF
To use a sheet saved in DXF (Drawing Exchange Format) file format,


34
In the Sheet data tab, the row indicating Select to add sheet in the
Sheet list would have been selected by default, if it is not selected
then click on the row indicating Select to add sheet in the Sheet list.
In the Sheet data tab, select the option Sheet DXF.
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial





Click on the
button to browse to the folder location where the
.DXF file is located.
Set Thickness, Material and Grain Direction values.
Click on the Add Sheet button.
The Sheet saved in .dxf format will be added to the sheet list.
A thumbnail view of the shape of the sheet will be displayed in the
Sheet Preview.
The preview of the Sheet
DXF added to sheet list is
displayed here
Adding a Sheet stored in .dxf file format
Note: After a sheet is added to the Sheet list, its parameters can be edited either in
Sheet List grid or in the respective fields below the Sheet list grid similar to
part data editing.
Defining Multi Head Options Parameters
The Create Nesting Job dialog box is used to set the part, sheet and nesting
parameters for Single Part nesting as well as Multi-Part nesting.
For flame cutting applications, CAMWorks Nesting provides an optional
functionality known as Multiple Tool Head Nesting. This functionality allows you
to nest two or more identical layouts simultaneously using multiple tool heads.
Machines which support nesting using multiple tool heads are known as Multi
tool head machines.
The tab named Multi head options in the Create Nesting Job dialog box allows
you to define/edit parameters related to nesting with multiple tool heads.
Understanding the CAMWorks Nesting Fundamentals
35
CAMWorks Nesting Tutorial
How the functionality of nesting with multiple tool heads
works
When nesting layout(s) are to be generated using multiple tool heads,
CAMWorks Nesting will first attempt to nest the parts using the userspecified number of tool heads. Suppose this tool heads number is „n‟. If a
best-fit layout is achievable, CAMWorks Nesting will generate „n‟ identical
nesting layouts on the sheet.
If a best-fit nesting layout is not achievable with this number, then
CAMWorks Nesting will try to nest using „n-1‟ number of tool heads. If this
number too fails, then it will try to nest using „n-2‟ tool heads and so on until
finally nesting with a single tool head.
The Default Settings in the Multi Head Options tab
Click on the Multi Head Options tab of the Create Nesting Job dialog box.
The Multi Head Options tab (as typically seen with default settings)
Observe the Machine Data group box. The default machine displayed in the
Machine field is SingleTHMachine. The Number of tool heads for this machine
is „1‟.
SingleTHMachine (Single Tool Head Machine)
SingleTHMachine is representative of machines with a single tool head. Such
machines are usually used for the nesting process. When this machine is
selected in the Multi Head Options tab, the functionality of nesting with
multiple tool heads will be disabled for the current nesting job. All the
parameters fields related to Multiple Tool Head Nesting in the tab are
disabled, indicating that Multiple Tool Head Nesting functionality is disabled.
36
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Enabling Multi Tool Head Machining
To generate nested layouts using a machine with multiple tool heads instead
of the default Single Tool Head machine, you need to select a machine with
multiple tool heads in the Machine field of the Multi Head Options tab.
For nesting with Multiple Tool Heads, select a machine other than
SingleTHMachine in the Machine dropdown list. The number of tool heads
possessed by the selected machine is listed in the Number of tool heads
field. If the machine has two or more tool heads, nesting with Multiple Tool
Heads will be enabled for the current nesting job.
The Multi Head Options tab (as typically displayed when Multiple Tool Head Nesting is active)
Parameters and Data fields in the Multi Head Options tab
This tab provides an interactive interface to view/edit the parameters related
to nesting with multiple tool heads. The following data fields are available in
the Multi head options tab:
 Sheet List
 Machine name
 Number of Tool Heads
 Multi-tool nesting type option
 Rail Direction
 Tool head distance
Understanding the CAMWorks Nesting Fundamentals
37
CAMWorks Nesting Tutorial
Multi head options tab in the Create Nesting Job dialog box
Sheet List
The Sheet List is populated by the sheets listed in the Sheet data tab of
the Create Nesting Job dialog box. Unlike the Sheet List grid in the Sheet
Data tab, this grid is read-only. For nesting with multiple tool heads, a
separate set of parameters needs to be defined for each individual sheet
listed in the Sheet List.
To define these parameters, highlight the desired sheet in the Sheet List.
The default values of these parameters will be displayed below the Sheet List
grid in their corresponding fields. Proceed to edit the parameters as desired.
Machine (machine name)
The default machine displayed in the Machine
field is the SingleTHMachine. When this
machine (representative of Single Tool Head
Machines) is selected, nesting with multiple
tool heads is disabled. All the other parameter
fields in the Multi Head Options tab which are
related to Multiple Tool Head Nesting will be
disabled.
Machine data dropdown list
All the other machines listed in the Machine dropdown list support Nesting
with Multiple Tool Heads. To enable nesting with multiple tool heads, select
the desired machine (other than SingleTHMachine) from the dropdown list.
When such a machine is selected, the default parameter values associated
with that machine are displayed in the Multi head options tab. These default
parameter values for each machine are defined in the Machine.ini file.
The Machine dropdown list is populated with the Machine names listed in the
Machine.ini file. Before executing a nesting job using multiple tool heads,
38
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
ensure that you customize the Machine.ini file to suit your nesting job
requirements.
Number of Tool Heads
For every machine listed in the Machine
dropdown list, the maximum number of
permissible tool heads is defined in the
Machine.ini file. When you select a particular
machine from the Machine dropdown list, the
maximum permissible number of tool heads
for that machine is displayed in the Number
of tool heads dropdown list.
Number of tool heads dropdown list
Based on your nesting requirements, you have the option of choosing any
number ranging from 1 to this maximum number from the Number of tool
heads dropdown list.
Multi-tool head nesting type
You can choose any one of the following
Multi-tool head nesting type option:
a. Fixed tool head distance:
When this option is chosen, the
distance between the tool heads
is fixed to the minimum tool
head distance.
Selection the multi-tool head nesting type
option
b. Variable tool head distance: When this option is chosen, the
distance between tool heads can vary but will be greater than the
minimum tool head distance.
When you select a particular machine from the Machine dropdown list, the
default Multi-tool head nesting type option for that machine is displayed in
the Multi Head Options tab. This default option is assigned in the Machine.ini
file. You can change this default option to suit your nesting job
requirements.
Rail direction
Rail direction is defined as the direction the master tool head follows while
cutting. It can be either horizontal (X) or vertical (Y). When the rail direction
is horizontal, the slave tool heads are either to the top or to the bottom of
the master tool head. When the rail direction is vertical, slave tool heads lie
either to the left or to the right of the master tool head.
The tool heads are arranged along the height of the sheet when the rail
direction is „X‟ and along the length of the sheet if the rail direction is „Y‟.
When you select a particular machine from the Machine dropdown list, the
default Rail direction for that particular machine is displayed with the Multi
head options tab. This default value is defined in the Machine.ini file. You
can change the Rail direction to suit your nesting job requirements.
Understanding the CAMWorks Nesting Fundamentals
39
CAMWorks Nesting Tutorial
Tool head distance
The Tool head distance value indicates minimum tool head distance to be
used for a nesting job involving multiple tool heads.
When you select a particular machine from the Machine dropdown list, the
default Tool head distance value for that particular machine is displayed with
the Multi head options tab. This default value is defined in the Machine.ini
file.
Editing the default settings for the Multi Head Options tab
The nesting specific information and default parameter values for machines
which support nesting with multiple tool heads is defined in the Machine.ini
file located in the \CAMWorksNestingData\CAMWorksNesting
201x\Lang\English folder.
If you intend to make use of the feature of nesting with multiple tool heads,
then the Machine.ini file can be customized depending on your requirements.
For a detailed understanding of how to customize this file, read the section
on Machine.ini.
Define Nesting Data Parameters
The Nesting Data group box in the bottom area of the Create Nesting Job dialog
box is used to set the following nesting parameters:
40

Part to Part Distance

Part to Sheet Distance

Output Assembly File path

Assembly template path

Save output as dxf

„Automatically Select Sheet‟ option

„Create separate assembly‟ option

Nesting Type

Nesting Time (in minutes)
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
Defining Nesting Parameter values
Part to Part Distance
The Part to Part Distance indicates the distance to be maintained between
two nested parts in the sheet. The default value is „0‟. Assign the required
value by entering it in the field.
Part to Sheet Distance
The Part to Sheet Distance indicates the distance to be maintained between
a part and the edge of the sheet. The default value is zero. Assign the
required value by entering it in the field.
Output Assembly file
The folder location specified in the field Output Assembly File indicates the
location where the generated Assembly of nested parts will be saved. The
default location is always the same folder location as the part(s)/assembly to
be nested. Click on the
button to select an alternate location to save the
Assembly file(s) that will generated after the successful execution of a
nesting job.
Understanding the CAMWorks Nesting Fundamentals
41
CAMWorks Nesting Tutorial
Assembly Template Path
An assembly templates (*.asmdot) is a template document that includes
user-defined parameters and customized options which forms the basis for
new assemblies.
Use the
button given next to the Assembly template field to browse to
the location where the desired assembly template is saved. In CAMWorks
Nesting, the default assembly template loaded is the one defined in the
Default Templates section of the SOLIDWORKS Systems Options.
Save output as dxf
The CAD data file format called Drawing Exchange format (.dxf) is an
international standard which enables data interoperability between AutoCAD
and other programs.
The Save output as dxf checkbox option is a feature which allows you to
save the nested layouts which are generated after executing a nesting job in
the .dxf format.
Use the
button given next to this field to browse to the folder location
where the .dxf files are to be saved. This field which is used to specify the
folder location is enabled only when the Save output as dxf checkbox is
checked.
If the Save output as dxf option is used when multiple nested layouts are
generated (saved either as separate configurations or as separate assembly
files), then a separate .dxf file will be created for each nested layout that is
output and saved in the specified folder location.
When the Save output as dxf checkbox is not checked, then the nested
layouts generated after executing a nesting job will be saved only in the
assembly file format (.sldasm).
Note: The assembly file format (.sldasm) is the standard file format in which the nested
layouts are generated. If the Save output as dxf option is used, then the nested
layouts will be generated in two file formats: .sldasm & .dxf and saved in the
specified folder locations.
Automatically Select Sheet
For a nesting job containing multiple parts and sheet types, it is difficult for
the user to select the best sheet type or best sequence of sheets in order to
obtain best yield based on the sheet utilization factor. Since it is very
important to predict and procure the inventory in correct numbers, an
Inventory Forecasting Module (IFM) which forecasts the optimum sheet
inventory is necessary.
The Inventory Forecasting Module operates within CAMWorks Nesting in the
form of Automatically Select Sheet option.
Automatic Sheet Selection supports two methods:
42
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
1. Unique Sheet Forecaster
If this method is selected, the feature would select one best sheet among
the set of sheets considered, depending upon overall utilization obtained.
After knowing which sheet type is the best for that particular nesting order,
the user can place an order for that much quantity of the sheet type. This
will help in reducing the sheet variety – thus reducing the time required for
machine specific sheet settings.
2. Combinatorial Sheet Forecaster
If this method is selected, the feature selects a combination of sheet types
from the set of sheets available in the Sheet list, depending on the overall
utilization obtained.
Setting the Forecaster Method in DefaultValues.ini
At any given point of time, only one of the above mentioned Forecasting
methods can be used. This setting is available in the DefaultValues.ini file.
The default method is Combinatorial Sheet Forecaster.
Create Separate Assembly
The Create separate assembly option is available under the Nesting Data
group box in the Create Nesting Job dialog box.
When multiple nesting layouts are generated after the execution of a nesting
job, CAMWorks Nesting lists all the nested layouts under the Configurations
Manager Tab of SOLIDWORKS. These nested layouts are saved as a part of a
single assembly file (*.sldasm).
If you wish to generate separate assemblies for each such nested layout
generated, the select the Create Separate Assembly option. After executing
a nesting job, all the nested layouts will then be saved as separate
assemblies in the destination folder specified in the Output Assembly file
location.
Nesting Type
Fast Nesting and Optimal Nesting indicate the two different sets of
algorithms used to implement Nesting.
Fast Nesting: This method should be used when nesting quickly is more
important than optimal sheet utilization.
Optimal Nesting: This method focuses on optimal utilization of the sheet
by running multiple algorithms and chooses the best result in terms of
utilization. It is the default setting for CAMWorks Nesting.
Max Nesting time
Time constraints can be applied to optimal nesting. The Max. nesting time
field is enabled when the Nesting type is set to Optimal Nesting. Use this
field to enter nesting time limit in minutes. This will restrict the maximum
Understanding the CAMWorks Nesting Fundamentals
43
CAMWorks Nesting Tutorial
allowable time for nesting to the set value. The default value for max nesting
time field is No constraint, which indicates that a full optimal nesting will be
run without any time constraints.
Note: Optimal Nesting option is not available for a nesting job that uses multiple tool
heads. In other words, the Optimal Nesting option is disabled when the
functionality of nesting with multiple tool heads is enabled.
Generating the Nested Layout
After setting the part, sheet and nesting parameters, click OK.
This sets into motion the process to generate a nested layout. Generating
the layout might take some time depending on the complexity of the part.
Two files will be generated during the nesting process, namely a text file and
an assembly file.
After the Nesting process is completed, CAMWorks Nesting will display a
message indicating the location of the text file containing the summary of
the Nest Results. Click OK to close the message. The Text file will be
displayed.
The Nested layout assembly will be displayed in the Graphics area. Both
these files are saved in the location indicated Output Assembly file path
stated in the Apply Nesting dialog box.
How the Nested layouts generated are saved within
SOLIDWORKS
Once the nesting process using the CAMWorks Nesting application is completed,
the nested layout(s) generated will always be saved as a SOLIDWORKS
assembly file (*.sldasm). Depending on various factors such as thickness and/or
material part of part, number of sheets, grain direction, etc., either one or
multiple Nested layouts will be generated.
 When only one nested layout is generated:
o The will be saved as a SOLIDWORKS Assembly file comprising of nested
parts.
o The sheet dimensions will be saved as a SOLIDWORKS sketch.
 When multiple nested layouts are generated:
o These nested layouts will be saved as a SOLIDWORKS Assembly file
comprising of assemblies. Each assembly is a nested layout comprising of
nested parts.
o The sheet dimensions for each sheet will be saved as a SOLIDWORKS
sketch.
Once the nested layout(s) are generated, each nested layout assembly (sheet
layout containing nested parts) will be listed in the SOLIDWORKS Configurations
Manager.
44
Understanding the CAMWorks Nesting Fundamentals
CAMWorks Nesting Tutorial
TUTORIAL 1 - NESTING AN ASSEMBLY
This tutorial is intended to give you a preview of how nesting is done for a simple
assembly file comprising sheet metal parts. The sheet metal parts will be nested
using a single tool head.
Generating a nested layout as explained in this tutorial will help you understand
better the concepts explained in the next section: Initialization Files of CAMWorks
Nesting.
Step 1: Open the Assembly
1.
Load the CAMWorks Nesting Add-In in SOLIDWORKS.
2.
Open the assembly file Tutorial_1.sldasm located in the
...\CAMWorksNestingData\Examples\Tutorials\Assemblies\Tutorial1 folder
of your CAMWorks Nesting installation folder. (Refer page 19)
Step 2: Assign Nesting Parameters
1.
Select Create Nesting Job from the CAMWorksNesting menu bar.
OR
Click on the Create Nest Job button on the CAMWorks Nesting Ribbon Bar.
2.
The Create Nesting Job dialog box is displayed. Click on the Multi Head
Options tab and ensure that SingleTHMachine is the machine listed in the
Machine field.
Part Data Tab
1.
Click on Part Data tab. The solid parts Tutorial_1a.sldprt and
Tutorial_1b.sldprt which comprise the assembly are listed in the Part List
along with their part parameters.
2.
In the Quantity column of the Part List, set the quantity of
Tutorial_1a.sldprt to 25 and the quantity of Tutorial_1b.sldprt to 38.Leave
all other default part parameter settings as it is. (Refer page 25)
3.
Assign a Step Angle of 90 degrees to both the parts Tutorial_1a.sldprt and
Tutorial_1b.sldprt.
Sheet Data Tab
1.
Click on the Sheet Data tab. Observe that the thickness and material
fields display values identical to those of the first part in the part list.
2.
To add a sheet, following are the steps:
a. Select Custom Size. The Length and Width fields will be activated and
will display default values as defined in the DefaultValues.ini file.
Tutorial 1 - Nesting an Assembly
45
CAMWorks Nesting Tutorial
b. Assign a length of 1200mm and a width of 1200 mm. Set the
sheet Quantity to „1‟.
c. Click Add Sheet to add the sheet to the Sheet List. (Refer page 31)
Nesting Parameters
1.
In the Nesting Parameters group box, set a Part to Part distance of 2 mm is
set and a Part to Sheet distance of 3mm.
2.
Click on the
button to select the location to save the output Assembly
file and Summary text file.
3.
Set the Nesting method to Optimal nesting.
4.
Click OK to execute the Nesting Process.
Step 3: Generating the Nested Layout
Summary Text
The Summary text file indicates that the prescribed quantities for all the
parts have been nested within the sheet. This summary text file is saved in
the same location as the assembly that was nested.
This nested assembly will be saved with the prefix ‘NestAssm-’ and suffix
‘.ResultsSummary’ added to the name of the assembly file that was nested.
Nesting Results Summary Text File
46
Tutorial 1 – Nesting an Assembly
CAMWorks Nesting Tutorial
Nested Assembly
The nested layout assembly generated after executing the nesting job and
the Summary Results file are stored in the same location as the assembly
file that was nested. This nested assembly will be saved with the prefix
‘NestAssm-’ added to the name of the assembly file that was nested.
The resultant nested layout is given on the next page.
Nested Layout of Assembly achieved with Fast Nesting
47
SECTION TWO
Initialization
Files
CAMWorks Nesting Tutorial
INITIALIZATION FILES OF CAMWORKS NESTING
CAMWorks Nesting provides the facility to define and edit default values,
settings and populate the dropdown fields.
These values can be defined, set or edited in the initialization files (files with
.ini extension) present in the CAMWorks Nesting installation folder.
Location of the CAMWorks Nesting Initialization files
All these initialization files are located in the CAMWorks Nesting installation
folder. A typical installation path will be:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Lang\English
Backing up the Initialization Files
Every time you install a fresh version or Service Pack of CAMWorks Nesting,
the initialization files will be overwritten. Hence, if you have customized the
settings in the various initialization files, we recommend that you take a
back-up of the initialization files before installing a fresh version of
CAMWorks Nesting.
Configuration settings available in Initialization files
Following are the various settings that can be controlled from the CAMWorks
Nesting Initialization files.
Setting
Initialization File
Define and store information on the standard
sheet sizes
StandardSheets-INCH.ini
StandardSheets-MM.ini
Populating the Materials dropdown list
Materials.ini
Defining default part quantity
DefaultValues.ini
Defining default sheet thickness and material
DefaultValues.ini
/
Defining default dimensions for Custom sheet DefaultValues.ini
Defining default values for Part to part
distance and Part to sheet distance
DefaultValues.ini
Enabling/disabling the option of Preferential
hole filling
DefaultValues.ini
Initialization Files of CAMWorks Nesting
49
CAMWorks Nesting Tutorial
Defining the default state of the Create
Separate Assembly option
DefaultValues.ini
Defining the default state of the
Automatically Select Sheet option
DefaultValues.ini
Defining default state of the ‘Save output as
dxf’ option
DefaultValues.ini
Enabling/disabling the functionality to link
CAMWorks Nesting to CAMWorks
DefaultValues.ini
Enabling/Disabling the Display of the
Message shown before linking CAMWorks
Nesting with CAMWorks
DefaultValues.ini
Enabling/disabling the option of flattening
sheet metal parts before generating nested
layouts
DefaultValues.ini
Setting the Inventory Forecast Method to be
used
DefaultValues.ini
Enabling/disabling the display of Assembly
quantities in the Create Nesting Job dialog
box
DefaultValues.ini
Setting the Stamp Feature Unfold Option for
sheet metal parts
DefaultValues.ini
Enabling/disabling the option of nesting with
multiple tool heads
Machine.ini
Enabling the interactive dialog box to edit
parameters associated with nesting with
multiple tool heads
Machine.ini
Note: It is highly recommended that you read this section in order to gain an
understanding of how to customize the CAMWorks Nesting settings to meet
your facility‟s requirements.
50
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
StandardsSheets-INCH.ini & StandardsSheets-MM.ini
CAMWorks Nesting provides the option to define and store information of
standard sheet sizes used at your facility. This provides the benefit of
automating repetitive operations and saves time during the nesting
procedure by eliminating the need to define sheet dimensions.
 To define the length and width of a sheet in IPS units, use the
StandardSheets-INCH.ini file
 To define the length and width of a sheet in MMGS units, use the
StandardSheets-MM.ini file
Viewing the StandardSheets-INCH.ini/ StandardsSheetsMM.ini file:
1. Go to the CAMWorks Nesting installation folder. (A typical
installation path will be...Drive:\CAMWorksNestingData\
CAMWorksNesting 201x\Lang\English)
2. Open the file named StandardSheets-INCH.ini or
StandardSheets-MM.ini.
3. The fifth line of both these files indicates the sheet count. For
example, if 15 standard sheets have been defined, then the sheet
count is set to 15.
Adding sheets to the StandardSheets-INCH.ini/
StandardsSheets-MM.ini file:
1. The parameters defined in for a standard sheet include its name,
length, width.
2. Increment the Sheet count by 1 every time you add a sheet.
3. For example, suppose the StandardSheets-MM.ini file has 24
standard sheets defined. To add a 25th sheet with name S25, length
of 3500 mm and width of 2200 mm, increment the sheet count by
one and set it to 25. The format for defining this new sheet in the
StandardSheets-MM.ini file is as follows:
[Sheet25]
Name = S25
Length = 3500
Width = 2200
Adding a Standard Sheet in the StandardSheets-MM.ini file
Initialization Files of CAMWorks Nesting
51
CAMWorks Nesting Tutorial
Editing parameters in StandardSheets-INCH.ini/
StandardsSheets-MM.ini file
1. Once defined, the parameters of a sheet defined in the
StandardSheets-INCH.ini and StandardSheets-MM.ini can be
changed as and when the need arises.
2. Consider this example: Suppose a sheet named S23(12’ X8’) with a
Length of 144 inches and width of 96 inches is defined in the
StandardSheets-INCH.ini file. To change this sheet‟s name to
Std_Sheet23 (15’ x10’) with a length of 180 inches and width of
120 inches, the following changes need to be done in the
StandardSheets-INCH.ini file.
Sheet Parameters before changing
[Sheet23]
Name = S23(12‟ x8‟)
Length = 144
Width = 96
Sheet Parameters after changing
[Sheet23]
Name = Std_Sheet_23(15‟ x10‟)
Length = 180
Width = 120
Editing Parameters of a Standard Sheet in StandardSheets-INCH.ini
52
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Material.ini
The Material dropdown list available in the Pat Data tab allows you to assign
the material of the part(s) to be nested.
CAMWorks Nesting provides the option to populate the Material dropdown
list and thus store standard materials used at your facility. This provides the
benefit of making the material selection easier by enabling you to select
desired material from the dropdown list instead of manually typing it in.
Location
This file is located in the CAMWorks Nesting installation folder.
A typical installation path will be:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Lang\English
Viewing/Editing the Material dropdown list
1. Open the Material.ini file located in the CAMWorks Nesting installation
folder.
2. The second line of this file indicates the number of materials already
listed. For example, if 10 materials are defined in the file, then the
MaterialCount is set to „10‟.
3. To add more materials to the list, enter the name of the new material
in the same syntax as those already listed.
4. Increment the Material Count by 1 every time you add a material.
5. For example, to add a fifth material to a Material list containing four
materials, set the Material count to 5 and add the new material at the
bottom of the list:
[Material]
MaterialCount = 5
Material1 = Steel
Material2 = Copper
Material3 = Iron
Material4 = Bronze
Material5 = Aluminium
Typical syntax of the Material.ini file
Note: CAMWorks Nesting extracts the part parameter of Material from the Solid Part and
displays it in the Material field as default material of the part. When the material
cannot be extracted from the 3D model, CAMWorks Nesting assigns the first
material listed in the Material.ini file as the default material for the part.
Initialization Files of CAMWorks Nesting
53
CAMWorks Nesting Tutorial
DefaultValues.ini
This file is used to assign default values of part, sheet and nesting data
parameters. Certain default settings which cannot be set in the Create
Nesting Job dialog box are set from the DefaultValues.ini file.
Location
This file is located in the CAMWorks Nesting installation folder.
A typical installation path will be:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Lang\English
Assigning default Part Quantity
The default value for part‟s quantity can be assigned and edited in the
DefaultValues.ini file.
Steps to edit default part quantity in the DefaultValues.ini file
1. Open the file named DefaultValues.ini located in the CAMWorks
Nesting installation folder.
2. Observe the section named [PartData]. The default quantity is
defined in this section.
3. Edit the quantity value to apply a new default value for quantity of
the parts to be nested. For example, to assign a new default
quantity of '6', the value in the DefaultValues.ini should be changed
as follows:
[PartData]
;Quantity only Integers, real values are not supported
Quantity = 6
Typical syntax for setting Part quantity in DefaultValues.ini
Defining default Sheet Thickness and Quantity
 The DefaultValues.ini file can be used to define the default sheet
thickness for sheets of type Custom Size and Sheet DXF.
 The default sheet Quantity for all sheet types is defined in
DefaultValues.ini.
Steps to edit default sheet thickness and quantity in DefaultValues.ini file
1. Open the file named DefaultValues.ini located in the CAMWorks
Nesting installation folder.
2. Observe the section named [SheetData]. The default quantity (line
number 2) and thickness (line no. 3 and 4) for a sheet are defined
in this section.
54
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
3. The default quantity is always defined as an integer. Edit the
quantity value to apply a new default value for quantity of the
sheets.
4. The thickness value is defined in both millimeters (MMGS units) and
inches (IPS units). Edit these values to change the default value of
thickness.
5. For example, to assign a new default thickness of 4mm in MMGS
units, 0.1 inch in IPS units and a quantity of '2', the values in the
DefaultValues.ini will be changed as follows:
[SheetData]
;Quantity only Integers, real values are not supported
Quantity = 2
Thickness-MM = 4.000000
Thickness-Inch = 0.1
Typical syntax for setting Sheet Thickness & quantity in DefaultValues.ini
Defining default dimensions for Custom Sheet
 For sheets of type Standard Size, the dimensions for each sheet is
defined either in the StandardSheets-INCH.ini or StandardSheetsMM.ini file based on the unit system used.
 For sheets of type Custom Size, the dimensions are to be input by
the user. The default dimensions displayed on selection of sheet
type Custom Size is defined in the DefaultValues.ini file. Since the
dimensions are defined either in the MMGS or IPS unit system, the
default values too are defined in MMGS and IPS units separately.
Editing the Default Custom Size Dimensions in the DefaultValues.ini file
1. Open the file named DefaultValues.ini located in the CAMWorks
Nesting installation folder.
2. Observe the section named [CustomSheet]. The default Length and
Width to be displayed, when sheet of type Custom Size is selected,
is displayed in this section.
3. The length and width is defined in both MMGS and IPS units. Edit
these values to change the default Length and Width values.
4. For example, to assign a new default length of 2500mm and a
Width of 800 mm (MMGS units) and a length of 120 inches and
width of 72 inches (IPS units), the values under [CustomSheet] in
the DefaultValues.ini should be changed as follows:
Initialization Files of CAMWorks Nesting
55
CAMWorks Nesting Tutorial
[CustomSheet]
Length-MM = 2500
Width-MM = 800
Length-Inch = 120
Width-Inch = 72
Typical syntax for setting default dimensions for custom size
sheet in DefaultValues.ini
Assigning default Part to Part Distance & Part to Sheet
Distance
The default values to be displayed for Part to part distance and Part to
sheet distance in the Nesting Data Group Box are defined in the
DefaultValues.ini file.
Editing the Part to Part distance and Part to Sheet Distance
1. Open the DefaultValues.ini file located in the CAMWorks Nesting
installation folder.
2. Observe the section named [NestingData]. The default values for
Part to part distance and Part to sheet distance are defined here.
3. The Part to part distance and Part to sheet distance are defined in
both MMGS and IPS units. Edit these values to change the default
values.
4. For example, consider that a Part to Part Distance of 3mm and a
Part to Sheet Distance of 2mm is to be assigned in the new default
values in the MMGS units. Similarly, a Part to Part Distance of 0.125
inch and a Part to Sheet Distance of 0.25 inch is to be assigned in
the new default values in the MMGS units.
5. To apply these changes, the values under [NestingData] in the
DefaultValues.ini file should be changed as follows:
[NestingData]
PartToPartDistance-MM = 3
PartToPartDistance-Inch = 0.1250000
PartToSheetDistance-MM = 2
PartToSheetDistance-Inch = 0.250000
Typical syntax for setting default Part to Part and Part to Sheet distance
56
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Enabling/Disabling the Preferential Hole Filling Functionality
The „Preferential hole filling‟ functionality enables a smaller part to be
nested in the holes of larger parts during the nesting process resulting
in higher sheet utilization and minimal scrap.
Setting the PreferHoleFilling flag in the DefaultValues.ini file to „1‟
enables this functionality while setting it to „0‟ will disable the
functionality.
[NestingData]
;Options for PreferHoleFilling: 0 : No, 1 : Yes
PreferHoleFilling = 1
Settings in DefaultValues.ini file to enable Preferential Hole Filling
Note:
The option of Preferential Hole Filling cannot be set from within the Create
Nesting Job dialog box. You need to assign your preferred settings in the
DefaultValues.ini file for this option.
This functionality is illustrated in Tutorial 5.
Assigning default state for the Create Separate Assembly
option
You can set the default option whether the Create Separate Assembly
checkbox in the Nesting Data group box is to remain checked/
unchecked when you open the Create Nesting Job dialog box.
Setting the CreateSeparateAssembly flag in the DefaultValues.ini
file to „0‟ leaves this checkbox unchecked while setting it to „1‟ will
place a check in this checkbox.
[NestingData]
;Options for CreateSeparateAssembly: 0 : No, 1 : Yes
CreateSeparateAssembly = 0
Setting for the „Create Separate Assembly‟ option in DefaultValues.ini file
Initialization Files of CAMWorks Nesting
57
CAMWorks Nesting Tutorial
Assigning default state for the Automatically Select sheet
option
You can set the default option whether the Automatically select sheet
checkbox in the Nesting Data group box is to remain checked/
unchecked when you open the Create Nesting Job dialog box.
Setting the AutomaticallySelectSheet flag in the DefaultValues.ini
file to „0‟ leaves this checkbox unchecked while setting it to „1‟ will
place a check in this checkbox.
[NestingData]
;Options for Tick/Un-tick AutomaticallySelectSheet: 0:No, 1:Yes
AutomaticallySelectSheet = 1
Settings for the „Automatically Select Sheet‟ option in DefaultValues.ini file
Enabling/Disabling the option of Flattening Sheet Metal Parts
With respect to nesting of native sheet metal parts, you can choose
whether the nested layout is to be computed based on the flattened or
non-flattened sheet metal parts.
Setting the FlattenSheetMetalPart flag in the DefaultValues.ini file to
„1‟ enables computation of the nested layout based on the flattened
(unfolded) sheet metal parts. Setting this flag to „0‟ will lead to
computation of the nested layout based on non-flattened sheet metal
parts.
Note that this setting applies only to native sheet metal parts and not
imported sheet metal parts.
[NestingData]
;Options for FlattenSheetMetalPart: 0 : No, 1 : Yes
FlattenSheetMetalPart = 1
Settings in DefaultValues.ini file to enable flattening of sheet metal parts for nesting
Note:
The option of flattening or not flattening sheet metal parts for computation of
the nested layout cannot be set within the „Create Nesting Job‟ dialog box. You
need to assign the settings in the DefaultValues.ini file for this option.
This functionality is illustrated in Tutorial 3 and Tutorial 6.
For information on flattening imported sheet metal parts, refer Tutorial 7 &
Tutorial 8.
58
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Enabling/Disabling the option of utilizing ‘Fix Component’ or
‘Mate-Lock’ feature
The nested layout generated after a nesting job is an assembly of
parts. Sometimes, the parts may get accidentally repositioned from
their original position in the nested assembly due to human error, thus
disturbing the nested layout.
The 'Fix component' feature within SOLIDWORKS/CAMWorks Solids
prevents the movement of parts within an assembly for which this
feature is enabled. Similarly, the 'Mate-lock' feature of
SOLIDWORKS/CAMWorks Solids too serves the same purpose.
CAMWorks Nesting provides a setting in the DefaultValues.ini file
wherein the 'Fix component' or „Mate-Lock‟ feature of SOLIDWORKS/
CAMWorks Solids can be activated by default for all the parts in nested
layout(s) generated after the execution of a nesting job.
When the FixComponent flag in the DefaultValues.ini file is set to „1‟,
the 'Fix component' feature of SOLIDWORKS/CAMWorks Solids is
activated as default setting. However, the default setting of this flag at
the time of installation is „0‟, indicating that both the „Fix Component‟
and „Mate-Lock‟ features are inactive.
[NestingData]
;Option for FixComponent: 0 : No, 1 : Yes, 2: Mate - Lock
FixComponent = 1
Settings in DefaultValues.ini file to activate the „Fix Component‟ Feature
When the FixComponent flag in the DefaultValues.ini file is set to „2‟,
the 'Mate-Lock' feature of SOLIDWORKS/CAMWorks Solids is activated
as default setting.
[NestingData]
;Option for FixComponent: 0 : No, 1 : Yes, 2: Mate - Lock
FixComponent = 2
Settings in DefaultValues.ini file to activate the „Mate-Lock‟ Feature of
SolidWorks
Note: The settings for the „Fix Component‟ or „Mate-Lock‟ Feature cannot be changed
within the Create Nesting Job dialog box. You can only change the settings in the
DefaultValues.ini file.
Initialization Files of CAMWorks Nesting
59
CAMWorks Nesting Tutorial
Assigning the default Inventory Forecasting method
The Inventory Forecasting Module operates within CAMWorks Nesting
in the form of Automatically select sheet option. CAMWorks Nesting
supports two inventory forecasting methods viz. Unique Sheet
Forecaster and Combinatorial Sheet Forecaster.
The forecasting method to be used is defined in the DefaultVales.ini
file using the IFMType flag. Setting this flag to „1‟ enables the Unique
Sheet Forecaster method while setting it to „2‟ enables the
Combinatorial Sheet Forecaster method.
[NestingData]
;Option for IFMType: 1: For UNIQUE_SHEET_FORECASTER,
;2: For COMBINATORIAL_SHEET_FORECASTER
IFMType = 2
Settings in DefaultValues.ini file to assign the Inventory Forecasting
method to be used
Note: The Inventory Forecasting Method (IFM) used cannot be changed within the
Create Nesting Job dialog box. You need to change the settings in the
DefaultValues.ini file to change the method for inventory forecasting.
Assigning default state for the ‘Save Output as dxf’ option
You can set the default option whether the Save output as dxf
checkbox in the Nesting Data group box should remain checked/
unchecked when you open the Create Nesting Job dialog box.
In the [NestingData] section of the DefaultValues.ini file, setting the
DxfFile flag to „0‟ leaves this checkbox unchecked while setting it to
„1‟ places a check in this checkbox.
[NestingData]
Option for creating DXF file: 1 : Yes, 0 : No
DxfFile = 1
Settings for the „Save output as dxf‟ option in DefaultValues.ini file
60
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Enabling/disabling the functionality to add nested Parts to
CAMWorks Part Manager
An option is provided within CAMWorks Nesting that allows you to
automatically link the nested layout output of CAMWorks Nesting as
the input for CAMWorks. This automation saves considerable time by
reducing the steps required to generate the NC code.
For more details, read: Functionality to link CAMWorks Nesting with
CAMWorks
In the section named [AddPartsToCW] of the DefaultValues.ini file,
setting the flag named AddPartstoCWManager to „1‟ enables the
functionality and „0‟ disables this functionality.
By default, this flag is set to „1‟. Thus, the functionality is enabled by
default.
[AddPartsToCW]
AddPartstoCWManager=1 :Yes, 0 : No
AddPartstoCWManager = 1
Settings for enabling the functionality to link CAMWorks Nesting with CAMWorks
This functionality is illustrated in Tutorial 13.
Enabling/disabling the Display of the Message shown before
linking CAMWorks Nesting with CAMWorks
An option provide the how to enable/disable the display of the
message before linking CAMWorks Nesting with CAMWorks. The
setting for enabling/disabling the display of this message is controlled
from the DefaultValues.ini file.
In the section named [AddPartsToCW] of the DefaultValues.ini file,
setting the flag named DontShowAddPartsToCWWarning to „1‟ enables
the functionality and „0‟ disables this functionality.
By default, this flag is set to „1‟. This setting enables the display of the
warning message but the warning message will be displayed in the
CAMWorks Nesting UI only if the flag named 'AddPartstoCWManager' is
set to '1' in the DefaultValues.ini file.
[AddPartsToCW]
DontShowAddPartsToCWWarning=1 : Show msg, 0 : Don't show msg
DontShowAddPartsToCWWarning=1
Settings for enabling the functionality to display the warning message
This functionality is illustrated in Tutorial 13.
Initialization Files of CAMWorks Nesting
61
CAMWorks Nesting Tutorial
Enabling/disabling the feature of ‘Assigning Assembly
Quantities’
This setting comes into effect if you are nesting an assembly. It is
used to set the default state whether Quantity column for the
Assembly (and its constituent sub-assemblies, if any) are to be
displayed in the Part Data tab of the Create Nesting Job dialog box.
In the [AssemblyData] section of the DefaultValues.ini file, setting the
ShowAssemblyQuantity flag to „1‟ enables the display of Assembly
name and Quantity in the Part List grid of the Part Data tab in the
Create Nesting Job d0 ialog box. The parts comprising the assembly
and its sub-assemblies too will be listed in the Part Grid. This is the
default setting.
When this flag is set to „0‟, the Assembly name and Quantity columns
will not be displayed in the Part Data tab of the Create Nesting Job
dialog box. Only the parts comprising the assembly to be nested will
be listed in the dialog box.
[AssemblyData]
;Options for ShowAssemblyQuantity; 0 : Only Part Data,
1: Both Assembly and Part Data
ShowAssemblyQuantity = 1
Settings to enable display of Assembly Quantities in the Part Data tab of the
„Create Nesting Job‟ dialog box
This functionality is illustrated in Tutorial 9.
Settings for the Stamp Feature Unfold Option
The setting to control the behavior of the stamp feature display on a
sheet metal part after the part is unfolded can be assigned only from
the DefaultValues.ini file.
There are three available settings to control the behavior of the stamp
feature after the part is unfolded. This setting is controlled by the flag
named StampFeatureUnfoldingOption in the [Unfold_Options]
section of the DefaultValues.ini file.
Following are the values that can be assigned to this flag to control the
stamp feature behavior:
62
i.
0 : Assigning the value „0‟ ensures that the stamp feature is
retained after the part is unfolded. (This is the default
setting at the time of installation.)
ii.
1 : When the value „1‟ is assigned to this flag, the stamp
feature is patched with a flat planar surface after the part is
unfolded.
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
iii.
2 : When the value „2‟ is assigned to this flag, the stamp
feature is ignored after the part is unfolded. The area
covered by the stamp feature is replaced with a hole.
[Unfold_Options]
;StampFeatureUnfoldingOption=0 : Retain, 1 : Patch, 2 : Ignore
StampFeatureUnfoldingOption=0
Settings for the Stamp Feature Unfold Option for sheet metal parts
This functionality is illustrated in Tutorial 11.
Initialization Files of CAMWorks Nesting
63
CAMWorks Nesting Tutorial
Machine.ini
For flame cutting applications, CAMWorks Nesting provides an optional
functionality known as Multiple Tool Head Nesting. This functionality allows
you to nest two or more identical layouts simultaneously using multiple tool
heads. Machines which support nesting using multiple tool heads are known
as Multi tool head machines.
The nesting specific information and default values of parameters for such
machines are configured in the Machine.ini file.
 If your plan to make use of the Nesting with Multiple Tool Heads feature,
then the Machine.ini file needs to be customized depending on the
requirements at your machining facility.
 If you do not plan to use the feature of Nesting with Multiple Tool Heads,
then you can either disable the feature or leave the default settings
untouched.
Configuration settings in the Machine.ini file
The following settings are configured from the Machine.ini file:
 Enabling/ disabling the functionality for nesting with multiple tool
heads
 Enabling/Disabling the display of the Multi Head Options tab in the
Create Nesting Job dialog box
 The number (count) and names of machines which support the
functionality for nesting with multiple tool heads
 Default values of parameters associated with nesting with multiple tool
heads for such machines
Location
The Machine.ini file is located in the CAMWorks Nesting installation folder.
A typical installation path will be:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Lang\English
64
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Enabling/Disabling the option of Nesting with Multiple Tool
heads
1. Open the file named Machine.ini located in the CAMWorks Nesting
installation folder. Observe the first section named [MultiHeadData].
[MultiHeadData]
;Multi head flag; set to True(1) for multi tool head nesting, or else set to False(0)
MultiHeadFlag = 1
Syntax for enabling the option for nesting with multiple tools heads
2. The second line under this section contains the MultiHeadFlag. The
flag named MultiHeadFlag is used to enable/disable the functionality of
nesting with multiple tools.
a. When the MultiHeadFlag is set to „1‟, the option of nesting with
multiple tool heads will be activated. This is the default setting at
the time of installation.
b. When the MultiHeadFlag is set to „0‟, the option of nesting with
multiple tool heads will be disabled. No interactive dialog box (the
Multi Head Options tab in the Create Nesting Job dialog box) to
view /edit parameters associated with Multiple Tool Head Nesting
will be displayed. The settings of ShowMultiHeadDialog flag will be
immaterial since the function is inactive.
Note: To disable the feature of Nesting with Multiple Tool Heads, set the MultiHeadFlag
in the Machine.ini file to „0‟.
Initialization Files of CAMWorks Nesting
65
CAMWorks Nesting Tutorial
Enabling/disabling the display of the Multi Head Options tab
in the Create Nesting Job dialog box
The Multi Head Options tab in the Create Nesting Job dialog box is the
interactive interface that allows you to view/edit the parameters related to
Nesting with Multiple Tool Heads. The setting to enable/disable the display of
this tab is controlled from the Machine.ini file.
1. Open the file named Machine.ini located in the CAMWorks Nesting
installation folder. Observe the first section named [MultiHeadData].
[MultiHeadData]
;Multi head flag; set to True(1) for multi tool head nesting, or else set to False(0)
MultiHeadFlag = 1
;Value to indicate whether Multi head api needs to be shown or not : Yes : 1, No , 0
ShowMultiHeadDialog = 1
Syntax for enabling the display of the Multi Head Option tab
2. The fourth line under this section contains the ShowMultiHeadDialog
flag. When MultiHeadFlag is set to „1‟, the feature of Nesting with
Multiple Tool Heads is activated. The ShowMultiHeadDialog flag is used
to set the option whether a nesting job will be executed interactively
using user-specified parameters or with default parameter values
assigned to the Default machine in the Machine.ini file. This is
explained as follows:
 If the ShowMultiHeadDialog is also set to „1‟, then the Multi
head Options tab is displayed in the Create Nesting Job dialog
box. This tab allows you to view/edit the parameters for
nesting with multiple tool heads. This is the default setting at
the time of installation.
 If both the MultiHeadFlag and ShowMultiHeadDialog are set to
„0‟, then the feature of Nesting with Multiple Tool Heads will
be disabled and the Multi head Options tab will not be
displayed in the Create Nesting Job dialog box.
 If the MultiHeadFlag is set to „1‟ and the ShowMultiHeadDialog
is set to „0‟, then the feature of Nesting with Multiple Tool
Heads will be active but Multi head Options tab will not be
displayed in the Create Nesting Job dialog box. Consequently,
the next nesting job executed will use the default parameter
values assigned to the Default machine in the Machine.ini file
and complete the nesting process.
Note: The ShowMultiHeadDialog flag controls whether the Multi Head Options tab in the
Create Nesting Job dialog box will be displayed or not.
66
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Defining the Machines which support nesting with multiple
tools
For machines at your facility which support nesting with multiple tools, you
need to define their names and the number of such machines. You also need
to specify the default machine to be used when multiple machines are
present.
In the Machine.ini file, these machine names, machine count and default
machine to be used are defined in the [DefaultMachine] section.
Assigning the Machine Count, machine names and default machine
1. Observe the section named [DefaultMachine] of the Machine.ini
located in the CAMWorks Nesting installation folder.
[DefaultMachine]
;Machine# where # is a number greater than 0 and less than the value of “Machine
Count”
MachineCount = 5
Machine1 = SingleTHMachine
Machine2 = MachineName1
Machine3 = MachineName2
Machine4 = MachineName3
Machine5 = MachineName4
;Default machine name: # where # is a number between 0 and MachineCount
DefaultMachineName = Machine1
Typical syntax for defining the machine names, machine count and default machine
2. The machine count, name of the machines and default machine to be
used are defined here.
 MachineCount: The integer value assigned to this setting indicates
the number of machines which support the „nesting with multiple
tools‟ functionality. The machine count has to necessarily be an
integer value greater than zero. Increment the MachineCount by 1
every time you add a machine.
For example, if you have three machines at your facility, the
machine count will be „3‟.

Machine# = <machine name>: This setting indicates names of
the machines which support the nesting with multiple tools
functionality. Machine# denotes the machine number. # is a
number greater than zero and less than/equal to the MachineCount
value. The <machine name> is an alphanumeric text string that
represents the machine name. The defined machine names form a
list of machines.
In the Multi head options tab of the Create Nesting Job dialog box
(the interactive dialog box to edit the multiple tool head related
Initialization Files of CAMWorks Nesting
67
CAMWorks Nesting Tutorial
parameters), the Machine dropdown list is populated by the
Machines listed in this setting.

DefaultMachineName: This setting is used to indicate the default
machine from the list of machine(s) defined. When MultiHeadFlag is
set to „1‟ and ShowMultiHeadDialog is set to „0‟, the nesting job will
be executed using default parameters of the machine assigned in
this setting.
Example: Consider that you have three machines which support
the Nesting with multiple tools functionality. First
machine is named SUN360, second is named RAK100
and the third MARS99. The first machine is to be
assigned as the default machine. Then the settings
under [DefaultMachine] section in the Machine.ini file
should be as follows:
MachineCount = 3
Machine1 = SUN360
Machine2 = RAK100
Machine3 = MARS99
DefaultMachineName = SUN360
The Default Machine Configuration
Observe the [DefaultMachine] section of the Machine.ini file. Machine1
(SingleTHMachine) is assigned as the default machine. This machine
contains only a single tool head and thus represents machines used to
execute nesting jobs using a single tool head.
If majority of your nesting jobs are done using single tool head machines,
then it is highly recommended you leave Machine1 (SingleTHMachine) set as
the default machine. Using SingleTHMachine as the default machine ensures
that all nesting job are executed considering a single tool head. This setting
effectively keeps the feature of Nesting with multiple tool heads inactive
unless another machine is manually chosen by the user in the Multi Head
Options tab of the Create Nesting Job dialog box.
Note: If a majority of your nesting jobs are executed with single tool head machines,
then it is highly recommended that you do not change the machine
(SingleTHMachine) assigned as the Default Machine in the Machine.ini file.
68
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial
Defining default parameter values for Machines which
support nesting with multiple tools
Default values need to be assigned to the parameters associated with
nesting with multiple tools for the machine(s) at your facility.
For every machine listed in the [DefaultMachine] section, these default
parameter values is set individually in the [Machine#] section. (#
refers to Machine number)
Assigning default values to parameters associated with nesting with
multiple tool heads
1. Open the file named Machine.ini located in the CAMWorks Nesting
installation folder.
2. Observe any of the sections named [Machine#]. (# refers to Machine
number)
3. For every machine that was listed in the [DefaultMachine] section, the
default parameters associated with nesting with multiple tool heads
are assigned here. For every listed machine, a separate [Machine#]
section with default parameter values needs to be created.
As an example, the parameter values for [Machine2] are given below:
[Machine2]
;Maximum number of tool heads
MaxNoToolHeads = 5
;Rail direction: X or Y
RailDirection = X
;Tool head distance
ToolHeadDistance-MM = 500
ToolHeadDistance-INCH = 20
;Multi head nesting type: Fixed : 1 , Variable: 2
MultiToolHeadNestingType = 1
Typical syntax for assigning default values to parameters associated with nesting with
multiple tools
4. These parameters are explained below:

MaxNoToolHeads: Indicates the maximum number of tool heads
available for the machine.
For example, if the MaxNoToolHeads is 4 for a particular machine,
then in the Multi Head Options tab of the Create Nesting Job dialog
box, the Number of tool heads dropdown list will be populated with
integer values in the range of 1 to 4. You can assign the number of
tool heads as any number from 1 to 4 by selecting it from the
dropdown list.

Rail Direction: You can assign the default rail direction as „X‟ or
„Y‟. This default rail direction will be displayed in the Multi Head
Initialization Files of CAMWorks Nesting
69
CAMWorks Nesting Tutorial
Options tab of the Create Nesting Job dialog box. The default option
can be changed within this dialog box.

ToolHeadDistance-MM & ToolHeadDistance-INCH: This value
indicates the default minimum tool head distance to be used for
nesting with multiple tool heads.
When the MMGS units are used, CAMWorks Nesting will display the
value assigned to ToolHeadDistance-MM as the default Tool head
distance in the Multi Head Options tab of the Create Nesting Job
dialog box. This default value displayed can be edited within the
dialog box.
When the IPS units are used, CAMWorks Nesting will display the
value assigned to ToolHeadDistance-INCH as the default Tool head
distance in the Multi Head Options tab of the Create Nesting Job
dialog box. This default value displayed can be edited within the
dialog box.

MultiToolHeadNestingType: You can choose between Fixed tool
head distance and Variable tool head distance for the multi-tool
head nesting type. The default multi-tool head nesting type option
will be displayed in the Multi Head Options tab of the Create Nesting
Job dialog box in the respective parameter fields. The default option
can be changed within the dialog box.
a. Fixed tool head distance: Assign „1‟ to
MultiToolHeadNestingType to indicate Fixed tool head distance as
the default multi-tool head nesting type.
b. Variable tool head distance: Assign „2‟ to
MultiToolHeadNestingType to indicate Variable tool head distance
as the default multi-Tool head nesting type.
Adding a new machine in the Machine.ini file
The following example illustrates how to add a new machine to the list
of machines in the Machine.ini file.
Example: Consider that three machines named „SUN360‟, „RAK100‟
and „MARS99‟ are already listed in the Machine.ini file with
„SUN360‟ assigned as the default machine. You wish to add
a new machine with the name „SKY444‟ to this list and
assign it as the default machine. The default parameters to
be assigned to this machine are as follows:
70
Initialization Files of CAMWorks Nesting
CAMWorks Nesting Tutorial





Max number of tool heads:
6
Default Rail Direction:
Y
Tool Head Distance (in millimeters): 125mm
Tool Head Distance (in inches):
5 inches
Default multi-tool head nesting type: Variable tool head distance
Solution:
1. Open the Machine.ini file.
2. Go the section named [DefaultMachine] and make the following
changes:
[DefaultMachine]
MachineCount = 3
Machine1 = SUN360
Machine2 = RAK100
Machine3 = MARS99
DefaultMachineName = SUN360
[DefaultMachine] before changes
[DefaultMachine]
MachineCount = 4
Machine1 = SUN360
Machine2 = RAK100
Machine3 = MARS99
Machine4 = SKY444
DefaultMachineName = SKY444
[DefaultMachine] after changes
3. Next, after the [Machine3] section in the Machine.ini file, add a new
section named [Machine4] with the following values assigned to its
parameters:
[Machine4]
;Maximum number of tool heads
MaxNoToolHeads = 6
;Rail direction: X or Y
RailDirection = Y
;Tool head distance
ToolHeadDistance-MM = 125
ToolHeadDistance-INCH = 5
;Multi head nesting type: Fixed : 1, Variable : 2
MultiToolHeadNestingType = 2
Assigning default parameter values to the new machine added in the Machine.ini file
4. Save the changes made to Machine.ini file. The new machine will
now be added to the list of machines. In the Multi Head Options tab
of the Create Nesting Job dialog box, this machine will be available
in the dropdown list of available machines.
Initialization Files of CAMWorks Nesting
71
SECTION THREE
CAMWorks Nesting
Tutorials
CAMWorks Nesting Tutorial
TUTORIAL 2- SINGLE PART, SINGLE SHEET
NESTING FOR A SOLID PART
Introduction
This tutorial explains how to nest a solid part in a sheet layout. You will also
learn how to nest the part using CAMWorks Nesting commands that
automatically nest multiple instances of the part on a pre-defined sheet and
generates a best fit resulting in high sheet utilization and minimal scrap.
Topic covered in this Tutorial:
 Selecting the part to be nested
 Setting part parameters such as thickness, quantity, material, grain
direction and rotation angle.
 Defining sheet size of type Standard Size
 Selecting the Normal Direction
 Selecting the output assembly file
STEP 1: Open the Part
1. Load the CAMWorks Nesting Add-In in SOLIDWORKS or CAMWorks
Solids.
2. Open the part file Tutorial_2.sldprt in the following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Parts
Tutorial_2.sldprt
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
73
CAMWorks Nesting Tutorial
STEP 2: Define the Part Parameters
1. Select Create Nest Job from the
CAMWorksNesting menu bar.
OR
Click on the Create Nesting Job button
on the CAMWorks Nesting Ribbon Bar.
2. The Create Nesting Job dialog box is
displayed. Use the Part data tab of
this dialog box to set the parameters
for the part.
3. The solid part Tutorial_2.sldprt is
listed in the Part List along with its
nesting parameters.
Select Create Nesting Job in the
CAMWorksNesting menu
The Part Data tab of the Create Nesting Job dialog box
Assign the following values to the following Part Parameters:
a) Thickness: CAMWorks Nesting extracts the part parameter of
Thickness from the Solid Part and displays it in the Thickness field
74
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
CAMWorks Nesting Tutorial
as default thickness for the part. The thickness of the part, as
extracted from the solid part, is displayed as 10 mm.
b) Material: CAMWorks Nesting extracts the material info from the
Solid Part and displays it in the material field. The material for this
part, as extracted from the solid part, is Steel.
c) Quantity: The default quantity value is displayed in the Quantity
field (As per default value defined in the DefaultValues.ini file).
Double click on the „Quantity‟ field in the Part list. Set the Part
Quantity to „100‟.
d) Angle: Double on the Angle column of the Part List. Edit and assign
an angle of 90 degrees.
e) Grain Direction: Leave the Grain direction set to None.
f) Normal Face: By default, CAMWorks Nesting chooses the face with
the largest number of features. So the bottom face of the solid part
is chosen by default. The normal direction is indicated by an arrow
in the graphics area. To chose the top face (indicated by pink color)
as the normal face, do either of the following:
i.
Click on the Reverse button
ii.
In the graphics area, click on the top most face of the solid
part (face in pink color)
Observe that the arrow indicating the normal direction changes
accordingly.
Normal direction when bottom face is selected
Normal direction when top face is selected
STEP 3: Define the Sheet Parameters & adding a
standard sheet
1. Click on the Sheet Data tab. Observe that the assigned thickness and
material of the sheet are identical to those of the part to be nested.
2. Set the sheet Quantity to „1‟.
3. In this tutorial, we will nest the part using a Standard size sheet. Click
on the Standard size dropdown list. Observe the Standard Sheet sizes
defined in the Standard size dropdown list.
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
75
CAMWorks Nesting Tutorial
Standard size sheets dropdown list
4. Observe that the standard sizes defined in the Standard Sheets.ini file
are listed in the dropdown list. In this example, we will choose the
second sheet displayed in the list. (with Length = 1800 mm & Width =
1500 mm)
5. Click Add Sheet button. The sheet is added to the Sheet list.
Selected sheet added to Sheet list
76
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
CAMWorks Nesting Tutorial
STEP 4: Selecting a machine with Single Tool Head for
the Nesting Process
1. Click on the Multi Head Options tab.
2. In the Machine Data group box, ensure that the Machine selected is
SingleTHMachine. The Number of tool heads for this machine should
be „1‟.
Selecting SingleTHMachine as the machine in the Multi Head Options tab
Selecting SingleTHMachine as the machine ensures the nesting job is
executed considering a single tool head and not multiple tool heads.
STEP 5: Define Nesting Parameters
1. Observe the Nesting Data Group Box. For this tutorial, set a Part to
Part distance of 4 mm and a Part to Sheet distance of 4mm.
2. Use the
button to specify the folder location where the Output
Assembly file and Summary text file will be saved.
3. Leave the checkbox Save output as dxf checked. Use the
button
next to this checkbox to assign the folder location where the nested
layouts generated will be saved in the .dxf file format.
4. Set the Nesting method to Fast Nesting.
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
77
CAMWorks Nesting Tutorial
Defining Nesting Parameter values
STEP 6: Generating the Nested Layout
1. After setting the part, sheet and nesting parameters, click OK. This
sets into motion the process to generate a nested layout.
2. After the Nesting process is completed, CAMWorks Nesting will display
a message indicating the location of the text file containing the
summary of the Nest Results. Click OK to close the message. The
Text file will be displayed.
3. The Nested layout assembly will be displayed in the Graphics area.
Both the summary file and the assembly files are saved in the location
indicated Output Assembly File path stated in the Create Nesting Job
dialog box.
4. Browse to the folder location specified for saving the nested layouts in
the .dxf format. Observe that the nested layout in .dxf file format is
saved in the folder.
In this tutorial, we will observe the 3 nesting results:
i.
Nesting layout generated when top face of the part is chosen as
normal face
78
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
CAMWorks Nesting Tutorial
ii.
iii.
Nesting layout generated when bottom face of the part is chosen as
normal face
Nesting layout when Grain direction is set for part and the sheet.
Result A
Follow all the above steps and view the Nested layout. Observe that all
the 100 instances of the part (specified quantity) have been nested.
Result A: Nest Result obtained with the top face of the part chosen as normal face
Close up view of the Nesting Layout
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
79
CAMWorks Nesting Tutorial
Result B
Repeat all the steps listed in this tutorial without changing the default
Normal direction (Step2-4-f). To set the previous normal direction, select the
bottom face (gray-colored face) of the part in the graphics area when the
Create Nesting Job dialog box is displayed and the Part Data tab is the active
tab. View the nesting layout. Observe that all the 100 instances of the part
(specified quantity was 100) have been nested.
Result B: Nest Result obtained with the bottom face of the part chosen as normal face
Close up view of the Nesting Layout
80
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
CAMWorks Nesting Tutorial
Result C
Repeat all the steps listed in this tutorial. However, this time, in Step 2-4e, set the Grain Direction of the Part to X direction. In the Sheet Data tab,
set the Grain Direction of the Sheet to X direction. Execute Nesting. View
the nesting layout. All the parts are nested along the specified grain
direction. Observe that only 96 instances of the part are nested while the
quantity specified was 100. The same result will be obtained if the Grain
direction of both the part and sheet are set to Y direction.
Result C: Nest Result obtained with the top face of the part chosen as normal
direction
Tutorial 2 – Single Part, Single Sheet Nesting for a Solid Part
81
CAMWorks Nesting Tutorial
TUTORIAL 3 – SINGLE PART, SINGLE SHEET
NESTING FOR SHEET METAL PART
Introduction
This tutorial explains how to nest a sheet metal part in a sheet layout. You
will also learn how to nest the part using CAMWorks Nesting commands that
automatically nests multiple instances of the part on a pre-defined sheet and
generates a best fit resulting in high sheet utilization and minimal scrap.
Topic covered in this Tutorial:
 Selecting the sheet metal part to be nested
 Setting user-defined material for the part.
 Setting the Angle List
 Defining sheet size of type „Custom Size‟
STEP 1: Open the Part
1. Load the CAMWorks Nesting Add-In in SOLIDWORKS/CAMWorks
Solids.
2. Open the part file Tutorial_3.sldprt in the following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Parts
Tutorial_3.sldprt
82
Tutorial 3 – Single Part, Single Sheet Nesting for Sheet Metal Part
CAMWorks Nesting Tutorial
STEP 2: Change in Configuration File settings
Enabling the option to Flatten Sheet Metal Part
In this tutorial, you will nest the sheet metal part based on its dimensions
after flattening. The default settings configured in the DefaultValues.ini file
ensure that sheet metal parts are flattened before the nesting job is
executed. If you are unsure about the settings, open the DefaultValues.ini
file and set the FlattenSheetMetalPart flag to „1‟ in order to activate the
option of flattening.
Enabling the Fix Component Feature of SOLIDWORKS
In the configuration file DefaultValues.ini (located within the CAMWorks Nesting
Installation folder), ensure that the flag FixComponent under [NestingData]
section is set to „1‟.
This setting enables the SOLIDWORKS Fix Component feature which will
ensure that after the Nested layouts are generated, the parts in the Nested
layout assembly do not get accidentally repositioned.
STEP 3: Define the Part Parameters
1. Select „Create Nest Job‟ from the CAMWorksNesting menu bar.
2. The Create Nesting Job dialog box opens. Observe that the sheet
metal part Tutorial_3.sldprt displayed in the graphics area is
automatically flattened.
Tutorial_3.sldprt after flattening
3. In the Part Data tab, set the following nesting parameters:
Tutorial 3 – Single Part, Single Sheet Nesting for Sheet Metal Part
83
CAMWorks Nesting Tutorial
a) Thickness: The thickness of the sheet metal part, as extracted
from the solid part is 3mm. In this tutorial, no changes are made to
the thickness.
b) Material: Since Material related information is not defined for this
sheet metal part, CAMWorks Nesting will display the first material
(Steel) in the Material drop down list as the default material. In this
tutorial, we will assign a material „Chrome Steel‟ which is not part of
the Material Dropdown list. To assign „Chrome Steel‟ as the
material, following are the steps:
i.
In the Part List, highlight the part for which material is to be
assigned.
ii.
In the Material combo box (located below the Part List), enter
the material name as „Chrome Steel‟.
iii.
Shift focus. Observe that the Material of the part is updated in
the Part List.
c) Quantity: Set the Part Quantity to „125‟.
d) Angle: Set a step angle of 900.
e) Grain Direction: Leave the Grain direction is set to „None‟.
f) Normal Face: No changes are made to the default normal face
selection.
STEP 4: Defining a „Custom‟ size sheet
1. Click on the Sheet Data tab. Observe that the assigned thickness and
material of the sheet are identical to those of the part to be nested.
2. In this tutorial, a custom sheet will be used to nest the parts:
a) Select „Custom Size‟. The Length and Width fields will be activated
and will display default values as defined in the DefaultValues.ini
file.
b) Assign a length of 1500mm and a width of 1200 mm.
c) Set the Sheet quantity to 1.
d) Some intelligence is added in CAMWorks Nesting such that it
ensures the sheets with relevant material and thickness is
available for nesting the part. CAMWorks Nesting automatically
extracts the thickness and material of the first part in the part list
and assigns these as the default value of the first sheet. Observe
that the material field displays „Chrome Steel‟ and thickness field
displays 3 mm.
e) Click Add Sheet to add the sheet to the Sheet List.
f) In the sheet List, the Sheet name of the added Custom Sheet can
be changed as required by double-clicking on the sheet name in the
sheet list.
84
Tutorial 3 – Single Part, Single Sheet Nesting for Sheet Metal Part
CAMWorks Nesting Tutorial
g) Sheet name in the Sheet Name column of the Sheet List. Assign a
new name Custom(1500‟X1200‟)
Defining a Custom Sheet
STEP 5: Selecting a machine with Single Tool Head for
the Nesting Process
1. Click on the Multi Head Options tab.
2. In the Machine Data group box, ensure that the Machine selected is
SingleTHMachine. The Number of tool heads for this machine should
be „1‟.
Selecting SingleTHMachine as the machine ensures the nesting job is
executed considering a single tool head and not multiple tool heads.
STEP 6: Define Nesting Parameters
1. In the Nesting Data Group Box, set a Part to Part distance of 3 mm
and a Part to Sheet distance of 2 mm.
2. Use the
button next to the Output assembly field to specify where
the nested layout and the Summary text file that are generated will be
saved.
STEP 7: Generating the Nested Layout
a. Select Fast Nesting as the Nesting method. Click OK.
b. Read the Results Summary text file. It indicates that 124 instances of
the part required are nested.
Tutorial 3 – Single Part, Single Sheet Nesting for Sheet Metal Part
85
CAMWorks Nesting Tutorial
Nesting layout obtained for Tutorial_3.sldprt
86
Tutorial 3 – Single Part, Single Sheet Nesting for Sheet Metal Part
CAMWorks Nesting Tutorial
TUTORIAL 4 – NESTING OF MULTIPLE PARTS BASED
ON THICKNESS
Introduction
This tutorial explains how to nest multiple solid parts of varying thicknesses.
You will observe how CAMWorks Nesting generates a multiple layout based
on the part thickness in a single Nesting job.
Topic covered in this Tutorial:
 Using the Nest by Folder option
 Assembly Nesting of multiple parts
 Selectively nest few parts in the Part List
 Defining a sheet using a DXF file
 Nesting multiple parts of varying thickness on sheets of corresponding
thickness
 Nesting of multi-body parts and assemblies containing multi-body
parts.
STEP 1: Using „Nest by Folder‟ to open the Assembly
1. Select Nest by Folder option in the CAMWorks Nesting menu bar.
OR
Click on the Nest by Folder button on
the CAMWorks Nesting Ribbon Bar.
CAMWorks Nesting Ribbon
Bar
„Browse‟ for Folder dialog box
2. The Browse for folder dialog box opens. Browse to the folder named
Tutorial4 in the following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial4
Tutorial 4 – Nesting of Multiple parts based on Thickness
87
CAMWorks Nesting Tutorial
3. CAMWorks Nesting opens all the parts contained in the folder as an
assembly in the SOLIDWORKS Graphics area.
4. The Create Nesting Job dialog box is displayed. All the parts present in
the folder are listed in the Part List of the Part data tab.
STEP 2: Define the Part Parameters
„Nest by Folder‟ parts listed in the Part List
Selectively Nesting Parts
In the Part data tab, observe the
Part name column of the Part List.
Every listed part has a checkbox
to its right which is selected. Such
a selected checkbox indicates that
the associated part will be taken
up for Nesting during the Nesting
process. To selectively nest only
certain parts in the Part list,
88
Deselecting parts which are not be nested
Tutorial 4 – Nesting of Multiple parts based on Thickness
CAMWorks Nesting Tutorial
deselect the checkbox of those parts which you do not want to nest.
In this tutorial, we will initially nest only the parts „TutPart4A SM‟ and
„TutPart4D SM‟. Both of these are sheet metal parts. Hence, in the Part list,
uncheck the checkboxes given against the parts „TutPart4B SM‟ and
„TutPart4C SM‟.
TutPart4A SM
TutPart4D SM
Material
Since Material related information is not defined for this sheet metal part,
CAMWorks Nesting will display the first material in the Material drop down
list as the default material (Steel). In this tutorial, we will assign a material
Copper to all the parts. This material is listed in the Material Dropdown list.
Select TutPart4A and TutPart4D by pressing ctrl key and assign Copper from
the Material dropdown list.
Normal Face
No changes are made to the default normal face selection for any of the
parts.
Grain Direction
Leave the Grain direction set to None.
Step Angle
Assign a Step Angle of 900 to all the parts.
Quantity
Assign a quantity of „62‟ to both the parts to be nested.
Tutorial 4 – Nesting of Multiple parts based on Thickness
89
CAMWorks Nesting Tutorial
STEP 3: Adding a sheet of using „DXF‟ file.
In previous tutorials, we learned how to add Standard size and Custom size
sheets. In this tutorial, we will use a file in .dxf format to define the sheet.
Following are the steps to define a sheet using a file in .dxf format:
1. Under the Sheet data tab, select the option Sheet DXF.
2. This activates the field used to indicate the path of the DXF file. Click on the
button to browse to the folder containing the DXF file.
3. Select the .dxf format file named „Tutorial4_sheet.dxf‟ from following
location.
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Examples\Tutorials\ Sheets
4. CAMWorks Nesting populates the thickness and material field for each
prospective sheet to be added to the sheet list based on the serial order of
the parts listed in the part tab. Hence, by default, the Thickness field and the
Material field will display the values of the first selected part listed in the
part list. In this tutorial, the thickness and material of the first part (3mm
and Copper respectively) will be displayed as default values.
5. Assign Sheet quantity as „1‟ and Grain direction as None.
6. Click Add sheet to add the file in .dxf format to the Sheet List.
DXF file added to sheet list
7. The file in .dxf format is added to the Sheet List. The Sheet preview
indicates that this sheet is a remnant (remainder) sheet.
90
Tutorial 4 – Nesting of Multiple parts based on Thickness
CAMWorks Nesting Tutorial
STEP 4: Selecting a machine with Single Tool Head for
the Nesting Process
1. Click on the Multi Head Options tab.
2. In the Machine Data group box, ensure that the Machine selected is
SingleTHMachine. The Number of tool heads for this machine should
be „1‟.
Selecting SingleTHMachine as the machine ensures the nesting job is
executed considering a single tool head and not multiple tool heads.
STEP 5: Define Nesting Parameters
1. In the Nesting Data Group Box, set a Part to Part distance of 2mm and a
Part to sheet distance of 2mm.
2. Under Nesting type, select Fast Nesting as the Nesting method.
3. Use the
button next to the Output assembly field to specify where the
nested layouts and the Summary text file that are generated will be
saved.
4. Click OK to execute the nesting process.
5. Observe the Nested layout. The assigned quantities of both parts have
been nested.
Nested Layout in the DXF sheet
Tutorial 4 – Nesting of Multiple parts based on Thickness
91
CAMWorks Nesting Tutorial
STEP 6: Nesting all the Parts in the Assembly
In the following section, we will learn how to nest parts of varying thickness in
a single nesting job.
1. Close the generated assembly file. The four parts are still displayed in the
SOLIDWORKS Graphics area. Select Create Nesting Job from the
CAMWorksNesting menu. The Create Nesting Job dialog box is displayed.
2. Observe the Part list. As observed in Step 2 of this tutorial, two of the
parts viz. „TutPart4A SM [Default]‟ and „TutPart4D SM [Default]‟ are sheet
metal parts of 3mm thickness each. The other two parts, „TutPart4B SM
[Default]‟ and „TutPart4C SM [Default]‟ are solid parts of thickness 20 mm
each.
TutPart4B SM.sldprt
TutPart4C SM.sldprt
3. Double click on thickness header in the part list; it automatically arranges
the parts based on thickness as shown below. Set the following quantities
for the parts displayed in the Part list:
92
Tutorial 4 – Nesting of Multiple parts based on Thickness
CAMWorks Nesting Tutorial
Part Name
TutPart4B 20mm.SLDPRT
TutPart4C 20mm.SLDPRT
TutPart4A SM.SLDPRT
TutPart4D SM.SLDPRT
Part Quantity
30
20
64
122
Thickness
20 mm
20 mm
3 mm
3 mm
4. Set the material, grain direction, normal face and angle with the values
as given in Step 2.
5. All the parts now have the same material but, as observed in the above
table, two parts have a thickness of 20mm while the other two have a
thickness of 3 mm. Hence, at least two sheets with a thickness of 20mm
and 3mm respectively will be required to nest these parts. In this tutorial,
we will use two standard sheets of size „S1 (6‟ X 4‟)‟, each assigned the
appropriate thickness to nest these parts.
Adding a standard sheet
Following are the steps to add a standard sheet for this tutorial:
i.
Click on the Sheet Data tab. In the Sheet list, click on Select to add
sheet.
ii.
To add a standard sheet, select the „S1 (6‟ X 4‟) – Len: 1800 mm
Width: 1200 mm‟ sheet from the Standard Size dropdown List.
iii.
CAMWorks Nesting populates the thickness and material field for
each sheet to be added to the sheet list based on the serial order of
the parts listed in the part tab. Hence, by default, the Thickness
field and the Material field will display the values of the first part
listed in the part list. In this tutorial, the thickness and material of
the first part is 3mm and Copper respectively. In case this value is
not displayed in the fields, assign the appropriate values.
iv.
In the Quantity field, assign a quantity of „1‟.
v.
Leave the Grain Direction set to None.
vi.
Click Add Sheet to add the sheet to the Sheet list.
vii.
The standard sheet is added to the sheet list. Click on Select to add
sheet in the sheet list.
viii.
Repeat step 2.
ix.
This time, as per the principle explained in step iii, the thickness
and Material field will display values of the next part in the part list
which has either its thickness or material or both different from the
previous part. Thus, thickness field will display a value of 20mm
and material field will display „Copper‟.
x.
Repeat step iv, v and vi to add the sheet.
Tutorial 4 – Nesting of Multiple parts based on Thickness
93
CAMWorks Nesting Tutorial
6. In the Nesting data group box, leave the Part to part distance and Part to
sheet distance set to „0mm‟. Specify the location for the output assembly
file and Summary text file using the
Assembly File field.
button next to the Output
7. Click OK to execute the Nesting process.
8. View the Summary text file. All the parts have been nested as per their
assigned quantities.
Nested Layout of TutPart4A SM.SLDPRT and TutPart4D SM.SLDPRT
94
Tutorial 4 – Nesting of Multiple parts based on Thickness
CAMWorks Nesting Tutorial
Nested Layout of TutPart4B SM.SLDPRT and TutPart4C SM.SLDPRT
Nesting of multi-body parts
CAMWorks Nesting supports nesting of multi-body parts and assemblies
containing multi-body parts. However, additional steps must be executed in
order to nest such a part or assembly.
CAMWorks Nesting processes the multi-body part before it can be nested. In
order to nest such a part, CAMWorks Nesting creates and saves each body
contained in the multi-body part as a new part. It then proceeds to create an
assembly comprising these newly created parts. This newly created assembly
becomes the active document considered for the nesting process.
Steps to nest a Multi-body Part
i.
ii.
iii.
iv.
Model or open a sheet metal part/ solid part model in SOLIDWORKS/
CAMWorks Solids.
Select Create Nesting Job from the CAMWorksNesting menu bar.
CAMWorks Nesting will check the part for multiple bodies.
If the part has multiple bodies, you will be prompted with a message box
stating that each body of the part will be saved as a new part and that a
new assembly will be created for this multi body part with each body as a
separate component. Click OK to continue.
Tutorial 4 – Nesting of Multiple parts based on Thickness
95
CAMWorks Nesting Tutorial
v.
vi.
vii.
viii.
ix.
x.
If you agree to proceed, a new part will be created for each body and will
be stored in a new folder located inside the folder containing the parent
part (original part with multiple bodies).
Suppose the name of the parent part is PartName. Then the new folder
will be named as PartName_WithoutMultiBodyParts. If a folder with such
a name already exists, then the newly created folder will be named
'PartName_WithoutMultipleBodyParts1' and so forth. The new part made
out of the first body of the parent part will be named as PartName_1; the
second body will be named PartName_2 and so forth. A new assembly
named Assembly.SLDASM comprising these new parts will be created and
saved in the newly created folder.
If the folder which contains the parent part does not have write
permissions, you will be prompted to choose a folder location to save the
newly created parts and to input the name of the new assembly to be
created. The parts created out of the parent part with multiple bodies will
be saved inside the folder specified by you.
The new assembly comprising these parts will be saved inside the same
folder with the name input by you.
This new assembly comprising parts created out of the parent part will
now become the active document considered for nesting process. The
single body parts are listed under the Part Data tab of the Create Nesting
Job dialog box.
Complete the nesting process for this assembly by following the general
steps explained in Tutorial 4.
Nesting of assemblies containing multi-body parts
CAMWorks Nesting supports nesting of multi-body parts and assemblies
containing multi-body parts. However, additional steps must be executed in
order to nest such a part or assembly.
CAMWorks Nesting processes the assembly containing multi-body part(s)
before it can be nested. Before nesting an assembly, CAMWorks Nesting checks
the assembly for parts containing multiple bodies. If multi-body parts are
found, CAMWorks Nesting will create a new part out of each body of the multibody part(s). After this action, either a new assembly containing parts with
single bodies will be created or the existing assembly will be modified to with
the multiple body part(s) being replaced with the newly created parts. The
action executed is based on the choice input by you. The newly created
assembly or modified existing assembly becomes the active document
considered for the nesting process.
Steps to nest an Assembly containing Multi-body Parts
i.
ii.
96
Model or open the Assembly to be nested in SOLIDWORKS/CAMWorks
Solids.
Select „Create Nesting Job‟ from the CAMWorksNesting menu bar.
Tutorial 4 – Nesting of Multiple parts based on Thickness
CAMWorks Nesting Tutorial
iii.
iv.
v.
vi.
vii.
viii.
CAMWorks Nesting will check the Assembly for parts with multiple bodies.
On detecting part(s) with multiple bodies in the assembly, you will be
prompted with a message box stating that each body of the part will be
saved as a new part and that either a new assembly will be created or the
existing assembly will be modified. Click Yes to create a new assembly
else click No to modify the existing assembly.
If you click Yes, a new assembly containing all parts with single bodies
will be created. If you click No, the existing assembly will be modified
with the multi-body part being replaced with single body parts. (In either
assembly, the multi-body part will be removed). Note that in case of
modifying the existing assembly, the sub-assemblies (if there are any)
will be removed and all parts will have the existing assembly as their
immediate parent.
Suppose the name of the existing assembly to be nested is XYZ.sldasm
and it contains two multi-body parts, say 'X' and 'Y' and a single body
part named 'Z'. Then CAMWorks Nesting creates new parts out the multibody parts and either generates the new assembly or modifies the
existing assembly in the following manner:
 A new folder named XYZ_WithoutMultiBodyParts is created within the
folder where the existing assembly is located.
 The new parts created out of the multiple bodies of part 'X' will be
named X_1, X_2 and so on and these parts will be saved in this
XYZ_WithoutMultiBodyParts folder.
 Similarly, the new parts created out of the multiple bodies of part 'Y'
will be named Y_1, Y_2 and so on and these parts will also be saved in
the same folder.
 The single body part named 'Z' too will be copied into this newly
created folder.
 If you selected Yes (i.e. you chose to create a new assembly with
single body parts), then this newly created assembly will be named
Assembly.sldasm and this file too will be saved in the
XYZ_WithoutMultiBodyParts folder. This new assembly file will
comprise of all new parts (X_1, X_2 etc.; Y_1,Y_2, etc.) created out
the original multi-body parts as well as the single-body parts (Z).
 If you selected No (i.e. you chose to modify the existing assembly
[XYZ.sldasm]), then the existing assembly will be modified to now
contain parts saved within the XYZ_WithoutMultiBodyParts folder.
Effectively, the original multi-body parts will be replaced with their
corresponding parts created out of the multiple bodies.
Thus the newly created assembly or modified existing assembly
containing single body parts will become the active document considered
for nesting process. The single body parts are listed under the Part Data
tab of the Create Nesting Job dialog box.
Complete the nesting process for this assembly by following the general
steps explained in Tutorial 4.
Tutorial 4 – Nesting of Multiple parts based on Thickness
97
CAMWorks Nesting Tutorial
TUTORIAL 5 – NEST BY MATERIAL, NEST BY
THICKNESS
Introduction
This tutorial explains how to nest multiple solid parts of varying thickness
and materials. You will observe how CAMWorks Nesting generates a multiple
layout based on the part material and thickness and performs Preferential
hole filling.
Topic covered in this Tutorial:
 Nesting multiple parts of varying thickness and material
 Preferential hole filling
 Viewing the nested layouts on multiple sheets
Preferential Hole Filling
In this tutorial, we will explore preferential hole filling. In one of the sheet
layouts, you will observe how a smaller part can be nested in the holes of
larger parts resulting in higher sheet utilization and minimal scrap.
STEP 1: Enabling „Preferential Hole Filling‟ functionality
Since the feature of Preferential Hole Filling will be used in this tutorial, it is
imperative that this feature be enabled. The default settings configured in the
DefaultValues.ini file are configured to keep this feature enabled for all the
nesting jobs. If you are unsure about the settings, open the DefaultValues.ini
file and set the PreferHoleFilling flag to „1‟ in order to enable the ‘Preferential
Hole Filling’ feature.
STEP 2: Using „Nest by Folder‟ to open the Assembly
1. Select Nest by Folder option in the CAMWorks Nesting menu bar.
OR
Click on the Nest by Folder button on the CAMWorks Nesting Ribbon Bar.
2. The Browse for folder dialog box opens. Browse to the folder named
Tutorial5 in the following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies
CAMWorks Nesting opens all the parts contained in the folder as an
assembly in the SOLIDWORKS Graphics area.
3. The Create Nesting Job dialog box is displayed. All the parts present in
the assembly are listed in the Part List of the Part data tab.
In the Part list, click on the column heading Part Name to sort the data in
ascending order from A to Z.
98
Tutorial 5 – Nest by Material, Nest by Thickness
CAMWorks Nesting Tutorial
Order the parts in ascending order of Part Names
„Nest by Folder‟ parts listed in the Part List
STEP 3: Define the Part Parameters
Thickness & Material of the parts
The thickness and material of the solid parts extracted from the solid models
is displayed in the Part List.

The part named „Tut5_Part1‟ and „Tut5_Part4‟ have the same material
„Alloy Steel (SS)‟ and thickness (10 mm).
Tut5_Part1.sldprt
Tut5_Part4.sldprt
 The parts „Tut5_Part2‟, „Tut5_Part3‟, „Tut5_Part5‟ and „Tut5_Part6‟
have identical material „Steel‟ and thickness (12.7 mm).

Tut5_Part2.sldprt
Tutorial 5 – Nest by Material, Nest by Thickness
Tut5_Part3.sldprt
99
CAMWorks Nesting Tutorial
Tut5_Part6.sldprt
Tut5_Part5.sldprt
Only parts with identical material and thickness can be nested within the
same sheet. Based on the above observation, it is clear that 2 different
sheets need to be defined to generate nested layouts. Each such sheet
nests parts having the same material and thickness.
Normal Face
No changes are made to the default normal face selection for any of the
parts.
Grain Direction
Leave the Grain direction set to None for all the parts.
Step Angle & Quantity
Set the following quantities for the parts:
Tut5_Part1
Step Angle to be
assigned
900
Quantity to be
assigned
12
Tut5_Part2
900
10
Tut5_Part3
900
11
Tut5_Part4
900
10
Tut5_Part5
900
10
Tut5_Part6
900
9
Part Name
100
Tutorial 5 – Nest by Material, Nest by Thickness
CAMWorks Nesting Tutorial
Setting appropriate Part angle and Quantity for the parts
STEP 4: Defining sheet parameters
To nest all the six parts in the part list, three different sheets of varying
thickness and material need to be added to the sheet list.
Adding Standard Sheet
Since the parts „Tut5_Part1.sldprt‟ and „Tut5_Part4.sldprt‟ have identical
material [Alloy Steel (SS)] and thickness (10 mm), they can be nested
within the same sheet.
To add a standard sheet to nest these parts, following are the steps:
1. Click on the Sheet Data tab. In the Sheet list, click on Select to add
sheet.
2. By default, the thickness of the first part listed in the Part list is
10mm. In case this value is not displayed in the thickness field, assign
a 10mm value.
3. By default, the material of the first part listed in the Part list is „Alloy
Steel (SS)‟. In case this value is not displayed in the material field,
type the material name into the field.
Tutorial 5 – Nest by Material, Nest by Thickness
101
CAMWorks Nesting Tutorial
4. To add a standard sheet, select the „S13 (10‟ X 4‟) – Len: 3000 mm
Width: 1200 mm‟ sheet from the Standard Size dropdown List.
5. In the Quantity field, assign a quantity of „1‟.
6. Click Add Sheet to add the sheet to the Sheet list.
Adding Standard Sheet 2
Next, the parts „Tut5_Part2‟, „Tut5_Part3‟, „Tut5_Part5‟ and „Tut5_Part6‟
have identical material [Steel] and thickness [12.7mm]. They can be nested
on the same sheet.
Follow the same steps i. to vi. given above to add the standard sheet to nest
these parts. However, in step ii, choose the standard sheet of size „S24 (12‟
X 10‟) – Len: 3600 mm Width: 3000 mm‟.
In step iii, a thickness of 12.7 mm needs to be assigned to the sheet.
Observe that CAMWorks Nesting already displays 12.7 mm as the default
thickness.
In step iv, you need to assign the material of the sheet as Steel. Observe
that CAMWorks Nesting already now displays this material in the material
field.
Adding multiple sheets of varying thickness and material to the sheet list
102
Tutorial 5 – Nest by Material, Nest by Thickness
CAMWorks Nesting Tutorial
STEP 5: Selecting a machine with Single Tool Head for
the Nesting Process
1. Click on the Multi Head Options tab.
2. In the Machine Data group box, ensure that the Machine selected is
SingleTHMachine. The Number of tool heads for this machine should
be „1‟.
Selecting SingleTHMachine as the machine ensures the nesting job is
executed considering a single tool head and not multiple tool heads.
STEP 6: Define Nesting Parameters
1. In the Nesting Data Group Box, set a Part to Part distance of 5 mm and a
Part to Sheet distance of 5 mm.
2. Select Fast Nesting as the Nesting method.
3. Click OK to execute the nesting process.
4. Leave the checkbox Save output as dxf checked. Use the
button next
to the Output assembly field to assign the folder location where the
nested layouts will be saved in the dxf file format.
Step 7: Generating the Nested Layout
The nested layouts are generated in two file formats:
 Assembly file format (.sldasm)
 Drawing Exchange Format (.dxf)
Saving Files in the .dxf format
Browse to the folder location assigned for saving the nested layouts in .dxf
format. Since two nested layouts were generated, observe that two separate
files have been saved in the .dxf format in this folder.
Summary File
The Summary text file indicates that all the parts have been nested. Observe
that the smaller parts have been nested in the holes of the larger parts.
Tutorial 5 – Nest by Material, Nest by Thickness
103
CAMWorks Nesting Tutorial
Summary Text File
Viewing the Nested Layouts
Use the SOLIDWORKS/CAMWorks Solids Configurations tree to view the
Nested layouts generated.
SOLIDWORKS Configuration Tree
104
Tutorial 5 – Nest by Material, Nest by Thickness
CAMWorks Nesting Tutorial
Nesting layout (Tut5_Part2.sldprt, Tut5_Part3.sldprt, Tut5_Part5.sldprt and Tut5_Part6.sldprt)
Nesting layout with preferential hole filling (Tut5_Part1.sldprt & Tut5_Part4.sldprt)
Tutorial 5 – Nest by Material, Nest by Thickness
105
CAMWorks Nesting Tutorial
TUTORIAL 6 – NESTING WITH MULTIPLE TOOL
HEADS
Introduction
This tutorial explains how to nest multiple solid parts of the same thickness
and material in two or more identical layouts on a sheet simultaneously by
using multiple tool heads.
Topic covered in this Tutorial:
 Activating the functionality of nesting with multiple tool heads.
 Nesting parts within a sheet using multiple tool heads to create
identical nested regions.
STEP 1: Open the Assembly
Open the assembly file Tutorial_6_Multi_Tool.sldasm in the folllwoing
folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial6
Tutorial_6_Multi_Tool.sldasm
This assembly is made up of three parts.
Tutorial_6_Part1.sldprt
106
Tutorial_6_Part2.sldprt
Tutorial_6_Part3.sldprt
Tutorial 6 – Nesting with Multiple Tool Heads
CAMWorks Nesting Tutorial
STEP 2: Enabling the option of flattening the sheet metal
parts
In this tutorial, you will nest the sheet metal part based on its dimensions after
flattening. The default settings configured in the DefaultValues.ini file ensure
that sheet metal parts are flattened before the nesting job is executed. If you
are unsure about the settings, open the DefaultValues.ini file and set the
FlattenSheetMetalPart flag to „1‟ in order to activate the option of flattening.
STEP 3: Define the Part Parameters
1. Select Create Nesting Job from the CAMWorks Nesting menu. All the
parts which constitute the assembly are listed in the Part List of the Part
data tab of this dialog box.
Defining the Part Parameters
2. Observe the Thickness and the Material of all the three parts are
identical. These default values will remain unchanged. Identical thickness
and material will enable nesting of these parts in the same sheet.
3. Assign the Quantity „100‟ to all the three parts.
4. Assign a Step Angle of 90 degrees to all the three parts.
5. Assign the material as „Steel‟ for all the parts.
6. Leave the Grain Direction set to None for all the three parts.
Tutorial 6 – Nesting with Multiple Tool Heads
107
CAMWorks Nesting Tutorial
STEP 4: Define the Sheet Parameters
In this exercise, you will use a custom sheet with a length of 3000mm and
width of 2900mm to nest the parts.
1. Click on the Sheet Data tab of the Create Nesting Job dialog box.
Defining the Sheet Parameters for Custom size sheet
2. In the Sheet list, click on Select to add sheet.
3. By default, the thickness of the first part given in the Part list is given
as the Thickness field (2mm). Leave this parameter value as it is.
4. By default, the material of the first part listed in the Part list is given in
the Material field (Steel). Leave this parameter value as it is.
5. In the Quantity field, assign a quantity of „1‟.
6. Leave the Grain Direction set to None and the Assembly Template set
to Default.
7. To add a custom size sheet, select the Custom size option. Assign a
Length of 3000mm and a Width of 2900mm.
8. Click Add Sheet to add the sheet to the Sheet list.
STEP 5: Define the Multi head options parameters
To nest using multiple tool heads, it is necessary to assign appropriate
values to the parameters associated with nesting using multiple tool heads.
The Multi head options tab of the Create nesting Job dialog box allows you
assign/edit these parameters.
1. Click on the Multi head options tab of the Create Nesting Job dialog
box.
108
Tutorial 6 – Nesting with Multiple Tool Heads
CAMWorks Nesting Tutorial
Defining the Multi head options parameters for nesting with multiple tool heads
2. The Sheet list in this dialog box lists the Custom size sheet added in
the Sheet Data tab. The parameters associated with nesting using
multiple tool heads have to be defined separately for each sheet listed
in the Sheet list.
3. Highlight the lone sheet listed in the Sheet list.
4. In the Machine dropdown list, select MachineName1 for the machine.
In case your Machine list has already been customized to suit your
facility‟s requirements, then MachineName1 will not be listed. To
proceed with the tutorial, you can do one of the following:
i. Create a dummy machine named MachineName1 with associated
parameters in the Machine.ini file so that the machine is listed
here in this list. This is explained in the section Adding a new
machine to the Machine.ini file.
ii. Select another machine from the Machine list which has at least
5 tool heads. All the other parameters can be edited to suit the
requirements of this tutorial before the nesting job is executed.
5. The default values for the parameters associated with MachineName1
will be displayed. (These default values are defined in the Machine.ini
file.)
The default values associated with the parameters are:
a. Number of Tool heads:
5
b. Rail Direction:
X
c. Multi-tool head nesting type:
Fixed tool head distance
d. Tool head distance:
500mm
In case you selected a machine other than MachineName1, edit the
parameters to assign them the values/options given above.
Tutorial 6 – Nesting with Multiple Tool Heads
109
CAMWorks Nesting Tutorial
6. In this tutorial, the nesting with multiple tools will be executed using
the default parameter values associated with the machine
MachineName1.
STEP 6: Define Nesting Parameters
1. In the Nesting Data Group Box, set a Part to Part distance of 10 mm and
a Part to Sheet distance of 10 mm.
2. Fast Nesting is the default Nesting type. Note that Optimal Nesting option
has been disabled.
3. Use the
button next to the Output assembly field to specify where the
nested layout assembly file and the Summary text file that are generated
will be saved.
4. Leave the Create separate assembly checkbox unchecked.
5. Click OK to execute the nesting process.
Step 7: Generating the Nested Layout
The Summary text file indicates that the prescribed quantities for all the
parts have been nested within the sheet.
Nesting Results Summary Text file
The nested layout generated after executing the nesting job is given on the
next page.
110
Tutorial 6 – Nesting with Multiple Tool Heads
CAMWorks Nesting Tutorial
Observe the nested layout. The five tool heads used create 5 identical
nested layouts in the „X‟ direction.
Parts which remain
to be machined
5
4
3
2
1
Nesting layout with 5 identical regions created using 5 tool heads
20 instances of the first part (Tutorial_6_Part1.sldprt), 20 instances of the
second part (Tutorial_6_Part2.sldprt) and 5 instances of the third part
(Tutorial_6_Part3.sldprt) are nested in each identical nesting region.
Thus, 100 instances of the first two parts are nested within the 5 identical
regions. Only 25 instances of the third part are nested within the identical
regions. The remaining 75 instances can be nested in the remnant sheet left
after nesting the 5 regions.
Tutorial 6 – Nesting with Multiple Tool Heads
111
CAMWorks Nesting Tutorial
TUTORIAL 7 – NESTING IMPORTED SHEET METAL
COMPONENTS WITH BENDS
Introduction
This tutorial explains how to unfold imported 3D sheet metal components
with bends using various menu options available within CAMWorks Nesting.
Topic covered in this Tutorial:
 Using the „Unfold Imported Bodies‟ dialog box
 Using the „Enable Auto Unfold‟ option
 Using the „Intelligent Unfold‟ command 
 Using the „Unfold All Parts‟ command
The functionality of Unfolding Sheet Metal Parts
CAMWorks Nesting supports nesting of imported part models. If the sheet
metal parts to be nested contain bends, then these parts should ideally be
unfolded before the nesting job is executed.
Most native sheet metal parts (parts created using the solid modeler of
SOLIDWORKS or CAMWorks Solids) as well as imported sheet metal parts
can be unfolded using the in-built functionality of the Solid Modeler itself.
However, sheet metal parts with complex architectures can sometimes be
flattened/unfolded incorrectly.
CAMWorks Nesting provides a more robust functionality for unfolding both
imported and native sheet metal parts. Sheet metal parts that are unfolded
incorrectly by the Solid Modeler can be unfolded correctly using this
functionality.
The ‘Unfold Imported Bodies’ dialog box
The CAMWorks Nesting functionality for unfolding both native and imported
sheet metal parts is provided in the form of ‘Unfold Imported Bodies’ dialog
box. This dialog box allows you to select sheet metal parts with bends to be
unfolded and assign parameters associated with unfolding sheet metal parts.
Note: The functionality of Unfolding is meant for sheet metal parts only. If the part(s)/
assembly to be nested contain imported solid parts, then these imported solid
parts too will be displayed in the „Unfold Imported Bodies‟ dialog box. Ensure that
you unselect the solid parts from the list of parts to be unfolded.
112
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
Commands to Invoke „Unfold Imported Bodies‟ dialog
box
1. The ‘Enable Auto Unfold’ Option
Click on the CAMWorksNesting menu. Observe that the Enable Auto
Unfold option is checked by default.
„Enable Auto Unfold‟ option in CAMWorksNesting menu

When the Enable Auto Unfold option is checked and the Create Nesting
Job command is executed for part(s)/assembly containing one or more
imported bodies, CAMWorks Nesting will automatically display the
Unfold Imported Bodies dialog box. Use this dialog box to select the
bodies to be unfolded and set the parameters associated with
unfolding.

When the Enable Auto Unfold option is not checked and the Create
Nesting Job command is executed for a part(s)/assembly containing
imported bodies, CAMWorks Nesting will display a warning message
stating that the part contains imported bodies and whether you wish to
unfold these imported bodies.
CAMWorks Nesting message displayed when part or assembly contains imported sheet
metal bodies with folds

If the part(s)/assembly to be nested comprises of one or more
sheet metal bodies with bends, then click Yes to unfold the
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
113
CAMWorks Nesting Tutorial
imported sheet metal parts. The Unfold Imported bodies dialog
box will be displayed. All the imported parts will be listed in the
dialog box. Note that native sheet metal parts with bends, if
present in the part(s)/assembly o be nested, will not be listed in
this dialog box. These native parts will either be unfolded/remain
folded based on settings for Flattening sheet metal parts in the
DefaultValues.ini.

If the part(s)/ assembly to be nested comprises of only solid parts
[i.e. it does not have a single sheet metal part with bend(s)], then
click No. (CAMWorks Nesting does not support unfolding of solid
parts.) The „Create Nesting Job‟ dialog box will be displayed.

If you select the Don’t show this message again option,
CAMWorks Nesting will remember your preference.
2. The ‘Intelligent Unfold’ Command
Function
The Solid Modeler (SOLIDWORKS/CAMWorks Solids) can only unfold
native sheet metal parts with bends. Imported sheet metal parts with
bends cannot be unfolded using Solid Modeler functionality. The
„Intelligent Unfold‟ command is ideal for nesting parts/assemblies
comprising imported sheet metal part(s) with bends.
Command Execution
1. Clicking on the „Intelligent unfold‟ command in the CAMWorksNesting
menu opens the Unfold Imported Bodies dialog box.
2. Alternatively, clicking on the Intelligent Unfold button on the
CAMWorks Nesting Ribbon Bar also opens this dialog box.
„Intelligent Unfold‟ command in
CAMWorksNesting menu
„Intelligent Unfold‟ button in the
CAMWorks Nesting Ribbon Bar
How it works
When the Unfold Imported Bodies dialog box is opened using the
Intelligent Unfold command, only imported parts will be listed. Any native
114
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
part present will not be listed. If there are any imported solid bodies
listed in the grid, ensure that you unselect them to avoid unfolding. Use
this dialog box to set parameters associated with flattening the parts
before nesting.
Note:
If you open the „Unfold Imported Bodies‟ dialog box using either the
„Intelligent Unfold‟ or „Create Nesting Job‟ command, then only imported
sheet metal parts with bends will be listed in the dialog box. Native sheet
metal parts with bends, if present, will not be listed.
When you click „OK‟ button of this dialog box:
1. The imported sheet metal parts selected for unfolding will be unfolded
based on user-defined parameters input in this dialog box.
2. Native sheet metal bodies with bends, if present in the
parts/assembly, will either be unfolded/remain folded based on
settings for Flattening sheet metal parts in the DefaultValues.ini. The
Solid Modeler‟s functionality for unfolding will be applied for unfolding
the native sheet metal parts.
Next Step
After unfolding the imported parts using this dialog box, you can click on
the „Create Nesting Job‟ menu option to proceed with the nesting process.
3. The ‘Unfold All Parts’ Command
Function
The Solid Modeler (SOLIDWORKS/CAMWorks Solids) has in-built
functionality for unfolding native sheet metal parts with bends. CAMWorks
Nesting too contains an in-built functionality to unfold both native and
imported sheet metal parts.
However, certain native sheet metal parts can sometimes be incorrectly
unfolded by the Solid Modeler. Such parts can then be alternatively
unfolded using the CAMWorks Nesting functionality.
The „Unfold All Parts‟ command is ideal when you wish to unfold all sheet
metal parts with bends (both native and imported) using the CAMWorks
Nesting functionality of unfolding.
When this command is executed:
1. The imported sheet metal parts will be unfolded using the CAMWorks
Nesting functionality of unfolding.
2. For native sheet metal parts, you can select/unselect the native sheet
metal parts to be unfolded using this functionality. Any unselected
native part will then be unfolded using the Solid Modeler functionality
of unfolding.
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
115
CAMWorks Nesting Tutorial
Command Execution
1. Clicking on the „Unfold All Parts‟ command in the CAMWorksNesting
menu opens the Unfold Imported Bodies dialog box.
2. Alternatively, clicking on the Unfold All Parts button on the CAMWorks
Nesting Ribbon Bar also opens this dialog box.
„Unfold All Parts‟ command in CAMWorksNesting
menu
„Unfold All Parts‟ button in the
CAMWorks Nesting Ribbon Bar
How it works
When the Unfold Imported Bodies dialog box is opened using the Unfold
All Parts command, both imported parts as well as native parts will be
listed within the dialog box.
 If there are any imported solid bodies listed in the grid, ensure that
you unselect them to avoid unfolding.
 If there are any native sheet metal parts that you do not wish to
unfold using the CAMWorks Nesting functionality for unfolding,
ensure that you unselect such parts. Use this dialog box to set
parameters associated with unfolding the sheet parts before
nesting.
Note: If you open the „Unfold Imported Bodies‟ dialog box using the „Unfold All Parts‟
command, then both imported sheet metal parts with bends as well as native
sheet metal parts with bends will be listed in the dialog box.
When you click „OK‟ button of this dialog box:
1. All the imported sheet metal parts selected for unfolding will be
unfolded based on user-defined parameters input in this dialog box.
2. All native sheet metal parts listed in the dialog box which were
selected for unfolding will be unfolded using the CAMWorks Nesting
functionality for unfolding.
3. If any native sheet metal part listed in the dialog box was deselected
from unfolding, then that part will be either be unfolded/remain folded
based on settings for Flattening sheet metal parts in the
116
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
DefaultValues.ini. If unfolded, then the Solid Modeler‟s functionality for
unfolding will be applied for unfolding the native sheet metal parts.
Next Step
After unfolding the sheet metal parts using this dialog box, you can
execute the „Create Nesting Job‟ command to proceed with the nesting
process.
STEP 1: Open the Assembly
Open the assembly file Tutorial7_Unfold_Assembly.sldasm in the
following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial7
Tutorial7_Unfold_Assembly.sldasm
This
i.
ii.
iii.
assembly comprises of three sheet metal parts:
Tutorial_7a_Native.sldprt
(native part)
Tutorial_7b_Imported.sldprt
(imported part)
Tutorial_7c_Imported.sldprt
(imported part)
Tutorial_7a_Native.sldprt
Tutorial_7b_Imported.sldprt
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
Tutorial_7c_Imported.sldprt
117
CAMWorks Nesting Tutorial
STEP 2: Unfolding the Parts with bends
1. In the CAMWorksNesting menu, ensure that there is no check placed
against the Enable Auto Unfold option.
2. Click on the menu item Create Nesting Job command in the
CAMWorksNesting menu.
OR
Click on the Create Nest Job button in the CAMWorks Nesting Ribbon Bar.
3. Since the assembly to be nested contains imported sheet metal parts with
bends, CAMWorks Nesting will display a message stating that the part
contains imported bodies and whether you want to unfold these bodies.
Click Yes.
Note: If the parts/assembly to be nested contains only native sheet metal parts with
bends, then this message won‟t be displayed. Instead, CAMWorks Nesting will
directly display the „Create Nesting Job‟ dialog box. The native parts will be
unfolded/remain folded depending upon the settings in the DefaultValues.ini
file.
4. The Unfold Imported Bodies dialog box is displayed. This dialog box is
used to facilitate the unfolding of sheet metal parts and associated
parameters before proceeding with a nesting job. All the imported parts
comprising this assembly are listed Unfold tab of this dialog box. In this
case, the sheet metal parts Tutorial_7b_Imported.sldprt and
Tutorial_7c_Imported.sldprt will be listed.
5. Observe that the sheet metal part named Tutorial_7a_Native.sldprt is
not listed in this grid. This is because Unfold Imported Bodies dialog box
is displayed using the „Intelligent Unfold‟ command lists only imported
parts. This native part will either be automatically unfolded or remain
unfolded depending upon the option settings for Flattening sheet metal
parts in the DefaultValues.ini. If unfolded, then the Solid Modeler
functionality for unfolding will be used.
Note: Native sheet metal parts will be listed in the Unfold Imported Bodies dialog box
only if the „Unfold all Parts‟ command is used to invoke this dialog box. Native
parts selected for unfolding in the Unfold Imported Bodies dialog box will be
unfolded using the CAMWorks Nesting functionality for unfolding instead of
the default Solid Modeler functionality.
6. In the Part List grid, remove the check
from the checkboxes of those
imported parts that you do not wish to unfold. In this tutorial, you will
unfold both the imported parts. Hence, do not remove the check from the
check boxes.
118
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
The „Unfold Imported Bodies‟ dialog box
4. Assign the following values to the Unfold Parameters:
i.
ii.
Thickness & Material: CAMWorks Nesting extracts the part
parameter of Thickness and Material from the Solid Part and
displays it in the Thickness and Material fields respectively as
default thickness and material for the part. The thickness of the
part, as extracted from the solid part, is displayed as 2mm and
the material is „steel‟. Leave these values as they are.
Unfold Type:
a) K-factor: CAMWorks Nesting displays K-factor value 0.5 as
default for unfold of the part, you can change the K-factor.
b) Bend Table: Optionally you can also select the bend table.
In this tutorial, we will use the default value of the K-factor for
both the sheet metal parts.
iii.
Reference face: By default, CAMWorks Nesting chooses the face
with the largest area as the Reference Face. In this tutorial, the
bottom face of the solid part is chosen by default. The normal
direction is indicated by an arrow in the graphics area.
5. Click the OK button of this dialog box to unfold the imported parts. The
unfolded parts are displayed in the graphics area of
SOLIDWORKS/CAMWorks Solids.
6. The Create Nesting Job dialog box is now displayed.
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
119
CAMWorks Nesting Tutorial
STEP 3: Defining the Part, Sheet & Nesting Parameters
Part Data Tab
In the Part data tab of the Create Nesting Job dialog box, assign the
following values to the parameters:
1. Thickness & Material: Observe that the Thickness and the Material of
all the three parts are identical. These default values will remain
unchanged. Identical thickness and material will enable nesting of these
parts in the same sheet.
2. Quantity: Assign the Quantity of 40 to all the three parts.
3. Step Angle: Assign a Step Angle of 90 degrees to all the three parts.
4. Grain Direction: Leave the Grain direction set to None for all the three
parts.
Defining the Individual Part Parameters in the „Create Nesting Job‟ dialog box
Sheet Data Tab
In this tutorial, we will use a standard sheet of size S3 [Length = 1800mm;
Width = 1800mm] to nest all the three parts.
Click on the Sheet data tab of the Create Nesting Job dialog box and assign
the following values to the parameters:
1. In the Sheet list grid, click on Select to add sheet.
2. Thickness & Material: By default, the thickness and material of the
first part given in the Part list grid of the Part Data tab is assigned as the
thickness and material in the Thickness (2mm) and Material (Steel) fields
respectively. Leave these parameter values as it is.
3. Quantity: In the Quantity field, assign a quantity of ‘1’.
4. Grain Direction: Leave the Grain direction set to None.
5. Assembly Template: Leave the Assembly Template set to Default.
6. Adding a Standard Sheet: To add a Standard size sheet,
120
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
i.
Select the Standard size option.
ii.
In the Standard size dropdown list, select S3 (6” X 6”)
7. Click on the Add sheet button to add the sheet to the Sheet List.
Defining the Sheet data and Nesting Data Parameters in the Create Nesting Job dialog box
Nesting Parameters
In the Nesting Data group box, assign the following parameters:
1. Set a Part to Part distance of 10 mm and a Part to Sheet distance of 10
mm.
2. Fast Nesting is the default Nesting type.
3. Use the
button next to the Output assembly field to specify where the
nested layout assembly and the Summary text file that are generated will
be saved.
4. Leave the Create separate assembly checkbox unchecked.
5. Click OK to execute the nesting process.
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
121
CAMWorks Nesting Tutorial
Step 4: Generating the Nested Layout
The Summary text file indicates that the prescribed quantities for all the
parts have been nested within the sheet.
Nesting Results Summary Text file
The nested layout assembly generated after executing the nesting job and
the Summary Results file are stored in the same location as the parts to be
nested.
All 40 instances of the each sheet metal part are nested within the same
sheet.
Nesting layout generated for all the three sheet metal parts comprising the assembly
122
Tutorial 7 – Nesting Imported Sheet Metal Components with Bends
CAMWorks Nesting Tutorial
TUTORIAL 8 – UNFOLDING IMPORTED 3D SHEET
METAL COMPONENTS WITH FAULTY SURFACES
Introduction
The previous tutorial (Tutorial 7) explained how to unfold imported 3D sheet
metal components using the „Unfold Imported Bodies‟ dialog box before
nesting such parts.
However, CAMWorks Nesting cannot fully unfold imported sheet metal parts
if such parts have faulty bodies or surfaces. Tutorial 8 explores how to nest
imported sheet metal parts containing faulty bodies or surfaces.
It is recommended that you go through the concepts explained in Tutorial 7
before commencing with this tutorial.
Topic covered in this Tutorial:
 Selective Unfolding of faulty parts
 Using the „Unfold Imported Bodies‟ dialog box to unfold imported sheet
metal parts with faults
STEP 1: Open the Assembly
Open the assembly file Tutorial8_Unfold_Assembly.sldasm in the
following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Examples\Tutorials\
Assemblies\Tutorial8
Tutorial8_Unfold_Assembly.sldasm
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
123
CAMWorks Nesting Tutorial
This assembly comprises of two identical sheet metal parts:
i.
Tutorial_8a_Faulty.sldprt
(imported part)
ii.
Tutorial_8b_Non-Faulty.sldprt
(imported part)
Though these two parts are identical, one of the parts has a faulty body.
STEP 2: Executing the „Intelligent Unfold‟ command
1. In the CAMWorksNesting menu, click on the menu item Intelligent Unfold.
2. Since one of the parts comprising this assembly has a faulty body,
CAMWorks Nesting will display a message stating that the assembly
contains faulty parts/surfaces and that you will need to select/deselect
faces directly on the model for unfolding.
CAMWorks Nesting message indicating the presence of
faulty imported parts with bends
3. Click OK to close this dialog box and proceed with nesting.
If you don‟t wish to see this error message again in future nesting jobs,
select Don’t show this message again before you click OK.
If you click CANCEL by selecting the close button on the top right hand
corner of this message, then the job will not proceed for nesting.
4. The Unfold Imported Bodies dialog box is displayed. All the imported
parts with bends that constitute this assembly are listed Unfold tab of this
dialog box. The faulty sheet metal part is highlighted in red colored font
while the non-faulty part will be displayed in the default black colored
font.
STEP 3: Selective unfolding of imported parts
As explained in Step
2, the „Unfold Imported Bodies‟ dialog box is used to
facilitate the unfolding of imported sheet metal parts and associated
parameters before proceeding with a nesting job.
124
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
CAMWorks Nesting Tutorial
Following are the steps to open the „Unfold Imported Bodies‟ dialog box to
unfold the sheet metal parts and assign associated parameters:
1. Observe the Part Quality column in the Unfolded Imported Bodies dialog
box. This column indicates which imported parts are faulty and which are
non-faulty.
The „Unfold Imported Bodies‟ dialog box
2. Highlight the Faulty part in the Part List grid of this dialog box. Observe
that a Status message is displayed in the bottom left hand corner of
SOLIDWORKS/CAMWorks Solids.
Status message displayed when a faulty part is highlighted in the „Unfold Imported
Bodies‟ dialog box
3. In the graphics area, observe the faulty part. Notice that the certain bent
edges of the faulty part are highlighted in green. Rotate the assembly so
that the bottom surfaces are visible in order to get a clear view.
4. In the graphics area, observe the faulty sheet metal part
(Tutorial_8a_Faulty.sldprt). Notice that the certain bent edges of the
faulty part are highlighted in green. All the faces tangentially connected
to the reference face and will be highlighted in dark green colors on the
faulty part. The default reference face for a part is always the surface
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
125
CAMWorks Nesting Tutorial
with the largest area. This reference face is highlighted in light olive
green color.
Faulty part
Reference face
Non- faulty part
Tangentially connected faces highlighted in green on the
faulty part
5. As indicated by the status message, only the highlighted green faces in
the faulty part will be processed for unfolding while non-faulty part(s) will
be unfolded automatically.
6. You can remove all the faces thus selected for unfolding by clicking on the
reference face of the part in the graphics area. (The reference face is the
one with the normal arrow and always highlighted in light olive green
color). When you click on the highlighted reference face, all the selected
faces, including the reference face, are discarded.
Deselected
reference face
All highlighted green faces are deselected from unfolding
when you click on the reference face
126
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
CAMWorks Nesting Tutorial
7. Observe the Unfold Imported Bodies dialog box. Since the faulty part no
longer has a reference face, the Reference Face field in this dialog box
displays a message prompting you to select a reference face on the part.
Message in Ref Face column prompting user to select a reference face
8. Rotate the part so that the top
surfaces are once again visible. In
the graphics area, pick the planar
surface on the faulty part as shown in
the image on the right. This planar
surface will become the reference
face (highlighted in light olive green
color) for the faulty part. All the
corresponding faces tangent to this
reference face will be highlighted in
green. Faces highlighted in green
indicate that they will be unfolded.
Click on this
face to select it
as reference
face
9. If you select one of the highlighted green surfaces, then all the
highlighted green faces which are adjacent to the selected face and also
disconnected from the
Selected bent
reference face will be
face discarded
discarded from unfolding.
For example, click on the
bend adjacent to the
reference face as shown in
the image on the left.
Observe that this bent
surface as well as the planar
face that was adjacent and
connected to it was
discarded.
Adjacent face
discarded
10. In the graphics area, click
on the bent face of the faulty part that you deselected in the previous
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
127
CAMWorks Nesting Tutorial
step. Observe that this face and its adjacent face (which was
disconnected from the reference face) are once again highlighted.
Selected face
highlighted
Adjacent face
also selected
Click on this
face
11. To add faces for unfolding to the set of green faces already highlighted,
click on that desired face in the graphics area. This action also selects all
faces tangent to the selected face for unfolding.
Selected face
added
Select this face for
addition
Faces tangent to selected
face are also selected
When you select a non-highlighted face for addition, all faces tangent to this face are also
selected for unfolding
12. In the Unfold Imported Bodies dialog box, assign a thickness of 3mm to
the faulty part.
13. Click the OK button of this dialog box to unfold the imported parts.
CAMWorks Nesting will check the imported parts for the number of
disconnected face chains. If the selected part still retains more than one
disconnected face chain, then an error message will be displayed
prompting you to remove unwanted face chains. The parts won‟t be
128
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
CAMWorks Nesting Tutorial
unfolded and the Unfold Imported Bodies dialog box will remain
displayed.
Error message dialog box
14. This error message is displayed because two faces you selected as
references faces for the faulty part do not form a single face chain. The
presence of a gap creates two face chains. For imported sheet metal
parts, CAMWorks Nesting can unfold only a single face chain. If multiple
disconnected face chains are manually selected by you, then this error
message regarding the presence of multiple face chains will be displayed
and the nesting process will not proceed further. Observe the non-faulty
part. There is only a single face chain in this part.
For imported sheet metal parts containing bends which are to be unfolded
before nesting, CAMWorks Nesting can only unfold any one single face
chain. Multiple face chains cannot be unfolded and thereby cannot be
nested.
Gap
Face Chain 2
Face Chain 1
Click on this face to
deselect Face Chain 2
CAMWorks Nesting cannot unfold an imported sheet metal part with bends when
multiple face chains are present
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
129
CAMWorks Nesting Tutorial
15. To proceed with nesting, you need to ensure that only one face chain is
selected on the faulty part. Since there are two face chains present,
deselect one of the face chains by clicking on face chain with the smaller
reference area as shown in the above image.
16. Click on the OK button of the Unfold Imported Bodies dialog box.
Observe that for the non-faulty imported part, its entire body is
flattened. For the faulty part, only the faces highlighted in green are
flattened. The Create Nesting Job dialog box is displayed.
STEP 4: Executing the Nesting Job
Part Data Tab
In the Part data tab of the Create Nesting Job dialog box, assign the
following values to the parameters:
1. Thickness & Material: Observe that the Thickness and the Material of
all the two parts are identical. These default values will remain
unchanged. Identical thickness and material will enable nesting of these
parts in the same sheet.
2. Quantity:
Assign a Quantity of 80 to part named Tutorial_8a_Faulty.
Assign a Quantity of 65 to part named Tutorial_8b_Non-Faulty.
3. Step Angle: Assign a Step Angle of 90 degrees to both the parts.
4. Grain Direction: Leave the Grain direction set to None for both the
parts.
Sheet Data Tab
In this tutorial, we will use a customized sheet [Length = 2200mm; Width =
2200mm] to nest both the imported parts.
Click on the Sheet data tab of the Create Nesting Job dialog box and assign
the following values to the parameters:
1. In the Sheet list grid, click on Select to add sheet.
2. Thickness & Material: By default, the thickness and material of the
first part given in the Part list grid of the Part Data tab is assigned as the
thickness and material in the Thickness (3mm) and Material (Steel) fields
respectively. Leave these parameter values as it is.
3. Quantity: In the Quantity field, assign a quantity of ‘1’.
4. Grain Direction: Leave the Grain direction set to None.
5. Assembly Template: Ensure that the Assembly Template is set to
Default.
6. Adding a Custom size Sheet: To add a Custom size sheet,
130
i.
Assign a length of 2200mm in the Length field.
ii.
Assign a width of 2200mm in the Width field
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
CAMWorks Nesting Tutorial
7. Click on the Add sheet button to add the sheet to the Sheet List.
Nesting Parameters
In the Nesting Data group box, assign the following parameters:
1. Set a Part to Part distance of 10 mm and a Part to Sheet distance of 10
mm.
2. Fast Nesting is the default Nesting type.
3. Use the
button next to the Output assembly field to specify where the
generated nested layout assembly file and the Summary text file will be
saved.
4. Leave the Create separate assembly checkbox unchecked.
5. Click OK to execute the nesting process.
Step 5: Generating the Nested Layout
The Summary text file indicates that the prescribed quantities for all the
parts have been nested within the sheet.
Nesting Results Summary Text file
The nested layout assembly generated after executing the nesting job and
the Summary Results file are stored in the folder location specified in the
Output assembly field of the Nesting Parameters group box in the Create
Nesting Job dialog box.
The nested layout is given on the next page.
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
131
CAMWorks Nesting Tutorial
Nesting layout generated for the two sheet metal parts comprising the assembly
132
Tutorial 8 – Unfolding Imported 3D Sheet Metal Components with Faulty Surfaces
CAMWorks Nesting Tutorial
TUTORIAL 9 – ASSIGNING ASSEMBLY QUANTITIES
Introduction
CAMWorks Nesting provides a feature wherein, if an Assembly is to be
nested, you can assign a quantity to the Assembly itself within the Part Data
tab of the Create Nesting Job dialog box. Assigning the quantity to the
assembly being nested automatically updates the quantities of its
constituent parts. Thus, the need to assign quantity values to individual
parts of the assembly is eliminated.
In this tutorial, you will explore how assigning quantity value to the
assembly to be nested (or its constituent sub-assemblies) automatically
updates the part quantity values.
Topic covered in this Tutorial:

Enabling the feature for Assigning Assembly Quantities

Assigning Quantity value to the Assembly to be nested

Assigning Quantity values to the sub-assemblies of the assembly

Overwriting the quantities assigned automatically to the individual
parts of an assembly with user-defined quantity values
STEP 1: Open the Assembly
Open the assembly file Parent Assembly.sldasm in the following folder
location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial9
Parent Assembly.sldasm
Tutorial 9 – Assigning Assembly Quantities
133
CAMWorks Nesting Tutorial
Components of the Parent Assembly
This
i.
ii.
iii.
Parent Assembly consists of:
Assembly1,
Assembly2
and
Part 4.
Parent Assembly in the FeatureManager Design tree
Assembly 1 comprises Part1 and
Part2.
Components of Assembly1 highlighted on
Parent Assembly
Assembly1 in FeatureManager Design
tree
134
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
Assembly2 comprises Assembly3 and Part 3.
Components of Assembly2
highlighted on Parent Assembly
Assembly2 in FeatureManager Design
tree
Assembly3 (sub-assembly of Assembly2) comprises Part1 and Part4.
Assembly3 in FeatureManager Design tree
Tutorial 9 – Assigning Assembly Quantities
Components of Assembly3 highlighted on
Parent Assembly
135
CAMWorks Nesting Tutorial
Part4 is a component of Parent Assembly as stated previously.
Part4 highlighted on Parent Assembly
Part4 in FeatureManager Design tree
Thus, the Parent Assembly consists of the following sub-assemblies and
parts:
Parent Assembly
Assembly 1
Part1
Part2
Assembly 2
Assembly3
Part1
136
Part4
Part3
Part4
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
STEP 2: Enabling the option of flattening the sheet metal
parts
The assembly to be nested (Parent Assembly.sldasm) consists of sheet metal
parts. These sheet metal parts need to be unfolded before executing the
nesting job. To nest these sheet metal parts based on its dimensions after
flattening, the option for flattening (unfolding) sheet metal parts needs to be
configured in the DefaultValues.ini file. If you are unsure about the settings,
open the DefaultValues.ini file and set the FlattenSheetMetalPart flag to „1‟ in
order to activate the option of flattening.
STEP 3: Enabling the feature for Assigning Assembly
Quantities
To assign quantity value to the assembly is to be nested (Parent
Assembly.sldasm), the feature for assigning Assembly Quantities needs to be
enabled in in the DefaultValues.ini file. If you are unsure about the settings,
open the DefaultValues.ini file and set the ShowAssemblyQuantity flag to „1‟ in
order to enable the feature of Assigning Assembly Quantities.
STEP 4: Open the „Create Nesting Job‟ Dialog box
1. In the CAMWorksNesting menu
bar, ensure that the Enable Auto
Unfold option is checked.
Activating this option ensures
that sheet metal components to
be nested are automatically
unfolded based on their
dimensions before executing the
nesting job.
2. Select Create Nesting Job from
the CAMWorksNesting menu bar.
OR
„Enable Auto Unfold‟ option checked in
the CAMWorksNesting menu
Click on the Create Nesting Job
button on the CAMWorks Nesting Ribbon bar.
3. The Create Nesting Job dialog box is displayed. Observe that the
parent assembly (Parent Assembly.sldasm), its sub-assemblies as well
as the parts comprising these sub-assemblies have been listed in the
Part Data tab in the Create Nesting Job dialog box.
Tutorial 9 – Assigning Assembly Quantities
137
CAMWorks Nesting Tutorial
Assembly Column
The Parent Assembly and its sub-assemblies are listed in the
Assembly column of the Part List in alphabetical order. The quantity
of the Parent Assembly and its sub-assemblies are listed in the
Quantity column.
Parent Assembly and sub-assemblies listed in the Part List grid of Part Data tab
Part name column
Use the vertical scroll bar to scroll down the Part List. Observe that the
parts constituting the Parent assembly and sub-assemblies are listed
in the Part name column along with associated parameters of
Thickness, Quantity, Material, Rotation type, Angle, etc.
Parts constituting the Parent Assembly and sub-assemblies listed in the Part List
Quantity Column
Observe the Quantity column. The number of instances each subassembly and part appears in the Parent Assembly is listed. In the
Quantity column, ensure that the Quantity for Parent Assembly is „1‟.
(If it isn‟t, double-click on this field in the Part list grid and assign a
quantity of „1‟.)
When the quantity for Parent assembly is „1‟, the quantity of its
constituent sub-assemblies and parts will be as follows:
138
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
Name
Quantity
Parent Assembly
1
Assembly1
1
Assembly2
1
Assembly3
1
Part1
2
Part2
1
Part3
1
Part4
2
Step 5: Changing the quantity of the Parent assembly
1. In the Part list grid, double-click on the Quantity field for Parent
Assembly and change the Quantity to „20‟. Press the Tab button to
shift the focus.
Observe that the Quantity values of all the constituent sub-assemblies
and parts were automatically updated to reflect new values based on
the Parent Assembly.
Name
Original Quantity
New Quantity
Parent Assembly
1
20
Assembly1
1
20
Assembly2
1
20
Assembly3
1
20
Part1
2
40
Part2
1
20
Part3
1
20
Part4
2
20
Analysis
i.
Assembly1 and Assembly2: Both Assembly1 and Assembly2
have one instance each in the Parent Assembly. Hence, when the
quantity of the Parent Assembly is updated, the quantity of this
sub-assembly too will be updated to the same value.
Tutorial 9 – Assigning Assembly Quantities
139
CAMWorks Nesting Tutorial
ii.
Assembly3: Assembly3 has one instance in Assembly2 which in
turn has one instance in the Parent Assembly. Hence, when the
quantity of the Parent Assembly is updated, the quantity of this
sub-assembly too will be updated to the same value.
iii.
Part1: This part has one instance in Assembly1 and another
instance in Assembly3. Hence, two instances of Part1 occur
within the Parent Assembly. Hence, when the quantity of the
Parent Assembly is updated, the quantity of Part1 will be
updated to double of the Parent Assembly‟s quantity value.
iv.
Part2: This part has one instance in Assembly1 which in turn
has one instance in the Parent Assembly. Hence, when the
quantity of the Parent Assembly is updated, the quantity of Part2
will be updated to the same value as that of the Parent
Assembly.
v.
Part3: This part has one instance in Assembly3 which has one
instance in Assembly2 and which in turn has one instance in the
Parent Assembly. Hence, when the quantity of the Parent
Assembly is updated, the quantity of Part3 will be updated to the
same value as that of the Parent Assembly.
vi.
Part4: This part has one instance in Assembly2 and another
instance in the Parent Assembly. Hence, two instances of Part4
occur within the Parent Assembly. Hence, when the quantity of
the Parent Assembly is updated, the quantity of Part4 will be
updated to double of the Parent Assembly‟s quantity value.
Thus, if you change the quantity of the assembly to be nested, then
the quantity of all its constituent sub-assemblies and parts will be
automatically updated to values in sync with quantity of the assembly.
This feature eliminates the need to assign individual quantities to the
constituent parts.
STEP 6: Changing the Quantity of a sub-assembly
1. In the Part list grid, double-click on the Quantity field for Assembly2
and change the Quantity to „22‟. Press the Tab button to shift the
focus.
Observe that the Quantity values for Assembly3, Part1, Part3 and
Part4 were automatically updated to reflect new values based on the
quantity of Assembly2.
140
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
Name
Original Quantity
New Quantity
Parent Assembly
20
20 (unchanged)
Assembly1
20
20 (unchanged)
Assembly2
20
22 (updated)
Assembly3
20
22 (updated)
Part1
40
42 (updated)
Part2
20
20 (unchanged)
Part3
20
22 (updated)
Part4
20
42 (updated)
Analysis
i.
Assembly1: Assembly1 is not a component of Assembly2.
Hence, its Quantity value will remain unchanged.
ii.
Assembly3: Within the Parent Assembly, the sub-assembly
named Assembly3 has only one instance - as component of
Assembly2. Hence, when the quantity of the Assembly2 is
updated, the quantity of this sub-assembly too will be updated
to the same value.
iii.
Part1:
Part1 has 20 instances in Assembly1 and 20 instances in
Assembly3  20 +20 = 40.
Assembly1 is not a component of Assembly2 and hence, the first
20 instances will remain unchanged.
However, Assembly3 has once instance in Assembly2. Hence,
when the quantity of Assembly2 is updated from „20‟ to „22‟, the
quantity of Assembly3 will be updated to „22‟. Since Part4 has
one instance in Assembly3, the quantity component will be
updated to „22‟.
The updated Quantity value for Part1 will be 20 instances in
Assembly1 and 22 instances in Assembly3  20+22 = 42.
iv.
Part2: Part2 is not a component of Assembly2. Hence, its
Quantity value will remain unchanged at „20‟ instances.
v.
Part3: This part has 20 instances in Assembly3 which in turn
has 20 instances in Assembly2. Hence, when the quantity of
Assembly2 is updated to „22‟, the quantity of Part3 will be
updated to the same value as that of the Assembly2.
Tutorial 9 – Assigning Assembly Quantities
141
CAMWorks Nesting Tutorial
Thus, the updated Quantity value for Part3 will be 22 instances
in Assembly3.
vi.
Part4:
Part4 has 20 instances in the Parent Assembly and 20 instances
in Assembly2  20 +20 = 40.
Since the Parent Assembly is not a component of Assembly2, the
first 20 instances will remain unchanged.
However, the next 20 instances are in Assembly2. Hence, when
the quantity of Assembly2 is updated from „20‟ to „22‟, the
quantity of Part4 will also be updated to „22‟.
The updated Quantity value for Part4 will be 20 instances in
Parent Assembly and 22 instances in Assembly2  20+22 = 42.
Note: If you change the quantity of a sub-assembly listed in the Part List grid of the
Part Data tab, then only the quantities of its constituent sub-assemblies and
parts will be updated. The quantities of parts/assemblies which are not a
component of this sub-assembly will remain unchanged.
STEP 7: Changing the Quantity of Parent Assembly
1. In the Part list grid, double-click on the Quantity field for Parent
Assembly and change the quantity to „10‟. Press the Tab button to shift
the focus.
2. Observe that the quantity values of all the constituent sub-assemblies
and parts were automatically updated to reflect new values based on
the Parent Assembly.
Updated Result of the Parts
142
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
Name
Quantity
Parent Assembly
10
Assembly1
10
Assembly2
10
Assembly3
10
Part1
20
Part2
10
Part3
10
Part4
20
Note: If you change the quantity of the Parent assembly, then the quantity of its
constituent sub-assemblies and parts will be recalculated and automatically
updated.
Step 8: Overwriting automatically assigned Quantity
values for Parts with user-defined values
CAMWorks Nesting executes all nesting jobs based on the quantity of the
parts in the Part Data tab (and not based on the quantity of the
Assembly). This is the reason why, when you assign a quantity to an
assembly in the Part Data tab, the quantity of its constituent parts are
updated.
Even when the feature for Assigning Assembly Quantities is active, you
can assign user-defined quantity values to the individual parts in the Part
List grid at any point of time.
1. Double-click on the Quantity field for each of the four parts in the Part
list grid and assign a quantity of „15‟ to each part.
If you proceed further with the nesting job, the quantity considered
will be based on these user-defined values of the parts.
Parts constituting the Parent Assembly and sub-assemblies listed in the Part List
Tutorial 9 – Assigning Assembly Quantities
143
CAMWorks Nesting Tutorial
2. Assign a quantity of „10‟ to the Parent Assembly. Observe that the
quantity of all the sub-assemblies and parts are updated to the values
given in Step 7.
Note: You can update the Part quantities with user-defined quantity values at any
point of time even if the feature for assigning assembly quantities is active.
However, your user-defined values will be overwritten with automatically
assigned values if you once again assign quantity values to the assembly
constituting the parts.
Step 9: Deactivating the feature of assigning assembly
quantities
1. Observe the Assembly column of the Part list grid of the Part data tab.
The arrow mark pointing upwards indicates that the feature for
Assigning Assembly Quantities is currently active.
Arrow mark in the Assembly column pointing upwards
If the feature for assigning assembly quantities is enabled in the
DefaultValues.ini file, then, whenever you open the Create Nesting Job
dialog box, the arrow mark in the Assembly column of the Part list grid
will point upwards indicating that the feature is currently active.
Deactivating the feature only for the current nesting job
1. Left-click on the Assembly column heading. Observe that the arrow
mark in the Assembly column now points downwards. The Part list no
longer displays any assembly in the Assembly column. This column will
be empty. Only parts constituting the assembly will be listed in the
Part list grid. The arrow pointing downwards indicates the feature for
assigning assembly quantities is currently inactive.
Arrow mark in the Assembly column pointing downwards
If you do not wish to use the feature of assigning assembly quantities
for a particular nesting job, then deactivate this feature temporarily
only the current job by having the arrow mark in the Assembly column
point downwards.
144
Tutorial 9 – Assigning Assembly Quantities
CAMWorks Nesting Tutorial
Deactivating the feature for all nesting jobs
1. If you work primarily with parts rather than assemblies or if you
prefer assigning user-defined quantities to the part of an assembly,
you might consider disabling the feature of assigning assembly
quantities.
To disable the feature of assigning assembly quantities, set the
ShowAssemblyQuantity flag in the DefaultValues.ini file to „0‟ and exit
after saving the new settings.
2. With the feature disable, the next time you open the Create Nesting
Job dialog box in order to nest an assembly, the Assembly column will
not be displayed at all in the Part data tab. Only the parts comprising
the assembly will be listed.
3. You can enable this feature again by setting the
ShowAssemblyQuantity flag in the DefaultValues.ini file back to „1‟.
Note: When the feature for assigning assembly quantities is disabled, the Assembly
column will not be displayed in the Part list grid of the Part data tab within the
„Create Nesting Job‟ dialog box.
Complete the nesting job by assigning the remaining Part parameters, Sheet
parameters and Nesting data parameters.
Tutorial 9 – Assigning Assembly Quantities
145
CAMWorks Nesting Tutorial
TUTORIAL 10 – UNFOLDING SHEET METAL
COMPONENTS USING „INTERACTIVE UNFOLD‟
COMMAND
Introduction
The ‘Interactive Unfold’ Command
The „Interactive Unfold‟ command is a means to selectively unfold faces of
parts with bends before nesting the parts. This is done by providing a
reference face and selecting faces to unfold either automatically or manually
with respect to the reference face. Both native as well as imported parts can
be unfolded using this command.
Difference between the various Unfold commands
Given below is table of comparison highlighting the difference in the way a
part is unfolded using the various Unfold commands.
Intelligent
Unfold
Command
Unfold All
Parts
Command
Interactive
Unfold
Command
Create Nest
Job
Command
Faulty Native Part
Non-Faulty Native Part
Faulty Imported Part
Non-Faulty Imported
Part
Legend:
User can change the default reference face and define the chain of faces to unfold.
User can change the default reference face but cannot define chain of faces to unfold.
Command not applicable to native parts
Opens the dialog box associated with „Intelligent Unfold‟.
Part is unfolded using SOLIDWORKS functionality
146
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
The ‘Chain Faces’ option for Unfold commands
The Chain Faces is a checkbox option present in the Unfold dialog box of all
Unfold commands.


When this checkbox option is
enabled, all faces connected
tangentially to the reference
face are automatically
selected.
Chain Faces Option in Unfold dialog box
When this checkbox option is disabled, faces connected tangentially to
the reference face will not be automatically selected. You need to
manually select each face to be unfolded.
If the Chain Faces option is enabled/disabled at any point of time during the unfolding
process, then the changed settings for this option are applicable for all further
selections. However, the faces already selected/deselected will not affected.
Topic covered in this Tutorial:
This tutorial explains how to selectively unfold imported and native 3D sheet
metal parts with non-faulty bodies using the „Interactive Unfold‟ command.
The tutorial explores

Using the „Interactive Unfold‟ with the „Chain Faces‟ option enabled

Using the „Interactive Unfold‟ with the „Chain Faces‟ option disabled
STEP 1: Open the Assembly
Open the assembly file Tutorial10_Interactive_Unfold.sldasm in the
following folder location.
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Assemblies\Tutorial10
Native Part
Imported Part
Tutorial10_Interactive_Unfold.sldasm
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
147
CAMWorks Nesting Tutorial
This assembly comprises of two different sheet metal parts:
i. InteractiveUnfold_Native.sldprt
(Native Part)
ii. InteractiveUnfold_Imported.sldprt
(Imported Part)
Both the parts have non-faulty bodies.
STEP 2: Executing the „Interactive Unfold‟ command
1. Click on the Interactive Unfold command in the CAMWorksNesting
menu. Alternatively, click on the Interactive Unfold button on the
CAMWorks Nesting Ribbon Bar.
„Interactive Unfold‟ button in the
CAMWorks Nesting Ribbon Bar
„Interactive Unfold‟ command
in CAMWorksNesting menu
2. CAMWorks Nesting will display a message stating that you will need to
select/deselect faces directly on the model for unfolding.
-
Click OK to close the
message box and proceed
with unfolding.
-
If you don‟t wish to see this
warning message again in
future nesting jobs, select
the checkbox Don’t show
this message again
before you click OK.
-
148
CAMWorks Nesting Message
If you click CANCEL by selecting the close button
on the top
right hand corner of the message box, then the job will not
proceed for nesting.
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
3. When you click the OK button in the message, the Interactive Unfold
dialog box is displayed. All the parts comprising the assembly (both
native and imported) are listed in the Part List grid of this dialog box.
Since the assembly used in this tutorial consists of one imported part
and one native part, both are listed in the Part List grid.
4. If you do not wish to unfold any particular part listed in the Part List
grid, you can deselect the part from unfolding by unchecking the
checkbox next to the part name in the Part List grid.
In this tutorial, you will unfold both the listed parts. Hence, both the
checkboxes indicating the parts to be unfolded will remain checked.
STEP 3: Selective Unfolding of Parts when „Chain Faces‟
option is enabled
1. Highlight any part in the Part List grid of the Interactive Unfold dialog
box. Observe that a Status message is displayed in the bottom left
corner of the Status bar of SOLIDWORKS/CAMWorks Solids.
Status message displayed when a part is highlighted in the „Interactive Unfold‟ dialog
2. In the Interactive Unfold dialog box, both the non-faulty imported and
non-faulty native parts are listed in the Part List grid and will be
processed through selective unfolding.
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
149
CAMWorks Nesting Tutorial
Interactive Unfold dialog box
3. In the graphics area, observe that a reference face (yellow color) and
faces connected tangentially (green color) to the reference face are
highlighted automatically on both the imported and native parts, thus
indicating the faces to be unfolded.
Imported Part
Native Part
Reference Face
Reference Face
Reference Faces and Faces tangentially connected to the reference
face highlighted in Yellow and Green color respectively
150
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
Deselecting/ Selecting the faces to be unfolded
Faces of the part which are selected for unfolding are highlighted in
green color when the Interactive Unfold dialog box is open. If you wish
to deselect such a face from being unfolded, then you need to mouse
click on that face of the part in the graphics area.

When you deselect a green-colored face, then all the faces which are adjacent
to the deselected face but now disconnected from the reference face due to
this deselection will also be deselected automatically.

Similarly, when you select an unselected face, all the faces adjacent to it that
now connected to the reference face due to the selection will be selected
automatically. Their selection is indicated by green color highlights.
This feature of automatic selection/deselection of faces is possible only
when the Chain faces option is enabled.
In this section, we will explore the selection/deselection of the faces to be
unfolded when the Chain Faces option is enabled.
Consider the native part of the assembly in this tutorial in its default
selection state. For the purposes of illustration the various faces have
been labeled as given below.
Reference
Face
Face b
Face a
Face c
Face d
The following illustrations explain how to select/deselect faces to be
unfolded.
Illustration 1:
i. On the native part, click on Face d as shown in the image on the
right.
ii. Observe that only Face d is deselected. The only face adjacent to Face
d is Face c. However, Face c is not deselected and continues to be
highlighted in green indicating its selection for unfolding. This is
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
151
CAMWorks Nesting Tutorial
because it continues to be connected to the Reference face via Face a
and Face b.
iii. Click on Face d again in order to select it.
Reference Face
Face b
Face a
Face c
Face d
(deselected)
Illustration 2:
i. On the native part, click on Face c in order to deselect it.
ii. Observe that in addition to Face c, the Face d (which is adjacent to
Face c) is also deselected. This is because the deselection of Face c
causes Face d to become completely disconnected from the reference
face.
iii. Click on Face c again in order to select it. The Face d will also be
automatically selected.
Reference Face
Click on Face c
152
Face d
(automatically deselected)
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
Illustration 3:
i. On the native part, click on Face a (the
bent face on the left) in order to
deselect it.
Reference Face
Observe that Face c, (which is adjacent
to Face a) is not deselected. This is
because Face c continues to remain
connected to the Reference face via
Face b.
ii. Now click on Face b in order to deselect
it.
Click on
Face a
Observe that, along with Face b, Face
c and Face d are also deselected.
Face c is adjacent to both Face a and
Face b and connected to the reference
face via these two faces. When both
Face a and Face b are deselected,
Face c is no longer connected to the
Reference face and hence is
automatically deselected.
Click on
Face b
Face d is adjacent to Face c. When
Face c is deselected, then Face d will
no longer be connected to the reference
face and is hence deselected.
iii. Now click on either Face a or Face b in
order to select it once again.
Observe that if you select Face a, then
Face b, Face c and Face d are also
automatically selected. Similarly, if you
selected Face b, then Face a, Face c
and Face d are also selected
automatically for unfolding. This is
because these adjacent faces are then
once again connected to the Reference
face.
Face c
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
Face d
153
CAMWorks Nesting Tutorial
Changing the Reference Face
By default, the reference face is the face with the largest surface area
(highlighted in yellow color when the Interactive Unfold dialog box is open).
All faces tangential to the reference face are selected for unfolding. You can
change the face selected as the reference face.
Deselecting the Reference Face
To deselect the reference face of a part, you need to click on the
Reference face of the part in the graphics area.
1. In the graphics area, click on the Reference face (highlighted in yellow
color) of the native part.
Observe that the Reference face is deselected and all the faces
selected for unfolding are also deselected.
Click on the
Reference Face
2. After deselecting the Reference face, observe the Interactive Unfold
dialog box. Since the native part no longer has a reference face; the
Reference Face field for the native part in this dialog box prompts you
to select a reference face on the part by displaying the message
“Select a Ref Face”.
Message in Ref Face column prompting user to select a reference face
154
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
Selecting a Reference Face
When no face is selected as the reference
face for unfolding on a part, the „Interactive
Unfold‟ dialog box prompts you to select a
face as the Reference face for the particular
part. In order to select a face as the
reference face, click on the desired face in
the graphics area.
1. In the previous step, the reference face of
the native part was deselected. Now, in
the graphics area, pick the planar surface on
Click on the face to select it as
the part as shown in the image on the right.
reference face
This planar surface will become the reference
face (highlighted in yellow color) for the native
part. All the faces tangential to this new reference face will be
highlighted in green thus indicating their selection for unfolding.
Not that auto-selection of tangential faces for unfolding is enabled only
when the „Chain Faces‟ option is selected in the Interactive Unfold
dialog box.
Faces deselected
As long as the „Chain Faces‟ option is
automatically
checked, the principle of
selecting/deselecting the highlighted green
faces will apply i.e. If you deselect any
highlighted green face, then all the
highlighted green faces are adjacent to the
deselected face and now disconnected from
the reference face will be also be deselected. The
vice versa principle applies to selecting faces for
unfolding.
For example, click on the highlighted
Click on this face
green face with the largest surface
to manually
area in order to deselect it. Observe
deselect
that faces tangential to it which are
now disconnected from the reference face
due to the deselection are also deselected.
2.
Once the faces to unfold are selected, you need to click on the OK
button on the Interactive Unfold dialog box in order to unfold the part.
The flattened part will be displayed automatically in the graphics area.
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
155
CAMWorks Nesting Tutorial
STEP 4: Selective Unfolding of Parts when „Chain Faces‟
option is disabled
In this section of the tutorial, we will explore how to select references faces
and faces to unfold when the Chain Features option is disabled.
1. If you have followed the instructions given in Step 3 of this tutorial,
then close the assembly without saving any changes.
2. Reopen the assembly (Step 1) and execute the Interactive Unfold
command (Step 2).
Disabling the Chain Faces option
3. In the graphics area, observe that faces are selected for unfolding
(highlighted in green color) because the Chain Faces option is
enabled.
4. In the displayed Interactive Unfold dialog box, uncheck the Chain
Faces option.
5. After unchecking the option, close the Interactive Unfold dialog box by
clicking on the Cancel button in the dialog box. This action is necessary
for the in order to let the effect of the disabled Chain Features option
to take place.
6. Open the Interactive Unfold dialog box again by executing the
Interactive Unfold command on the CAMWorksNesting menu or
CAMWorks Nesting Ribbon bar.
7. In the graphics area, observe that only reference face (in yellow
color) will be selected for both the native and imported parts. The face
with the largest surface area is selected as the reference face by
default. You need to manually select the faces for unfolding.
Native Part
Imported Part
Reference Face
Reference Face
Only Reference Faces are highlighted in Yellow color
156
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
Selecting faces to unfold when Chain Faces option is disabled
To select a face for unfolding, the face should be either adjacent to the
reference face or connected to the reference face via an already selected
face. A face selected for unfolding is
Reference Face
highlighted in green color in the graphics area.
Example:
i. In the graphics area, on the native part,
click on the bent face of the native part
as shown in the image on the right. This
face then becomes highlighted in green.
Observe that since this face is adjacent
to the reference, it is selected for
unfolding.
Select face adjacent to
the reference face
ii. Now click on the face which is tangential
and adjacent to the newly selected face
as shown in the image on the right.
Observe that this face too is selected for
unfolding though it is not adjacent to the
reference face. This face is selected as a
face to be unfolded because it is
connected to the reference face via the
previously selected face.
You can thus select all the desired faces
for unfolding one by one by clicking on
faces adjacent to the reference face or
an already selected face.
Click on this face
to manually
select the face
iii. Now deselect the bent face selected for
unfolding by clicking on that face. Observe that
the face tangential to it (which was also selected
for unfolding) has now become a reference face.
This is indicated by the change in color from
green to yellow.
The face changes to a reference face because
the face connecting it to the original reference
face is no longer selected.
Two Reference Faces
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
157
CAMWorks Nesting Tutorial
Changing Reference face when Chain Faces option is disabled
To select a face as reference face when the Chain Faces option is disabled:
-
The face should be planar in nature. Curved faces cannot be selected
as a reference faces.
-
If no face is selected as a reference face on the part, then any planar
face can be selected as the Reference face.
-
If one or more faces are already selected as reference faces, then any
planar face which is neither adjacent to any of the reference faces nor
connected to them via a selected face can be selected as a reference
face.
A face selected as reference face will be highlighted in yellow color in the
graphics area.
Illustration:
i. In the graphics area, deselect any faces that you may have already
selected for unfolding by clicking on the face. If any face other than
the face with the largest surface area is also
selected as a reference face, then deselect
that face by clicking on it.
ii.
When only the face with the largest
surface area remains selected as
the reference face, then click on the
curved face. This curved face is
neither adjacent to the reference
face nor connected to it via a
selected face.
Face with largest
surface area
selected as
reference face
Curve Face
Observe that you cannot select the curved face as a reference face.
This is because only planar surfaces can be
selected as reference faces.
iii. Now click on the planar face adjacent to the
curved face. This face gets
First Reference
selected as a reference face since
Face
it fulfills all the conditions for selection of a
reference face. It is planar in nature, and neither
adjacent to the other reference face nor
connected to it via a selected face.
Second Reference
iv. Now click on any one of the bent faces in order
to connect the first and second reference face.
Face
Observe that second reference face that was selected in the previous
step now becomes a selected face (indicated by the change in color of
158
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
the face from yellow to green). This is because the moment the bent
face is selected, a face chain is formed
and the second reference becomes
connected to the original reference face
via the bent face.
v. Now click on the original reference face
(the face with the largest surface area)
in order to deselect it. Observe that the
planar face highlighted in green now
once again becomes the reference face.
This is because whenever you deselect a
reference connected to other face
Select Bent
chains, then the tangentially connected
Face
planar face will be selected as a new
reference face (selection indicated by change in color of the face from
green to yellow).
New Reference
Face
Deselect the
Reference Face
Now click on the deselected reference face
(face with largest surface area) once again in
order to select it.
Observe that this now selected as a selected
face for unfold since it is connected to the
current reference face via another selected
face.
vi. Now click on the all the remaining faces in
order to select them for unfolding. As
you select each face, they will be
highlighted in green color thus
indicating their selection.
Selected
face
vii. Now once again click on the central
planar surface (face with the largest
area) in order to deselect it.
Deselect this face
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
159
CAMWorks Nesting Tutorial
Observe that four faces (two
bent faces and two planar
faces) are now no longer
connected to the reference
face due to the deselection
of this face. These
disconnected faces will now
form separate face chains.
In each face chain, the
planar surface will become
the reference face.
As seen in the image on the
right, three face chains will
be formed with each
containing a reference face.
Face
Chain 3
Face Chain 2
Reference
Faces
Deselected face
Face Chain1
Note: In the newly formed face chain, if there is no planar surface available then
such chains will be rejected from the unfolding process automatically.
viii. Click the OK button of Interactive Unfold dialog box to unfold the
parts. Before
unfolding,
CAMWorks
Nesting will
check the parts
to be unfolded
for the number
of disconnected
face chains. If a
part selected for
unfolding retains
more than one
disconnected
Error message dialog box
face chain, then
an error message will be displayed prompting you to remove unwanted
face chains. The parts won‟t be unfolded and the Interactive Unfold
dialog box remains open.
To proceed with nesting, you need to ensure that only one face chain
is selected on the each part to be unfolded.
Note: On non-faulty parts, the Reference face and the selected faces form a single
face chain. CAMWorks Nesting can only unfold a single face chain when an
Unfold command is executed. Multiple face chains cannot be unfolded.
160
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
CAMWorks Nesting Tutorial
ix. In the graphics area, click on the
central face (face with the largest
surface area) in order to select it.
Selecting this face for unfolding
connects all the face chains.
x. Click the OK button of Interactive
Unfold dialog box to unfold the parts.
Observe that unfolding is successful for
both the imported part as well as the
native part.
Select this face
xi. Once unfolded, use the Create Nesting
Job command to nest these parts.
Sample Nesting Layout for native part after unfolding
Tutorial 10 – Unfolding Sheet Metal Components Using „Interactive Unfold‟ Command
161
CAMWorks Nesting Tutorial
TUTORIAL 11 – THE STAMP FEATURE UNFOLD
OPTION
Introduction
If a sheet metal part to be nested contains stamp features, an option is
provided within CAMWorks Nesting to control the display of these stamp
features after the part is unfolded using one of the unfold commands.
The setting to control the behavior of the stamp features display can be
assigned only from the DefaultValues.ini file. It cannot be set from the
'Create Nesting Job' dialog box.
Topic covered in this Tutorial:
In this tutorial, you will explore how the settings in the DefaultValues.ini
file affect the behaviour of the stamp features present on sheet metal
part when the sheet metal part is unfolded.
Assigning Stamp Feature Unfold Option settings in DefaultValues.ini
There are three available settings to control the behavior of the stamp
features before nesting the sheet metal part. These settings are
controlled from the DefaultValues.ini file.
1. Open the file named DefaultValues.ini located in the CAMWorks
Nesting Installation folder.
(Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Lang\English)
2. In the [Unfold_Options] section, observe the flag named
'StampFeatureUnfoldingOption'. This is the flag used to control the
behavior of stamp features after the part is unfolded. Following are the
settings:
i.
0: Assigning the value „0‟ ensures that the stamp feature is
retained after the part is unfolded. (This is the default setting
at the time of installation.)
ii.
1: When the value „1‟ is assigned to this flag, the stamp feature is
patched with a flat planar surface after the part is unfolded.
iii.
2: When the value „2‟ is assigned to this flag, the stamp feature is
ignored after the part is unfolded. The area covered by the
stamp feature is replaced with a hole.
3. Once you make any changes to the settings in the Defaultvalues.ini
file, save the changes and close the file.
162
Tutorial 11 – The Stamp Feature Unfold Option
CAMWorks Nesting Tutorial
Stamp Feature Unfold Option settings for Native parts & Imported Parts
After a sheet metal part with stamp feature(s) is unfolded, the resultant
display of the stamp feature based on settings in the DefaultValues.ini file
depends on whether the unfolded part is a native sheet metal part or
imported sheet metal part. In the case of native parts, it also depends on
the type of command used to unfold the part.
Given below is table indicating the relation between the various unfold
commands and the applicability of the Stamp Feature Unfold Option for
native parts and imported parts.
Type of Part
Native Part
„Intelligent Unfold‟
command
This command is not
applicable to native parts.
„Unfold All Parts‟
command
Stamp Feature Unfold
Option settings in
DefaultValues.ini file
applied when part is
unfolded using this
command.
„Interactive Unfold‟
Type of command
Unfold
Command
„Create Nest Job‟
command
If this command is
executed directly without
using any other unfold
command, then the stamp
features will be always
retained irrespective of the
settings in the
DefaultValues.ini file.
Imported Part
Stamp Feature
Unfold Option
settings in
DefaultValues.ini
file applied when
part is unfolded
using this
command.
This tutorial is divided into two sections:
Part 1: Stamp Feature Unfold Options for Native Sheet Metal Parts
Part 2: Stamp Feature Unfold Options for Imported Sheet Metal Parts
Tutorial 11– The Stamp Feature Unfold Option
163
CAMWorks Nesting Tutorial
Part 1: Stamp Feature Unfold Options for Native Sheet
Metal Parts
Step 1: Open the Part
1. Launch CAMWorks Nesting as an Add-In in
the SOLIDWORKS or CAMWorks Solids
environment.
2. Open the part file
Tutorial_11a_native.sldprt located in
the following folder:
Drive:\CAMWorksNestingData\CAMWorksNestin
g201x\Examples\Tutorials\Parts
3. Observe that this is a native part with a
stamp feature.
Tutorial_11a_native.sldprt
Step 2: Executing the Unfold Command
For the settings of the Stamp Feature Unfold Option in DefaultValues.ini to
take effect, you need to first unfold the part. To unfold the part you can use
the unfold commands available on the CAMWorks Nesting Ribbon bar as well
as the CAMWorksNesting menu. Following are the unfold commands you can
use to unfold a native part:
1. The „Unfold All Parts‟ command
When you execute this command, the Unfold All Parts dialog box will be
displayed. Click the OK button to unfold the part.
2. The „Interactive Unfold‟ command
When you execute this command, the Interactive Unfold dialog box will
be displayed. Click the OK button to unfold the part.
3. The „Create Nest Job‟ command
When you execute this command, the native part will be auto-unfolded
before the Create Nesting Job dialog box is displayed. (The native sheet
metal part will be unfolded only if the flag named FlattenSheetMetalPart
in the DefaultValues.ini file is set to „1‟. This is the default setting)
Note: The „Intelligent Unfold‟ command cannot be used to unfold the native parts. This
command is applicable only for imported parts.
164
Tutorial 11 – The Stamp Feature Unfold Option
CAMWorks Nesting Tutorial
Step 3: Retaining the stamp
feature
1. Open the DefaultValues.ini file
and set the
StampFeatureUnfoldingOption
flag to „0‟. This setting ensures
that the stamp feature is
retained after the part unfolding
process.
2. When you unfold the native part
using any one of the commands
mentioned in Step 2, the stamp
feature will be retained.
Result of the Retained Stamp Option
Step 4: Patching the stamp
feature
You will now set the stamp feature
unfolding option to patch the stamp
feature after unfolding.
1. Open the DefaultValues.ini file and
set the
StampFeatureUnfoldingOption flag
to „1‟. This setting ensures that the
Result of the Patch Stamp Feature option
stamp feature is patched after the
when the „Unfold All Parts‟ or „Interactive
part unfolding process.
Unfold‟ command is executed
2. Save the changes and close the
DefaultValues.ini file.
3. Unfold the part using either the
„Unfold All Parts‟ or „Interactive
Unfold‟ command.
Observe that the stamp feature is
patched (replaced) with a planar
surface after the part is unfolded.
4. Now close the part (without saving
the changes) and reopen the part
in SOLIDWORKS/CAMWorks Solids.
Directly execute the „Create Nest
Result of the Patch Stamp Feature
Job‟ command.
option when the „Create Nest Job‟
command is executed
Observe that the stamp feature is
retained instead of being patched.
This indicates that the setting for the Stamp Feature Unfold Option in the
DefaultValues.ini was not applied to the part.
Tutorial 11– The Stamp Feature Unfold Option
165
CAMWorks Nesting Tutorial
Note: If you unfold a native part directly using the „Create Nest Job‟ command, then the
Stamp features present on the part will always be retained on the part after it is
unfolded irrespective of the settings for „Stamp Feature Unfold Option‟ in the
DefaultValues.ini file. This behavior results because CAMWorks Nesting uses
SOLIDWORKS functionality to flatten the native sheet metal parts instead of
CAMWorks Nesting functionalities.
Step 5: Ignoring the stamp feature
You will now set the stamp feature unfolding option to ignore the stamp
feature after unfolding process.
1. Open the DefaultValues.ini file and set the StampFeatureUnfoldingOption
flag to „2‟. This setting ensures that the stamp feature is ignored after the
unfolding the part.
2. Save the changes and close the DefaultValues.ini file.
3. Unfold the part using either the „Unfold All Parts‟ or „Interactive Unfold‟
command. Observe that the stamp feature is ignored. The area covered
by the stamp feature is replaced with a hole.
4. Now close the part (without saving the changes) and reopen the part in
SOLIDWORKS/CAMWorks Solids. Directly execute the „Create Nest Job‟
command. Observe that the stamp feature is retained instead of being
ignored.
This indicates that the setting for the Stamp Feature Unfold Option in the
DefaultValues.ini was not applied to the part.
Result of the Ignore Stamp Feature option
when the „Unfold All Parts‟ or „Interactive
Unfold‟ command is executed
Result of the Ignore Stamp Feature
option when the „Create Nest Job‟
command is executed
Once the part is unfolded, proceed to nest the part using the Create Nesting
Job dialog box.
166
Tutorial 11 – The Stamp Feature Unfold Option
CAMWorks Nesting Tutorial
Step 6: Behaviour in native parts without bends
1. Open the part file Tutorial_11c_native.sldprt located in the following
folder:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Examples\Tutorials\Parts
Observe that this is an imported
part without bends. The part has a
stamp feature.
2. Execute Step 3, Step 4 and Step 5
and once again observe that the
behaviour of the stamp feature
changes as per the settings in the
DefaultValues.ini file only when the
„Unfold All Parts‟ or the „Interactive
Unfold‟ command is executed. If the
part is unfolded directly using the
Tutorial_11c_native.sldprt
„Create Nest job‟ command, then
the setting for Stamp Feature Unfold Option will not take effect and the
stamp feature will be retained.
Result of the Patch Stamp Feature option
when the „Unfold All Parts‟ or „Interactive
Unfold‟ command is executed
Result of the Ignore Stamp Feature option
when the „Unfold All Parts‟ or „Interactive
Unfold‟ command is executed
Note: The settings for the Stamp Feature Unfold Option in the DefaultValues.ini file is
applicable for a native part only if you first unfold the part using either the
„Unfold All Parts‟ or the „Interactive Unfold‟ command.
For a native part (with or without bends), the stamp feature is always retained
on the part if you directly execute the „Create Nest Job‟ command without first
executing the „Interactive Unfold‟ or „Unfold All Parts‟ command.
Tutorial 11– The Stamp Feature Unfold Option
167
CAMWorks Nesting Tutorial
Part 2: Stamp Feature Unfold Option for Imported Sheet
Metal Parts
Step 1: Open the Part
1. Launch CAMWorks Nesting as an Add-In in
the SOLIDWORKS or CAMWorks Solids
environment.
2. Open the part file
Tutorial_11b_imported.sldprt located in
the following folder:
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Parts
3. Observe that this is an imported part with
bends. The part has a stamp feature.
Tutorial_11b_imported.sldprt
Step 2: Executing the Unfold Command
For the settings of the Stamp Feature Unfold Option in DefaultValues.ini to
take effect, you need to first unfold the part. To unfold an imported part,
you can use any one of the following commands available on the CAMWorks
Nesting Ribbon bar as well as the CAMWorksNesting menu.
1. The „Intelligent Unfold‟ command
When you execute this command, the Unfold Imported Bodies dialog box
is displayed. Click the OK button to unfold the part.
2. The „Unfold All Parts‟ command
When you execute this command, the Unfold All Parts dialog box is
displayed. Click the OK button to unfold the part.
3. The „Interactive Unfold‟ command
When you execute this command, the Interactive Unfold dialog box is
displayed. Click the OK button to unfold the part.
4. The „Create Nest Job‟ command
When you directly execute this command for imported parts/assembly,
CAMWorks Nesting will display a message indicating that the
part/assembly contains imported parts and whether you wish to unfold
the parts before proceeding with the nesting process. Click Yes. The
Unfold All Parts dialog box will be displayed. Click OK button in this dialog
box to unfold the parts. If you click the Cancel button, then the parts will
neither be unfolded nor will the settings for the Stamp Feature Unfold
Options be applied to the parts.
168
Tutorial 11 – The Stamp Feature Unfold Option
CAMWorks Nesting Tutorial
Step 3: Retaining the stamp feature
You will now set the stamp feature unfolding option to retain the stamp
feature after unfolding the part.
1. Open the DefaultValues.ini file
and set the
StampFeatureUnfoldingOption
flag to „0‟. This setting ensures
that the stamp feature is
retained after the part unfolding
process.
2. Save the changes and close the
DefaultValues.ini file.
3. Unfold the part using any one of
the commands as listed in Step
2. Observe that the stamp
feature is retained after the part
is unfolded.
Result of the Retained Stamp Option
Step 4: Patching the stamp feature
You will now set the Stamp Feature Unfold Option to patch the stamp feature
after unfolding the part.
1. Open the DefaultValues.ini file and
set the
StampFeatureUnfoldingOption flag
to „1‟. This setting ensures that
the stamp feature is patched after
the part is unfolded.
2. Save the changes and close the
DefaultValues.ini file.
3. Unfold the part using any one of
the commands as listed in Step 2.
Observe that the stamp feature is
patched (replaced) with a planar
surface after the part is unfolded.
Result of the Patch Stamp Feature option after
the part is unfolded
Step 5: Ignoring the stamp feature
You will now set the Stamp Feature Unfold Option to ignore the stamp
feature after unfolding.
1. Open the DefaultValues.ini file and set the StampFeatureUnfoldingOption
flag to „2‟. This setting ensures that the stamp feature is ignored after the
unfolding the part.
Tutorial 11– The Stamp Feature Unfold Option
169
CAMWorks Nesting Tutorial
2. Save the changes and close the DefaultValues.ini file.
3. Unfold the part using any one of the commands listed in Step 2. Observe
that the stamp feature is ignored. The area covered by the stamp feature
is replaced with a hole.
Result of the Ignore Stamp Feature option after
the part is unfolded
Note: If you unfold an imported part containing stamp features before nesting the part,
then the stamp feature will be retained, patched or ignored based on
„StampFeatureUnfoldOption‟ flag settings in the DefaultValues.ini file.
Once the part is unfolded, proceed to nest the part using the Create Nesting
Job dialog box.
Step 6: Behaviour in imported parts without bends
1. Open the part file
Tutorial_11d_imported.sldprt
located in the following folder:
Drive:\CAMWorksNestingData\CAMWorks
Nesting 201x\Examples\Tutorials\Parts
Observe that this is an imported part
without bends. The part has a stamp
feature.
2. Execute Step 3, Step 4 and Step 5
and observe that the behaviour of
the stamp feature changes as per
the settings in the DefaultValues.ini
file.
170
Tutorial_11d_imported.sldprt
Tutorial 11 – The Stamp Feature Unfold Option
CAMWorks Nesting Tutorial
Result of the Patch Stamp Feature option after
the imported part is unfolded
Result of the Ignore Stamp Feature option after
the part is unfolded
Note: If you want the settings for the Stamp Feature Unfold Option in the
DefaultValues.ini file to be applied to an imported sheet metal part without any
bends, then unfold the part using any one of the unfold commands.
Tutorial 11– The Stamp Feature Unfold Option
171
CAMWorks Nesting Tutorial
TUTORIAL 12 – GENERATING NC CODES FOR
NESTED LAYOUTS USING CAMWORKS (I)
How the Nested layouts generated are saved within
SOLIDWORKS
Once the Nesting process using the CAMWorks Nesting application is
completed, the nested layout(s) generated will always be saved as a
SOLIDWORKS assembly file (*.sldasm). Depending on various factors such as
thickness and/or material part of part, number of sheets, grain direction, etc.,
either one or multiple Nested layouts will be generated.
 If only one nested layout is generated, then it will be saved as a
SOLIDWORKS Assembly file comprising of nested parts. The sheet
dimensions will be saved as a SOLIDWORKS sketch.
 If multiple nested layouts are generated, then these nested layouts will be
saved as a SOLIDWORKS Assembly file comprising of assemblies. Each
assembly is a nested layout comprising of nested parts. The sheet
dimensions for each sheet will be saved as a SOLIDWORKS sketch.
Once the nested layout(s) are generated, each nested layout assembly (sheet
layout containing nested parts) will be listed in the SOLIDWORKS Configurations
Manager.
Relation between CAMWorks Nesting and CAMWorks
Both CAMWorks Nesting and CAMWorks, developed by Geometric Americas, Inc.
are applications which are fully integrated with the CAD application of
SOLIDWORKS/CAMWorks Solids. While CAMWorks Nesting is a Nesting
application, CAMWorks is a highly-intelligent CAM application used for
generating NC codes.
After generating the nested layout with the CAMWorks Nesting application, the
next step would ideally be to generate NC codes for the nested layouts. To
generate NC codes, a CAM application needs to be used. Generating NC codes
using the CAMWorks application is easier than using other CAM application
since:
- Both CAMWorks Nesting and CAMWorks have been developed by the same
entity viz. Geometric Americas, Inc.
- Both these applications are fully integrated with SOLIDWORKS.
- Both these applications work with the same file types viz. file types that are
compatible with SOLIDWORKS.
- A new functionality is provided from CAMWorks Nesting 2014 SP1 version
onwards that automatically links the nested layout output of CAMWorks
Nesting as the input for CAMWorks, thereby reducing the number of steps
required for generating NC codes. (This functionality is discussed in the next
tutorial in detail).
In this tutorial and the next tutorial, you will learn how to generate NC codes for the nested
layouts using the CAMWorks application.
172
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
Steps to generate NC codes for Nested layouts
To generate NC codes for nested layout assemblies, a number of steps are
involved. Following are the steps for generating NC codes for Nested layouts
using CAMWorks:
Steps to generate
Nested Layouts
Steps to generate NC
codes
Define the Fixture Coordinate
System for the machine
Launch CAMWorks Nesting
and CAMWorks as Add-Ins
within SOLIDWORKS.
Define the Machine
Select the parts/assembly of
parts to be nested.
Nested assemblies are listed
in the SOLIDWORKS
Configuration Manager.
Generate Nested layout
assemblies using CAMWorks
Nesting application.
Add the parts in the Nested
layout assemblies to
CAMWorks Part Manager.
Define a common stock for
each nested layout assembly.
Define Machinable Features
Sort Part Instances to derive
optimal machining order.
These steps are automated
from CAMWorks 2014
SP2.2 version onwards
Generate the operations.
Readjust operation
parameters if necessary
Generate toolpaths
Run the Toolpath Simulation
Adjust the operation
parameters as required.
Generate NC Code
Flowchart illustrating how to generate NC codes for Nested Layout assemblies using CAMWorks
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
173
CAMWorks Nesting Tutorial
Generating the nested layout assembly
In this tutorial, you will generate NC codes for the nested layout generated in
Tutorial 3.
1. Launch CAMWorks Nesting as an Add-In in the SOLIDWORKS environment.
2. To generate the nested layout, do any one of the following:
a. Direct open the nested layout assembly file:
Open the assembly file Tutorial_12_Nested_Layout.sldasm located in the
following folder:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Examples\Tutorials\
Assemblies/Tutorial_12
Nested Layout
b. Generate the nested layout assembly:
i.
Open the part file Tutorial_3.sldprt located in the following folder:
Drive:\CAMWorksNestingData\CAMWorksNesting
201x\Examples\Tutorials\Parts
ii.
iii.
174
Follow the steps mentioned in the Tutorial 3 of this document to
generate the nested layout. However, while executing the Tutorial 3,
minor changes are required in Step 3 and Step 4 as follows:

Under the Step 3: Define the Part Parameters; change the
assigned quantity for parts from 125 to 12.

Under the Step 4: Defining a „Custom‟ size sheet, change the
assigned length to 600mm and a width to 350mm.

Execute all the other steps as it is mentioned in the Tutorial 3 to
generate the nested layout as shown below.
The generated nested layout obtained from Tutorial 3 will be used as
input for CAMWorks.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
3. In the SOLIDWORKS left hand side panel, click on
the SOLIDWORKS FeatureManager Design Tree.
FeatureManager Design Tree
4. Observe that a sketch
(Sheet1_CustomSheet1) representing the
dimensions of the Custom sheet (in which
the parts are nested) is listed in this tree.
Sketch representing dimensions
of Custom sheet
Step 1: Define the Fixture Coordinates
The Fixture Coordinate System defines the "home point" or main zero position
on the machine. It defines the default G-code origin, defines the XYZ machining
directions and acts as a reference point, if subroutines are used. This
coordinate system needs to be defined in the SOLIDWORKS FeatureManager
Design Tree.
Steps to set the Fixture Coordinates System
1. If necessary, rotate and zoom the nested layout assembly in the graphics
area to clearly view the position where you desire to assign the
coordinate system.
2. Click the Insert menu on the SOLIDWORKS menu bar.
3. From the dropdown
menu, select Reference
Geometry and then select
the Coordinate System
from the cascading
context menu.
The Coordinate System
dialog box is displayed.
4. In the graphics area,
click on the Coordinate
System origin.
Selecting „Coordinate System‟ from cascading menu
This action will display the selected coordinate system origin in the field
of Selection group box.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
175
CAMWorks Nesting Tutorial
5. The XYZ machining direction
should be same as displayed
in the image on the right. If
necessary, click on the
Reverse Axis Direction button
to obtain the correct
machining direction.
6.
Click the OK button to
save the changes and close
the dialog box.
The defined coordinated
system is listed under the
FeatureManager Design tree.
XYZ machining direction
Step 2: Define the Machine
Before you machine the Nested layout assembly, you need to define the
Machine that will be used to machine the assembly.
1. In the SOLIDWORKS left hand side panel, click on
the
CAMWorks Feature Tree tab. (Note that this
tab will be visible only if CAMWorks is loaded as an
Add-In within SOLIDWORKS)
CAMWorks Feature Tree
When the CAMWorks Feature tree is displayed, it initially lists
Configurations, Machine, Part Manager and Recycle Bin items.
2. Double-click on the
Machine item (Machine [Mill - metric] in this case) to
open the Machine dialog box.
3. The Machine tab of the Machine dialog box is displayed. This tab allows
you to select the machine that the assembly will be machined on. By
default, either the Mill - metric or Mill - inch will be already selected.
If you wish to select any other Mill machine or a user-defined Machine definition,
then highlight it in the Available Machines list and click the Select button.
4. Click on the Tool Crib tab, ensure that Tool Crib 1(metric) is selected.
To select an alternative tool crib, select the desired tool crib In the Available tool
cribs list box and click on the Select button.
5. Click on the Post Processor tab. This tab allows you to select a post
processor for generating NC codes or for generating enhanced CL files
that can be used by external third party post processing programs.
By default, the sample post processor M3AXIS-TUTORIAL is selected. For
this tutorial, this default post processor will be used.
If you wish to use another post processor or a customized post processor
provided to you by your CAMWorks Reseller, then highlight the desired post
processor in the Available list and click the Select button. If the post processor
176
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
is not listed, then click on the Browse button to navigate to the folder where the
post processor file is located.
6. Click on the Setup tab. This tab allows you to set the Fixture Coordinate
System for the machine.
-
Since a 2.5 Axis/ 3 Axis Mill Machine will be used to machine the
assembly, Indexing will remain set to None.
-
In the CNC comp options group box, ensure that the Calculate safe CNC
comp toolpath option is checked.
-
In the Fixture Coordinate system group box, highlight Coordinate Sytem1
in the Coordinate systems list box. This action will display the
highlighted entity in the Selected entity list box.
7. Click OK to apply the changes and close the Machine dialog box.
Step 3: Addition of nested Parts to Part Manager
The parts that are to be machined must be identified to CAMWorks by adding
them to the Part Manager item in the CAMWorks Feature tree.
The Assembly document (*.sldasm) contains different part model documents. In
addition to the parts that are going to be machined, the document might
contain clamps, fixture of machine components which are included to assist in
the layout of the parts and shop documentation. To help CAMWorks identify the
components of the assembly file to be machined, the parts that are to be
machined must be added to the Part Manager.

When machining multiple instances of the same part, you must add all
instances to the Part Manager.

Feature recognition will only run once for each unique part name.
Automatic and interactive features will be referenced automatically at all
other part instances.
Following are the steps to add parts to the Part Manager:
1.
Double click Part Manager item in the CAMWorks Feature tree.
The Manage Parts dialog box is displayed.
2. Select the part in the left corner of the
assembly as shown in the image on the
right.
For each unique part in the assembly,
the first instance that you select is called
the seed part. When an action is
performed on the seed part, the same
action will be applied to every other
instance of that part in the assembly.
Select the left corner part of Assembly
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
177
CAMWorks Nesting Tutorial
3. Highlight the part in the Selected Parts list and click the Add All Instances
button. The parts are listed in the order they are in the file.
OR
You can also pick the parts individually in the graphics area or in the
SOLIDWORKS FeatureManager Design Tree.
Part instances can be added at any time. You can select only one instance of a part
(the seed part) to work on first and then add other instances later. Any features,
operations and toolpaths that have been generated for the seed part are automatically
transferred to instances of the same part when they are added in the Manage Parts
dialog box.
4. Later in this tutorial, you use the Sort Instances function to change the
machining order.
5. Click OK to exit the Manage Parts dialog box. In the CAMWorks Feature
tree, under the Part Manager item, observe that:

The part name is listed under the Part Manager item.

A Feature Manager is created for each unique part. In this tutorial,
since only one unique part is machined, only one Feature Manager item
is created. (It will be used to define the Mill Part Setups and
machinable features associated with the seed part.)

For each unique part, all the instances are listed under the
Instances item. You can re-order and/or delete the part instances in
the tree.
Manage Parts Dialog Box
178
List of Parts
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
Step 4: Define the Stock
When you add parts in the Manage Parts dialog box, a default Stock is created
for each part based on a 0.00 bounding box offset (cuboid with the minimum
required dimensions from which the part can be machined). The Stock Manager
dialog box allows you to customize the stock associated with the parts.
In this tutorial, all the default individual stocks of type Bounding Box created for
each part will be replaced a common stock. All the parts will be machined from
this common stock.
1.
Double click Stock Manager in the CAMWorks Feature tree.
OR
Right click Stock Manager item in the CAMWorks Feature tree and select
Edit Definition on the context menu.
The Stock Manager dialog box is displayed. This dialog box allows you to
modify the existing default stock or create new stock for single parts or
define common stock for multiple parts. Observe that the default stock is
Bounding Box with zero offsets.
2.
Under Stock Type, select
Extruded Sketch.
3. Pick the rectangular sketch
representing the sheet in the
graphics area.
OR
In the top left corner of the
Highlight Sheet1_CustomSheet1 in the tree
graphics area, expand the
SOLIDWORKS tree (Tutorial_12_Nested_Layout) and select the sketch
Sheet1_CustomSheet1.
This action will select this sketch.
4.
In the Depth field, set the Depth to
3mm.
5. Scroll down the Stock Manager dialog box
and in the Create Stock group box, click the
Common button.
Click „Common‟ button
CAMWorks will display the warning message stating that parts instances
already have stock which will then be deleted.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
179
CAMWorks Nesting Tutorial
CAMWorks Warning Message
6. Click Yes to delete the individual stocks for the parts and replace them
with a common stock.
7.
Click OK to close the Stock Manager dialog box.
Step 5: Defining Machinable Features
The next step is to automatically extract the machinable features using the
Automatic Feature Recognition (AFR) technology available in CAMWorks. The
machinable features extracted all applicable to all instances of the part.
At the Mill Part Setup level, features can be inserted interactively using the New
2.5 Axis Feature or New Multi Surface Feature or New Part Perimeter Feature
commands. Such an insertion of features is known as Interactive Feature
Recognition.
For each unique part, the Machinable Features recognized are added under the
Feature Manager item of the CAMWorks Feature Tree. The features (both
automatically recognized or interactively inserted) for the seed part are
automatically copied to all other part instances defined in the Part Manager.
Extracting Machinable Feature using AFR
1.
Click the Extract Machinable Features button on the CAMWorks
Command Manager.
OR
Right click CAMWorks NC
Manager in the CAMWorks
Feature tree and select
Extract Machinable Features
command on the context
menu.
2. The CAMWorks Message
Window is displayed. This
window is displayed
automatically to report the
CAMWorks Message Window
180
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
progress of the current process. Close this Message Window.
3. On execution of the Extract Machinable Features command, CAMWorks
generates the Mill part Setup and the machinable features. The items are
displayed in the CAMWorks Feature tree under Part Manager>>Feature
Manager.
4. Expand the
Feature Manager item in the CAMWorks Feature tree by
clicking on the + sign next to it.
The Feature Manager lists the Mill Part Setup and machinable features that
were automatically recognized using AFR.
List of Machinable Features recognized using AFR
Interactively Inserting Features
The Part Perimeter feature was not recognized automatically using AFR. Hence,
this feature will be inserted interactively.
1.
Right click Mill Part Setup1 under the Feature Manager and select New Part
Perimeter Feature on the context menu.
The New Perimeter Feature dialog box is displayed.
2. Within this dialog box, change the Feature type to Boss.
3.
Click OK to close the dialog box.
The Perimeter Boss feature is added to the list of features under Mill Part
Setup1.
All features listed under Mill Part Setup1 are added to the seed part and
also to every instance of the part.
When you recognize features by Automatic Feature Recognition (AFR) or
Interactive Feature Recognition (IFR), the features listed in the CAMWorks
Feature tree will display in Magenta color (by default) till you generate
operations for these features. Once a valid operation is generated, the color of
the corresponding feature item will change Black color (by default) indicating
successful generation of the operation(s).
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
181
CAMWorks Nesting Tutorial
If operations could not be generated for a feature (because the feature
conditions have not been defined in the Technology Database for that particular
feature type), then the feature will continue to display in the initial color
(Magenta color), thus indicating that they have no operations defined.
You can set these colors on the Display tab in the CAMWorks Options dialog
box.
Step 6: Sorting Part Instances
When part instances are automatically added or manually added using the Add
All Instances button, the instances need not necessarily be listed in the best
machining order. CAMWorks provides options for sorting part instances to be
processed in a more efficient order.
Following are the steps to sort Part Instances:
1. Under Setup1 in the CAMWorks Feature Tree, expand all the listed feature
items by clicking on the plus sign next to them.
The order in which the part instances are listed under each feature is the
machining order for that feature. By default, for all features, the parts are
in the order they appear in the Part Manager. You can change the order
globally for all features or for individual features.
In this tutorial, you will set the machining order for all the features
globally.
2.
Double click Part Manager in the CAMWorks Feature Tree.
3. Click the Sort Instances button in the Manage Parts dialog box.
4. The Sort Instances dialog box is displayed. This dialog box provides
automatic or manual options for sorting the part instances for features in
the Setup.
The Part Manager instances option automatically sorts part instances for
all features in the Setup based on the user-defined order of instances
listed in the tree under the Part Manager. To set the order using this
option, expand the Part Manager and Instances items, then drag and drop
the part instances.
 The Part Manager instances option automatically sorts part instances
for all features in the Setup based on the user-defined order of
instances listed in the tree under the Part Manager. To set the order
using this option, expand the Part Manager and Instances items, then
drag and drop the part instances.
 Grid pattern automatically sorts part instances for all features in the
Setup based on the start corner, processing direction and process
order.
 The Feature instances option allows you to manually reorder the part
instances listed under each feature in the Setup. To set the order
using this option, expand a feature in the Setup, then use drag and
drop to move the part instances.
182
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
You can use one of the automatic methods, then if necessary, select the Feature
instances option and make changes to the part order for individual features.
5. Select the Grid pattern option.
When you will select the Grid pattern option, the order will change for the
part instances under every feature in the Setup.
6. Select the following Grid options:
 Start corner= Bottom left

Direction= Horizontal

Pattern= Zigzag
Sort Instances Dialog Box
7. Click OK to close the Manage Parts dialog box.
8. Click the ( ) plus sign next to any feature listed under Setup1. Observe any
changes in the order of the part instances.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
183
CAMWorks Nesting Tutorial
Expand the feature
under Setup
Part Instances rearranged
after sorting
Part Instances rearranged after executing Sort Instances command
Step 7: Generating the Operation Plan
An Operation Plan contains information on how each machinable feature is to
be machined and how the NC code will be output. When Generate Operation Plan
command is executed, operations for each machinable feature are created
automatically based on information in the TechDB. The operations generated
are listed in the CAMWorks Operation tree.
To execute this command:
1.
Click the Generate Operation Plan button on the CAMWorks Command
Manager.
OR
Right click the CAMWorks NC Manager item of the CAMWorks Feature tree
and select Generate Operation Plan on the context menu.
2. On execution of this command, CAMWorks switches to the CAMWorks
Operation tree. All the operations generated are listed under Setup1 in
the CAMWorks Operation tree.
184
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
Expand an operation to view
the feature for which it has
been generated
Generated Operations listed in
CAMWorks Operation Tree
When Operations are generated or interactively inserted, they will be displayed
in Magenta color (by default) in the CAMWorks Operation Tree till you generate
toolpaths for these operations. Once the toolpath is generated, the color of the
corresponding operation will change to Black color (by default) indicating
successful generation of the toolpath.
3. Click on the ( ) plus sign next to an operation indicates the feature for which
the operation has been generated. One or more operations may be
generated for each machinable feature. For example, click on the sign next
to Contour Mill5 operation. This operation has been generated for the Perimeter
Boss feature.
Step 8: Adjusting Operation Parameters
While generating the nested layout, the Part-to-part distance was set to 3 mm
and the Part-to-sheet distance was set to 2 mm.
The Contour Mill5 operation generated for Perimeter Boss feature is used to
machine the perimeter of the part and thereby separate it from the common
stock. Since the Part-to-part distance is 3 mm and the Part-to-sheet distance is 2 mm,
the Flat End Mill tool used for machining the Contour Mill5 operation should not
exceed 2mm in diameter else it might end up gouging the part.
1. In the Operation tree, double click Contour Mill5 operation.
OR
Right click Contour Mill5 and select Edit Definition on the context menu.
The Operation Parameters dialog box is displayed.
2. Click on the Tool tab and select the Mill Tool Page.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
185
CAMWorks Nesting Tutorial
Mill Tool Page under Tool Tab of Operation Parameters dialog box
Observe that the diameter of the tool currently selected for this operation
is 6mm. This tool will gouge the part. Hence, another tool needs to be
selected for machining this operation.
3. Under the Tool tab, click on the Tool Crib page.
4. In the displayed tool crib, highlight the 1mm diameter Flat End Mill Tool
within the list of displayed tools.
5. Click the Select button. This action will assign the highlighted tool as the
tool to be used for machining this operation.
Highlight a 1mm Flat End Mill Tool in the Tool Crib and click the Select button
186
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
6. CAMWorks will display a warning message indicating whether you wish to
replace the corresponding holder also. Click Yes to replace the
corresponding holder.
The Mill Tool page is now
displayed. It displays
the parameters of the
selected tool.
7. Click OK to apply the
changes and close the
Operation Parameters
dialog box.
CAMWorks Warning Message
Step 9: Defining G-code Program Zero Location
Toolpaths can be output relative to the Part Setup origin or a global Setup
origin. In this tutorial, you will use the Part Setup origin. The Part Setup origin
specifies only the toolpath zero point, not the XYZ machining direction. The
machining direction is based on the Fixture Coordinate System. When
machining multiple instances of the same part, the origin is defined relative to
the first (seed) part and referenced for all other instances of the same part.
1.
Double click Setup1 in the CAMWorks Operation tree.
The Setup Parameters dialog box is displayed.
2. On the Origin tab, make sure Part Setup origin is selected for the Output
origin.
Note that when Setup origin is selected, you can specify the origin using
several methods.
3. Click on the Offset tab.
The order of the parts on this page affects only the assignment of the
offsets, not the machining order.
4. In the Sort by group box, select Grid pattern.
When you pick this option, the parts in the table are automatically
reordered based on the current settings for Start corner, Direction and
Pattern.
5. Set the Grid pattern parameters to the same settings you used when
sorting part instances for the machining order (Step 7-Point 6):
 Start corner = Bottom left (specifies which part, based on a grid
layout, will be assigned the register equal to the Start Value)


Direction = Horizontal (relative to the Start corner part, the Direction
defines which part will be assigned the next offset register value)
Pattern = Zigzag (defines the order the offsets are assigned)
Notice that the part order is updated in the table. You can specify a
programmable coordinate offset and assign an offset to each part.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
187
CAMWorks Nesting Tutorial
6. Set the Work coordinate offset to Work Coordinate. This option will output
G54, G55, etc.
7. Set the Start value to 54 and the Increment to 1.
8. For the Start value, specify only the numerical value of the offset and not
the G-code prefix.
9. Click the Assign button of the Work Coordinate offset group box. The
numbers update in the Offset and Sub columns in the table.
10. Click OK to close the Setup Parameters dialog box.
Setup Parameters Dialog Box
Note:
Changing the machining order does not automatically change the offset
assignments. If you want the offset order to correspond to the machining
order, you need to sort the parts and reassign the offsets on the Offset tab.
Step 10: Generating Toolpaths and Sorting Operations
Operations are generated for machinable features and listed in the CAMWorks
Operation tree in the same order as the corresponding features in the
CAMWorks Feature tree. This sequence is not necessarily the ideal machining
sequence. Operations can be sorted in order to reduce machining time.
In this step, all the operations listed in the CAMWorks Operation tree will be
sorted in order to create a logical machining sequence.
188
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
1.
Click the Generate Toolpath button on the CAMWorks Command
Manager.
OR
Right click Setup1 in the Operation tree and select Generate Toolpath on the
context menu.
On executing the Generate Toolpath
command, CAMWorks calculates the
toolpaths for each operation in the Setup.
The font color of all the listed operations in
the Operation tree changes from magenta
to black. This change in color indicates that
toolpaths were successfully generated.
Note: If an operation displays in a magenta color
instead of black even after the Generate
Toolpath command has been executed,
then it indicates that the toolpath has not
been generated. This might occur in one of
the following situations:
i. When you insert a new operation
interactively;
Updated list of operations after
executing the Sort Command
ii. When you insert a new feature
interactively and then generate operations for the new feature
iii. When CAMWorks cannot generate the toolpath for an operation because of
an error in the toolpath algorithm or when a parameter is not correct.
2.
Right click Setup1 in the CAMWorks Operation tree and select Sort
Operations on the context menu.
3. On the Process tab, remove the check mark from the Process complete
feature option.
Remove the check mark from the „Process complete feature‟ option
4. Click on the Sort tab.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
189
CAMWorks Nesting Tutorial
5. In the Sort by Operation Type group box, drag and drop operations so that
Rough Mill is at the top of the list, followed by Contour Mill, Center Drill, and
Drill.
Drag and drop
operations to desired
sequence
Operations before sorting
Operations after sorting
6. Click Apply button and confirm that the tree view updates to sort the
operations according to this order. If it updates as expected, then click
OK.
The operations under Setup1 are sorted based in the order on the Sort
tab.
7. Left click any operation in the CAMWorks Operation tree. That operation
will be highlighted in the Operation tree.

The toolpath for that highlighted operation will be displayed in the
graphics area. As you highlight each operation in the tree, the
toolpaths for that corresponding operation will be displayed.

Turning operation parameters can be edited and the operation can be
renamed, moved, suppressed, deleted, etc. after toolpaths have been
generated. These commands are available in the RMB context menu.

If you make any changes, the toolpaths must be updated by executing
the Generate Toolpath command again at the Setup level.
8. Hold down the Shift key and select the first and last operation in the tree.
This action selects all the operations. The toolpaths for all the operations
will be displayed on the part showing the centerline of the toolpath.
190
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
Toolpaths for all the operations displayed on the part when all
the operations are selected in the Operation tree
Step 11: Simulate Toolpaths
CAMWorks provides the ability to simulate the toolpaths showing the tool
movement and the resulting shape of the part.
1.
Click the Simulate Toolpath button on the CAMWorks Command
Manager.
OR
Right click on Setup1 in the Operation tree and select Simulate Toolpath on
the context menu.
The Toolpath
Simulation toolbar is
displayed.
When you click on
the display control
Toolpath Simulation toolbar
buttons of the
Toolpath Simulation toolbar, the available settings associated with that
button are displayed in a dropdown list.
2. Set the following display options:
3.
-
Stock: Translucent display
-
Tool: Shaded display
-
Tool Holder: Shaded display
Click the Run button.
The simulation is run with the tool displayed during simulation.
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
191
CAMWorks Nesting Tutorial
4.
Use the Simulation Speed Control slider to control the speed of
the Simulation.
5.
To pause the simulation while
it is running, click on the Pause
button. When you click
Run
button again, the Simulation will
continue from the point where it
was paused.
6.
Click the Close button in the
upper right corner of the
Simulation toolbar to exit the
simulation mode and return to
the SOLIDWORKS display.
Toolpath Simulation
Step 12: Post Processing Toolpaths
Post processing is the final step in generating the NC program file. When you
use a CAMWorks internal post processor, this step translates generalized
toolpath and operation information into NC code for a specific machine tool
controller. CAMWorks creates NC code for each toolpath in the order the
operation appears in the CAMWorks Operation tree. When you post process a
part, CAMWorks creates two files: the NC program and the Setup Sheet. These
are text files that you can read, edit and print using a word processor or text
editor.
In this tutorial, you will post process all the operations and generate the NC
program:
1.
Click the Post Process button on the CAMWorks Command Manager.
OR
Right click on the CAMWorks NC Manager in the Operation tree and select
Post Process on the context menu.
The Post Output File dialog box is displayed so that you can save the NC
program file.
Typically, the NC program and Setup Sheet files are stored in the folder
that contained the last part that was opened. If you want these files in
another location, you can change the folder location.
Note: If the Post Process command is grayed out on the CAMWorks Command
Manager or on any context menu, make sure that you have selected a post
processor and generated the toolpaths. Refer Step 11 in this tutorial.
192
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
Post Output File dialog box
2. In the Post Output File dialog box, click the down arrow to the right of the
Save as type box.
Step Run
CAMWorks provides a list of
commonly used extensions that
you can select. For this exercise,
use the .txt extension.
Note: If you want change the default
extension from .txt to one of the
ones in the list or if you want a
different file name extension for
NC program files, you can edit or
create a .pinf file and specify the
new extension. For more
information on making these
changes, see the online Help.
3. In the File name textbox, type the
suitable file name, and then click
Save button.
4. The Post Process Output dialog box
is displayed. Click the Step button
on the control bar at the top.
CAMWorks starts to generate the
Post process Output dialog box
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
193
CAMWorks Nesting Tutorial
NC program and the first line of NC code displays in the NC code output
view box. The post processing mode is set to post process one line of
code at a time (Step mode).
5. Click the Step button. The next line of NC code is displayed.
6. Click the Run button
. Post processing continues until it is completed.
7. When the post processing is finished, view the code using the vertical
scroll bar.
8. Click OK to close the dialog box.
Note:
194
To understand the complete the process from defining the machine and
extracting the machinable features to simulating toolpath and generating the
NC code for nested parts using the CAMWorks, refer the Mill Assemblies
Tutorial of CAMWorks. To locate the tutorial, select the Start menu on the
Windows taskbar and follow the path:
All Programs>>CAMWorks201x>>Manuals>>Mill Assemblies Tutorial
Tutorial 12 – Generating NC codes For Nested Layouts using CAMWorks (I)
CAMWorks Nesting Tutorial
TUTORIAL 13 – GENERATING NC CODES FOR
NESTED LAYOUTS USING CAMWORKS (II)
Topics covered in this Tutorial:


Functionality to link CAMWorks Nesting with CAMWorks
Tutorial illustrating how to generate NC Codes for Nested Layouts using
CAMWorks
The previous tutorial explained how to generate NC codes using the CAMWorks
application.
If you are using CAMWorks Nesting 2014 SP1 or a later version in conjunction
with CAMWorks 2014 SP2.2 or a later version, then a new functionality that links
the CAMWorks Nesting output as the input for CAMWorks comes into effect.
In this tutorial, you will learn how to generate NC codes for nested layouts using
CAMWorks when the functionality to link CAMWorks Nesting with CAMWorks is
enabled.
Functionality to link CAMWorks Nesting with CAMWorks
A new functionality provided with CAMWorks Nesting 2014 SP1 version allows
you to automatically link the nested layout output of CAMWorks Nesting as the
input for CAMWorks.
When this functionality is enabled, the nested layouts output generated using
CAMWorks Nesting will be automatically fed as the input assembly for
CAMWorks. This is achieved by automatically listing all the nested parts in the
CAMWorks Part Manager and auto-defining the common stock for the nested
assemblies. This automation saves considerable time by reducing the steps
required to generate the NC code.
The new functionality introduced in CAMWorks Nesting 2014 SP1 version links the
CAMWorks Nesting application with the CAMWorks application. This linking is achieved by:
-
Automatic addition of nested parts in nested layouts to CAMWorks Part Manager
-
Automatic definition of the stock (from which the parts will be machined) in the
CAMWorks Stock Manager.
Pre-requisites for using this functionality
The functionality to link the CAMWorks Nesting application with CAMWorks
application will work if and only if all the below conditions are fulfilled:
 The CAMWorks Nesting version should be CAMWorks Nesting 2014 SP1 or a
later version.
 The CAMWorks version should be CAMWorks 2014 SP2.2 or later version.
 Both CAMWorks Nesting and CAMWorks should be loaded as Add-Ins in
SOLIDWORKS.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
195
CAMWorks Nesting Tutorial

The functionality should be enabled in the DefaultValues.ini Configuration file.
(By default, it is enabled.)
Advantages of this functionality
In CAMWorks Nesting versions prior to the 2014 SP1.0 version, after the nested
layouts were generated, users had to manually add instances of the parts
present in each nested layout to the CAMWorks Part Manager. The settings for
the common stock too had to be manually defined. These steps could be timeconsuming.
From CAMWorks Nesting 2014 SP1 version, the steps for adding parts to the
CAMWorks Part Manager and defining the stock can be automated using this new
functionality.
Refer the flowchart in the previous tutorial to gain an understanding of the
steps involved in generating NC codes and the steps that are automated when
this functionality is used.
Enabling the functionality
The option to link CAMWorks Nesting with CAMWorks is controlled from the
CAMWorks Nesting configuration file DefaultValues.ini through the flag
"AddPartstoCWManager". The functionality is enabled when the flag is set to “1”
and disabled when the flag is set to “0”. By default, this option is enabled.
For more details, read: Enabling/disabling the functionality to add nested parts
to the CAMWorks Part Manager.
How the functionality works
When enabled, the functionality works in the following manner:
1. After nested layouts are generated using CAMWorks Nesting, each nested
layout will be listed in the SOLIDWORKS Configurations Manager.
2. The CAMWorks Nesting application will then check for the presence of the
CAMWorks Add-In.
a. If the CAMWorks Add-In is not dete
cted, then this functionality
will not work.
b. If the CAMWorks Add-In is detected, but it is a version lower than
CAMWorks 2014 SP2.2, then the functionality will not work and the
following error message will be displayed:
CAMWorks Warning Message
196
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
c. If the CAMWorks Add-In is detected and it is CAMWorks 2014 SP2.2 or
a higher version, then this functionality will come into effect. The
CAMWorks Feature Tree tab will be populated in the following manner:
i. If multiple nested layouts are generated after the nesting process,
then each nested layout assembly will be listed under the
Configurations item. If only one nested layout is generated, then it
won‟ be listed under Configurations item.
ii. The parts (instances) present in each nested layout will be
automatically listed in the CAMWorks Part Manager. (Users can
delete unwanted parts listed in the Part Manager using the Delete
option.)
iii. In the CAMWorks Stock Manager, a common stock of type Extruded
Sketch will be automatically defined for the parts present in each
nested layout.
Automatic Definition of Stock in CAMWorks Stock Manager
For each nested layout asembly input into CAMWorks, a common stock of type
Extruded Sketch will be defined in the CAMWorks Stock Manager. The perimeter of
the Sheet used to nest the parts will be used as the sketch for extruding. If
Sheet sketch is not available (for example in cases where is sheet was defined
from a *.dxf file), then the stock of type „Bounding box‟ will be used.
When the functionality to link CAMWorks Nesting with CAMWorks is enabled, then for each
nested layout, the automatic definition of the stock in the CAMWorks Stock Manager will
have the following properties:
-
The stock created will be a common stock from which all the nested parts will be
machined.
-
The stock type will be Extruded Sketch where the dimensions (length and breadth of
the cuboid stock will be derived from a sketch).
-
The sketch picked for defining this stock will be the sketch representing the
dimensions of the sheet in which the parts are nested. (The sketch representing the
dimensions of the sheet will be listed in the SOLIDWORKS FeatureManger Design
Tree after the nested layouts are generated.)
-
The height of the stock will be equivalent to the thickness of the parts.
Tutorial illustrating Generating of NC codes for Nested
Layouts
This tutorial is divided into two sections:
 Section I illustrates how to generate Nested layouts for the example parts
using the CAMWorks Nesting application.
 Section II illustrates how to generate NC codes for the Nested layouts.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
197
CAMWorks Nesting Tutorial
Section I: Generating Nested layouts
In this section, you will nest an assembly comprising two native sheet metal
parts of different thicknesses.
1. In the configuration file DefaultValues.ini (located within the CAMWorks Nesting
Installation folder), ensure that the flag FixComponent under [NestingData]
section is set to „1‟.
This setting will ensure that after the Nested layouts are generated, the
parts in the Nested layout assembly do not get accidentally repositioned.
2. Ensure that both CAMWorks Nesting 2014 and CAMWorks 2014 are loaded as
Add-Ins within SOLIDWORKS.
3. Open the assembly file named Tutorial_13.sldasm located in the following
folder location:
Drive:\CAMWorksNestingData\CAMWorksNesting 201x\Examples\Tutorials\
Assemblies\Tutorial_13
This assembly file comprises of the following two sheet metal parts.
Tutorial_13_a.sldprt
Tutorial_13_b.sldprt
4. Select the Create Nest Job command on the CAMWorks Nesting Ribbon
bar.
OR
In the SOLIDWORKS menu bar, select CAMWorksNesting>>Create Nest
Job.
5. The Create Nesting Job dialog box is displayed. In the Part Data tab, assign
the following values to the various parameters:
Part
Thickness
Quantity
Material
Step
Angle
Grain
Direction
Tutorial_13_a.sldprt
1 mm
12
Steel
900
None
Tutorial_13_b.sldprt
3 mm
12
Steel
900
None
6. Since the two parts to be nested have different thicknesses, two different
sheets of varying thicknesses corresponding to the parts need to be
defined. In the Sheet Data tab, add two Custom size sheets with the
following dimensions and values assigned to the parameters:
198
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
Sheet Name
Length
(mm)
Width
(mm)
Thickness
Material
Quantity
Grain
Assembly
Direction Template
CustomSheet1
500
200
1 mm
Steel
1
None
Default
CustomSheet2
250
250
3 mm
Steel
1
None
Default
7. Within the Multi head options tab, in the Machine Data group box, ensure
that the Machine selected is SingleTHMachine (a machine with a single tool
head). The Number of tool heads for the machine will display 1.
8. In the Nesting Data group box:
- Assign a Part to part distance of 5mm and Part to sheet distance of 5mm.
-
Select Fast Nesting as the Nesting Type.
-
If you wish to save the output nested assembly in a folder location
other than the default location, then specify the location in the Output
Assembly field by using the
-
Browse button.
Ensure that the Save output as dxf option is unchecked.
9. Click the OK button to execute the Nesting command.
10. CAMWorks will display the warning message
11. CAMWorks Nesting will display a warning message prompting whether
you wish to add the nested parts to CAMWorks Part Manager
automatically.
CAMWorks Nesting Warning Message
12. Two nested layouts will be generated. These nested layouts will be saved
as a SOLIDWORKS Assembly file (*.sldasm).
13. The Summary text file indicates that all the parts have been nested. Close
this text file.
14. In the SOLIDWORKS left hand side panel, click on the
SOLIDWORKS
ConfigurationsManager tab. Observe that the nested layouts are listed
under this tab.
You can switch the nested layout assembly currently displayed in the
graphics area by double-clicking on the desired nested layout assembly
listed under this tab.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
199
CAMWorks Nesting Tutorial
Double-click on Layout 2 to display it in the graphics area. (The first
nested layout is usually displayed in the graphics area by default.)
SOLIDWORKS ConfigurationsManager Tree
15. Click on the SOLIDWORKS FeatureManager Design Tree tab. Observe that
the sketches for the three sheets are listed in this tab. These sketches will
be used to define the common stock (of type Extruded Sketch) for each
nested layout assembly.
Section II: Generating NC codes using CAMWorks
Step 1: Defining the Fixture Coordinate System for the Machine
The Fixture Coordinate System defines the “home point” or “main zero” position
on the machine. It defines the default G-code origin, defines the XYZ machining
directions and acts as a reference point, if subroutines are used. This
coordinate system needs to be defined in the SOLIDWORKS FeatureManager
Design Tree.
Following are the steps to define the Fixture Coordinate System:
1. If necessary, rotate and zoom the nested layout assembly in the graphics
area to clearly view the position where you desire to assign the
coordinate system.
2. Click the Insert menu on
the SOLIDWORKS menu
bar.
3. From the dropdown
menu, select Reference
Geometry and then select
the Coordinate System
from the cascading
menu.
Selecting „Coordinate System‟ from cascading menu
The Coordinate System dialog
box is displayed.
4. In the graphics area, click on
the point you wish to assign
as the Coordinate System origin.
This action will display the
selected coordinate system
origin in the Selection field of
the dialog box.
200
XYZ machining direction
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
5. The XYZ machining direction should be same as displayed in the image on
the right. If necessary, click on the Reverse Axis Direction button to obtain
the correct machining direction.
6.
Click the OK button to save the changes and close the dialog box.
The defined coordinated system is listed under the FeatureManager Design
Tree.
Step 2: Defining the Machine
Before you machine the Nested layout assemblies, you need to define the
Machine that will be used to machine the assembly.
1. In the SOLIDWORKS left hand side panel, click on the
CAMWorks
Feature Tree tab. (Note that this tab will be visible only if CAMWorks is
loaded as an Add-In within SOLIDWORKS)
2. Double-click on the
Machine item (Machine [Mill - metric] in this case) to
open the Machine dialog box.
3. The Machine tab of the Machine dialog box is displayed. This tab allows
you to select the machine that the assembly will be machine on. By
default, either the Mill - metric or Mill - inch will be already selected.
If you wish to select any other Mill machine or a user-defined Machine definition, then
highlight it in the Available Machines list and click the Select button.
4. Click on the Tool Crib tab, ensure that Tool crib1 (metric) is selected.
To select an alternative tool crib, select the desired tool crib In the Available tool cribs
list box and click on the Select button.
5. Click on the Post Processor tab. This tab allows you to select a post
processor for generating NC codes or for generating enhanced CL files
that can be used by external third party post processing programs.
By default, the sample post processor M3AXIS-TUTORIAL is selected. For
this tutorial, this default post processor will be used.
If you wish to use another post processor or a customized post processor provided to
you by your CAMWorks Reseller, then highlight the desired post processor in the
Available list and click the Select button. If the post processor is not listed, then click
on the Browse button to navigate to the folder where the post processor file is located.
6. Click on the Setup tab. This tab allows you to set the Fixture Coordinate
System for the machine.
-
Since a 2.5 Axis/ 3 Axis Mill Machine will be used to machine the
assembly, Indexing will remain set to None.
-
In the CNC comp options group box, ensure that the Calculate safe CNC
comp toolpath option is checked.
-
In the Fixture Coordinate system group box, highlight Coordinate System1
in the Coordinate systems list box.
This highlighted entity will be displayed in the Selected entity list box.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
201
CAMWorks Nesting Tutorial
7. Click OK to apply the
changes and close the
Machine dialog box.
8. In the CAMWorks Feature
Tree, under the
Configurations item,
double-click Layout 2 to
display it in the graphics
area. Click Yes within the
Warning Message dialog
box displayed.
9. Double-click on the
Machine item (Machine
[Mill - metric] in this case)
to open the Machine
dialog box.
10. Click on the Setup tab.
This tab allows you to set
the Fixture Coordinate
System for the machine.
11. In the Fixture Coordinate
Setup tab of Machine Dialog Box
System group box,
highlight Coordinate System1 in the Coordinate systems list box. This
highlighted entity will be displayed in the Selected entity list box.
12. Click OK to apply the changes and close the Machine dialog box.
Step 3: Verifying the Addition of Parts in the CAMWorks Part Manager
With the new functionality to link CAMWorks Nesting and CAMWorks, for each
Nested layout, the nested parts will be automatically added to the CAMWorks
Part Manager.
In this step, you will verify the automatic addition of parts to the CAMWorks Part
Manager for each nested layout.
1. In the SOLIDWORKS left hand side panel, click on the
Feature Tree tab.
CAMWorks
2. Within this tab, click on the ( ) plus sign to expand the
Configurations
item. Observe that the two nested layout assemblies generated are listed
under Configurations. (Note that if only one nested layout is generated
after the nesting process, then it will not be listed under Configurations.)
3. Expand the Part Manager item (if not already expanded) by clicking on the
( ) plus sign to its left. Under Part Manager:
-
202
The part name (Tutorial_13_a.sldprt) is listed under the Part Manager.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
-
A Feature Manager, which is created for each part, is used to define
the Mill Part Setups and machinable features associated to the seed
part.
-
For each unique part, all the instances are listed under the
Instances item. Observe that all 12 instances of the part in the nested
layout assembly are listed.
- When you highlight an instance of the part listed under Instances, the
corresponding part will be highlighted in the graphics area.
- To delete an instance of the part, highlight the instance of the part
under Instances and press the Delete button.
4. Under the Configurations item, double-click Layout 2. Click Yes within the
Warning Message dialog box displayed. The graphics area will now display
the second nested layout assembly.
(Alternatively, you can change the nested layout displayed in the graphics
area by using the SOLIDWORKS ConfigurationsManager tab.)
5. Once again, expand the items listed under Part Manager and observe that
all the instances of the part (Tutorial_13_b.sldprt) have been listed under
Part Manager.
Step 4: Automatic Stock Definition
With the new functionality to link CAMWorks Nesting and CAMWorks, for each
Nested layout, the stock definition will be automatically loaded in the CAMWorks
Stock Manager.
The Stock Manager allows you to customize the stock associated with the parts.
In this step, you will verify the stock definition that was automatically defined in
the CAMWorks Stock Manager.
1. In the CAMWorks Feature Tree, under
the Configurations item, double-click
Layout 1 to display it in the graphics
area. Click Yes within the Warning
Message dialog box displayed.
2. Double-click on the Stock Manager
item in the CAMWorks Feature tree.
OR
Right click Stock Manager item in the
CAMWorks Feature tree and select
Edit Definition on the context menu.
3. The Stock Manager dialog box is
displayed. Observe that:
-
In the Stock Type group box,
the selected Stock Type is
Command to open the Stock Manager dialog
box
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
203
CAMWorks Nesting Tutorial
Extruded Sketch.
4.
-
In the Extruded Sketch group box, the
Depth of the stock is set to
1mm. (This is equal to the thickness of the parts being nested).
-
In the Stock Size group box, the dimensions of the stock in the X, Y and
Z directions are indicated. The X (500 mm) and Y (200 mm) values
correspond to the dimensions of the sheet used for creating the nested
layout. The Z value (1mm) is equal to the thickness of the parts being
nested
-
In the Create Stock group box, the
Stock form selected is Common Stock.
(This selection indicates that all the
parts in the nested layout assembly will
be machined from a common stock.)
Click Cancel to close the Stock Manager
dialog box.
5. If required, you can similarly check the
stock definition for the Layout2.
„Common‟ is selected in the
Create Stock group box
Step 5: Defining Machinable Features and Interactively Inserting Features
Extracting Machinable Features for Layout 1:
The next step is to interactively insert Boss features after extracting the
machinable features using the Automatic Feature Recognition (AFR) technology
available in CAMWorks. Machinable Features thus recognized are added under
the
Feature Manager item of the CAMWorks Feature Tree.
At the Mill Part Setup level, features can be inserted interactively using the New 2.5 Axis
Feature or New Multi Surface Feature commands. CAMWorks automatically copies the
features to every other instance of the part selected in the Part Manager.
When machining multiple instances of the same part, if you only want to create one
instance of the feature, you can use the Assembly Feature command on the feature
context menu to declare the feature an Assembly Feature. By doing so, CAMWorks will
not copy the feature to all instances of the part.
In this tutorial, you will discard the machinable features that were extracted
automatically by executing the Extract Machinable Features command since the
machinable features recognized are not suitable for sheet metal machining.
Instead, you will interactively insert the Boss Features that define the perimeter
of the part.
Following are the step to recognize features automatically:
1. Ensure that Layout 1 is displayed in the graphics area.
204
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
2.
Click the Extract Machinable Features button on the CAMWorks Command
Manager.
OR
In the SOLIDWORKS menu bar, click on the CAMWorks menu and select
Extract Machinable Features command.
OR
Right click CAMWorks NC Manager in the CAMWorks Feature tree and select
Extract Machinable Features on the context menu.
3. The Message Window is displayed. This window is displayed automatically to
report the progress of the current process. Close this message window.
4. On execution of the Extract Machinable Features command, CAMWorks
generates the Mill Part Setup and the machinable features. The items are
displayed in the CAMWorks Feature tree.
5.
Click the plus sign next to the Feature Manager in the Feature tree.
The Feature Manager displays all the Mill Part Setups and machinable
features that were created by Automatic Feature Recognition.
Deleting the Mill Part Setups and Features from Layout 1:
In this tutorial, you will have to delete
Mill Part Setups and features and then
insert the Boss Feature interactively.
1. Press the Ctrl key on the keyboard
and left-click on Mill Part Setup2, Mill
Part Setup3, Mill Part Setup4 and Mill
Part Setup5 in the Feature Manager to
highlight the items.
2. Right click on the Mill Part Setup5 and
select Delete on the context menu.
3. CAMWorks will display a warning
message asking whether you are
sure about deleting the Mill Part
Setups and all dependent items. Click
Yes to confirm to deletion.
4. The features are moved to the
Recycle Bin. When a feature is
deleted, it is automatically placed in
the Recycle Bin, which is used to
store machinable features that you
do not intend to machine.
Selecting the Mill Part Setups to delete it
5. Click the ( ) minus sign to the left of the Recycle Bin to collapse it.
6. Similarly, you will delete all the features extracted in the Mill Part Setup1.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
205
CAMWorks Nesting Tutorial
7. Under Mill Part Setup1, click on
the first feature (i.e. Rectangular
Slot 1) and hold down the Shift key
on the keyboard and then click
on the last feature (i.e.
Rectangular Slot Group3) to
highlight all the items.
8. Right click and then select Delete
on the context menu. Click Yes
to confirm the deletion.
The features are moved to the
Recycle Bin.
9. Right click on the Recycle Bin
under the Feature Manager and
select the Empty on the context
menu.
Deleting all the features from Mill Part Setup1
10. CAMWorks will display a warning message asking whether you are sure
about emptying the Recycle Bin. Click Yes to confirm the process.
Interactively inserting Boss Feature in Layout 1:
After deleting the unwanted features and Mill part Setups, you will now
interactively insert the Boss Feature by using the New 2.5 Axis Feature command.
Following are the steps to insert the boss feature interactively:
1.
Right click on the Mill Part Setup1 in the CAMWorks Feature tree and select
the New 2.5 Axis Feature command on the context menu.
The 2.5 Axis Feature Wizard: Feature & Cross Section Definition dialog box is
displayed.
2. Select Boss as the Feature type from the
dropdown list.
3. Highlight in the Entities selected field to
set the focus.
4. Select the lower edge of the left corner
part in the graphics area as shown in
the image on right (highlighted in orange).
This action will display the Loop <1> in
the field of Entities selected.
5. Click Next to display the 2.5 Axis Feature
Wizard: End Conditions dialog box.
Select the bottom edge of the left corner
part
6. Set the depth to 1mm. (This is equal to the thickness of the parts being
nested).
7. If required, remove the check from the check box next to the Reverse
direction option in order to correct the direction.
206
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
8. Click Finish to insert the Irregular Boss feature under the Mill Part Setup1.
9. Click Close to exit the 2.5 Axis Feature Wizard dialog box.
Observe that the interactively inserted Boss feature is listed under Setup1 at
the bottom of the CAMWorks Feature Tree.
Interactively Inserting Mill Part Setup and Machinable Feature For Layout 2:
For Layout 2 in this tutorial, you will insert both the Mill Part Setup and Boss
Feature interactively.
Following are the steps to interactively insert Mill Part Setup and machinable
feature:
1. In the CAMWorks Feature Tree, under the Configurations item, double-click
Layout 2 to display it in the graphics area. Click Yes within the Warning
Message dialog box displayed.
2. Right-click on the Feature Manager under
the Tutorial_13_b.sldprt of CAMWorks
Feature tree and select New Mill part
Setup on the context menu.
The Mill Part Setup dialog box is
displayed.
3. Click on the left corner side part in the
graphics area as shown in the image on
right (highlighted in blue).
4. Make sure the direction (indicated by red
arrow) is correct on the
feature. If not, place a check
in the check box next to the
Reverse direction option.
Select left corner part highlighted in blue
5. Click OK to insert the setup
and close the dialog box.
Mill Part Setup1 is now listed
under Feature Manager in the
tree.
6.
Right click on the Mill Part
Setup1 in the CAMWorks
Feature tree and select the
New 2.5 Axis Feature command
on the context menu.
The 2.5 Axis Feature Wizard:
Feature & Cross Section Definition
dialog box is displayed.
7. Select the Feature type as
Boss from the dropdown list.
8. Click within the Entities selected
Mill Part Setup dialog box
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
207
CAMWorks Nesting Tutorial
field to set the focus and select the left corner part in the graphics area.
This action will display the Face <1> in the field of Entities selected.
9. Click Next button to display the 2.5 Axis Feature Wizard: End Conditions dialog
box.
10. Set the depth to 3mm. (This is equal to the thickness of the parts being
nested).
11. If required, remove the check from the check box next to the Reverse
direction option to correct the direction of the defined feature.
12. Click Finish to insert the Rectangular Boss feature under the Mill Part Setup1.
13. Click Close to exit the 2.5 Axis Feature Wizard dialog box.
Step 6: Sorting Part Instances to Determine Machining Order
When part instances are automatically added or manually added using the Add
All Instances button, the instances need not necessarily be listed in the best
machining order. CAMWorks provides options for sorting part instances to be
processed in a more efficient order.
The order in which the part instances are listed under the feature is the
machining order for that feature. By default, the parts for all features are in the
order they appear in the Part Manager. You can change the order globally for all
features or for individual features.
Following are the steps to sort instances:
1. Ensure that Layout 1 is displayed in the graphics area.
2.
3.
Under Setup1 in the CAMWorks Feature tree, click on the ( ) plus sign
next to the feature to expand the feature items.
Double click Part Manager in the CAMWorks Feature tree.
4. Click the Sort Instances button in the Manage Parts dialog box.
The Sort Instances dialog box is displayed.
5. Select the Grid pattern option.
6. Set the following options for Grid Pattern and then click the OK button.
- Start corner = Bottom left
-
Direction = Horizontal
-
Pattern = Zigzag
7. Click OK to close the Manage Parts dialog box.
8. Click the ( ) plus sign next to any feature listed under Setup1 and click each
part instance to view the machining order of the features in the graphics
area.
9. In the CAMWorks Feature Tree, under the Configurations item, double-click
Layout 2 to display it in the graphics area. Click Yes within the Warning
Message dialog box displayed.
10. Repeat the same steps from 2 to 8 for Layout 2.
208
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
Sort Instances Dialog Box
Step 7: Generating the Operation Plan and Adjusting Operation Parameters
When Generate Operation Plan command is executed, operations for
machinable feature are created automatically based on information in the
CAMWorks Technology Database.
Generating Operation Plan for Layout 1:
1. Ensure that Layout 1 is displayed in the graphics area.
2.
Click the Generate Operation Plan button on the CAMWorks Command
Manager.
OR
Right click the CAMWorks NC Manager of the Feature tree and select Generate
Operation Plan on the context menu.
In the Operation tree, the generated
operation Contour Mill1 is displayed under
Setup1.
Generated Operation listed in
Contour Mill1 operation is used for the
Operation Tree
Irregular Boss feature of the part.
3. In the Operation tree, double click Contour Mill1.
OR
Right click Contour Mill1 and select Edit Definition on the context menu.
The Operation Parameters dialog will be displayed.
4. Under Tool tab, click on the Mill tool page. Observe that a tool of 40mm
diameter is used to machine the Irregular boss feature. This irregular boss
feature represents the perimeter of the part. Since the Part to part distance
and Part to Sheet distance assigned before creating the nested layout was
5mm, selecting any tool with more than 5mm diameter will gouge the part.
Hence, the tool used to machine this operation needs to be changed to a tool
with a diameter 5mm or less.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
209
CAMWorks Nesting Tutorial
5. Click on the Tool tab and select the Tool Crib page.
6. Highlight the Flat End tool with diameter of 3mm within the list of displayed
tools.
7. Click the Select button. This
action will assign the
highlighted tool as the tool
to be used for machining
this operation.
8. CAMWorks will display a
warning message which
prompts you to select
whether the corresponding
CAMWorks Warning Message
holder of the tool is also to be
changed. Click Yes to replace the corresponding holder.
9. Click OK to apply the changes and close the Operation Parameters dialog
box.
Generating Operation Plan for Layout 2:
1. In the CAMWorks Feature Tree, under the Configurations item, double-click
Layout 2 to display it in the graphics area. Click Yes within the Warning
Message dialog box displayed.
2.
Click the Generate Operation Plan button on the CAMWorks Command
Manager. OR
Right click the CAMWorks NC Manager of the Feature tree and select Generate
Operation Plan on the context menu.
In the Operation tree, the generated Contour Mill1 operation is listed under
Setup1. Contour Mill1 operation is used for the Rectangular Boss feature of the
part. For this operation too, the tool used to machine the operation needs to
be replaced with a tool of 5mm or less.
3. Double click Contour Mill1 in the Operation tree.
OR
Right click Contour Mill1 in the Operation tree and select Edit Definition on the
context menu.
The Operation Parameters dialog box is
displayed.
4. Click on the Tool tab and select the Tool Crib
page.
Generated Operation listed in
Operation Tree
5. Highlight the Flat End tool with diameter 5mm or
less. For this tutorial, select the 4mm diameter Flat End mill within the list
for this operation and then click the Select button.
6. CAMWorks will display a Warning message. Click Yes to replace the
corresponding holder.
7. Click OK to apply the changes and close the Operation Parameters dialog
box.
210
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
Step 8: Defining G-code Program Zero Location
1. Ensure that Layout 1 is displayed in the graphics area.
2.
Double click Setup1 in the Operation tree.
The Setup Parameters dialog box is displayed.
3. On the Origin tab, make sure Part Setup origin is selected for the Output origin.
Note that when Setup origin is selected, you can specify the origin using
several methods.
4. Click on the Offset tab.
5. In the Sort by group box, select Grid pattern.
When you pick this option, the parts in the table are automatically reordered
based on the current settings for Start corner, Direction and Pattern.
6. Set the Grid pattern parameters to the same settings you used when sorting
part instances for the machining order:

Start corner= Bottom left

Direction= Horizontal

Pattern= Zigzag
7. Set the Work coordinate offset to Work Coordinate. This option will output
G54, G55, etc.
8. Set the Start value to 54 and the Increment to 1.
9. Click the Assign button of the Work Coordinate offset group box. Observe
that the numbers are updated in the Offset and Sub columns in the table.
10. Click OK to close the Setup Parameters dialog box.
11. In the CAMWorks Operation Tree, under the Configurations item, double-click
Layout 2 to display it in the graphics area. Click Yes within the Warning
Message dialog box displayed.
12. Repeat the same steps from 2 to 10 for Layout 2.
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
211
CAMWorks Nesting Tutorial
Setup Parameters Dialog Box (For Layout 1)
Step 9: Generating Toolpaths
CAMWorks calculates toolpaths using the operation parameters to define how to
machine each machinable feature.
1. Ensure that Layout 1 is displayed in the graphics area.
2.
Click the Generate Toolpath button on the CAMWorks Command Manager.
OR
Right click Setup1 in the Operation tree and select Generate Toolpath on the
context menu.
On executing the Generate Toolpath command, the toolpath is generated for
all the operations in the Setup.
3. Under the Configurations item, double-click Layout 2 to display it in the graphics
area. Click Yes within the Warning Message dialog box displayed.
4. Click the Generate Toolpath button on the CAMWorks Command Manager to
generate the toolpath.
212
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
CAMWorks Nesting Tutorial
Step 10: Simulate Toolpaths
CAMWorks provides the ability to simulate the toolpaths showing the tool
movement and the resulting shape of the part/assembly on machining the
stock.
1. Ensure that Layout 1 is displayed in the graphics area.
2.
Click the Simulate Toolpath button on the CAMWorks Command Manager.
OR
Right click on Setup1 in the operation tree and select Simulate Toolpath on the
context menu.
The Toolpath Simulation toolbar is displayed.
3. Set the following display options:
- Stock: Translucent display
4.
-
Tool: Shaded display
-
Tool Holder: Shaded display
Click the Run button.
The simulation is run with the tool and holder displayed during simulation.
5.
Click the Close button to exit the simulation mode and return to the
SOLIDWORKS display.
6. To view the toolpath simulation for Layout 2, switch the display to Layout2 in
the graphics area using the SOLIDWORKS Configuration Manager or
Configurations item in the CAMWorks Feature Tree and follow the same steps.
Toolpath Simulation for Layout 1
Toolpath Simulation for Layout 2
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
213
CAMWorks Nesting Tutorial
Step 11: Generate the NC code
Following are the steps to generate the NC program. Note that NC code needs
to be generated separately for Layout1 and Layout2.
1.
Click the Post Process button on the CAMWorks Command Manager.
OR
Step Run
Right click on the CAMWorks NC
Manager in the Operation tree and
select Post Process on the context
menu.
The Post Output File dialog box is
displayed so that you can save the
NC program file.
2. By default, NC files are stored into
the folder that contained the last
part model or assembly that was
opened in SOLIDWORKS. If you
want to save these files in another
location, you can change the folder
location.
3. In the Post Output File dialog box,
type the suitable file name, and
then click Save button.
The Post Process Output dialog box is
displayed.
4. Click the Step button
on the
control bar at the top of the dialog
box.
Post Process Output dialog box
5. CAMWorks begins to generate the NC program and the first line of NC code
displays in the NC code output view box.
6. Click the Step button again. The next line of NC code is displayed.
7.
Click the Run button. Post processing continues until it is completed.
When the post processing is finished, view the code using the vertical scroll
bar.
8. Click OK to close the dialog box.
9. Repeat the steps 1 to 8 for Layout2 in order to generate NC code for it.
214
Tutorial 13 – Generating NC codes For Nested Layouts using CAMWorks (II)
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertising