SolidWorks 2001 Getting Started User Manual

Below you will find brief information for SolidWorks 2001. This manual introduces basic concepts and terminology, providing exercises for creating parts, drawings, and assemblies. Learn to create a base feature, add bosses, cuts, modify features, and display section views.

PDF

Document

SolidWorks 2001

Getting Started

300 Baker Avenue

Concord, Massachusetts 01742 USA

U.S. Patent 5,815,154

SolidWorks Corporation is a Dassault Systemes

S.A. (Nasdaq:DASTY) company.

The information and the software discussed in this document are subject to change without notice and should not be considered commitments by

SolidWorks Corporation.

No material may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose without the express written permission of SolidWorks Corporation.

As a condition to your use of this software product, you agree to accept the limited warranty, disclaimer and other terms and conditions set forth in the SolidWorks Corporation License and

Subscription Service Agreement, which accompanies this software. If, after reading the

License Agreement, you do not agree with the limited warranty, the disclaimer or any of the other terms and conditions, promptly return the unused software and all accompanying documentation to SolidWorks Corporation and your money will be refunded.

The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of this license. All warranties given by SolidWorks

Corporation as to the software and documentation are set forth in the SolidWorks Corporation

License and Subscription Service Agreement, and nothing stated in, or implied by, this document or its contents shall be considered or deemed a modification or amendment of such warranties.

SolidWorks

and the SolidWorks logo are the registered trademarks of SolidWorks Corporation.

SolidWorks 2001 is a product name of

SolidWorks Corporation.

FeatureManager

® is a jointly owned registered trademark of SolidWorks Corporation.

Feature Palette™ and PhotoWorks™ are trademarks of SolidWorks Corporation.

Document Number: SWGSDENG011501

ACIS

is a registered trademark of Spatial

Technology Inc.

IGES

Access Library is a registered trademark of IGES Data Analysis, Inc.

FeatureWorks™ is a trademark of Geometric

Software Solutions Co. Limited.

GLOBEtrotter

and FLEXlm

are registered trademarks of Globetrotter Software, Inc.

Other brand or product names are trademarks or registered trademarks of their respective holders.

COMMERCIAL COMPUTER

SOFTWARE - PROPRIETARY

U.S. Government Restricted Rights. Use, duplication or disclosure by the Government is subject to restrictions as set forth in

FAR 52.227-19 (Commercial

Computer Software - Restricted Rights),

DFARS 252.227-7013(c)(1)(ii)(Rights in

Technical Data and Computer Software) and in the license agreement, as applicable.

Contractor/Manufacturer:

SolidWorks Corporation, 300 Baker Avenue,

Concord, Massachusetts 01742 USA

Portions of this software are copyrighted by and are the property of Unigraphics Solutions Inc.

D-Cubed Limited.

LightWork Design Limited.

Geometric Software Solutions Co. Limited.

Immersive Design, Inc.

Viewpoint Corporation

1998 IGES Data Analysis, Inc.

Contents

Mastering the Basics

Installation 1-1

Basic Functionality 2-1

The 40-Minute Running Start

Assembly Basics

Drawing Basics

Design Tables

More about Basic Functionality

3-1

4-1

5-1

6-1

Working with Features and Parts

Revolve and Sweep Features

Loft Features

Pattern Features

Fillet Features

More about Features and Parts

Working with Assemblies

Assembly Mates

Advanced Design Techniques

More about Assemblies

7-1

8-1

9-1

10-1

11-1

12-1

SolidWorks 2001 Getting Started iii

Working with Drawings and Detailing

Advanced Drawings and Detailing

Bill of Materials

More about Drawings and Detailing

13-1

14-1

Special Topics

Sheet Metal Part

Mold Design

3D Sketching

15-1

16-1

17-1

Importing Files / Using FeatureWorks Software 18-1

Learning to Use PhotoWorks 19-1

SolidWorks Animator 20-1

More about SolidWorks Functionality

SolidWorks 2001 Getting Started

Mastering the Basics

Installation

Basic Functionality

The 40-Minute Running Start

Assembly Basics

Drawing Basics

Design Tables

More about Basic Functionality

Installation

What is SolidWorks 2001?

SolidWorks

2001 is mechanical design automation software that takes advantage of the familiar Microsoft

Windows

graphical user interface. This easy-to-learn tool makes it possible for mechanical designers to quickly sketch out ideas, experiment with features and dimensions, and produce models and detailed drawings.

This Getting Started book discusses some basic concepts and terminology used throughout the SolidWorks 2001 application. It provides exercises to familiarize you with creating parts, drawings and assemblies, and introduces some of the most commonly used features of the SolidWorks 2001 mechanical design automation system.

This chapter provides an overview of the following topics: q

System requirements for installing and using SolidWorks 2001 software q

Installing the SolidWorks 2001 software q

SolidWorks 2001 service packs q

The SolidWorks Web site

SolidWorks 2001 Getting Started 1-1

Mastering the Basics

Preparing to Install the SolidWorks 2001 Software

System Requirements

For the most recent information about system requirements, refer to the SolidWorks 2001

Read This First.

Required Information for Installation

Before you install SolidWorks 2001, if you made changes to palette items, drawing templates, or PhotoWorks

materials in a previous release of the SolidWorks software, you should save backup copies of these files. Put the backup files in a folder where they cannot be lost or overwritten during the installation.

The SolidWorks 2001 Setup Wizard on the CD-ROM guides you through the installation procedure and asks for the following information: q

SolidWorks Serial Number. For new SolidWorks customers or non-subscription customers, the serial number is located on the box that contains your SolidWorks software. Subscription customers should continue to use the serial number on the

CD-ROM case from their first SolidWorks installation.

SolidWorks Registration Code:

• If you are a SolidWorks subscription customer, the registration wizard provides a registration code during the SolidWorks 2001 installation.

•

If you are a new SolidWorks customer, you are asked to use the registration wizard during installation. This generates a registration form that you can email or fax to

SolidWorks Corporation. A registration code is provided quickly by return email or fax. You have up to 30 days to use the product without the registration code.

•

If you are a continuing, non-subscription customer, you must have a registration code to update to the SolidWorks 2001 software.

Serial numbers for add-in software. If you purchased one or more of the software add-ins available with the SolidWorks application, a serial number for each purchased add-in is located on the box that contains your software add-ins. q

Allow or disallow model changes from drawing. This option makes it possible for a user to disallow the ability to make changes to part or assembly dimensions from the drawing. (You must reinstall the SolidWorks software to change this option.) The default, and most common configuration, is to allow the part and assembly dimensions to be changed from the drawing.

1-2

Chapter 1 Installation

Installation Procedures

The kinds of installations are, individual, client, server and client, and server only. The installation steps for an individual user or a server are the same, though some of the questions asked during the installation are different. q

Individual installation - This installation is for a computer that will run the

SolidWorks 2001 application from its own hard drive and will not share its executable files with any other computer, whether it is on a network or not.

• To do an individual installation, insert the SolidWorks 2001 CD-ROM in the computer’s CD drive and respond to the directions from the install wizard.

• A serial number and registration code are required.

Server only installation - This installation is for a computer that will not run the

SolidWorks 2001 application, but will only act as a server, sharing its SolidWorks installation with one or more SolidWorks client computers. (You must reinstall if you want to change this selection.) With this option, the server does not need to be licensed to run the SolidWorks application, but each client must have a license.

This installation should be performed by a network administrator or someone who has experience working with the network server.

NOTE:

The server and clients must be of the same platform type. There is no cross-platform installation.

Before starting a SolidWorks server update installation, it is important to ensure that no SolidWorks clients are running.

•

Insert the SolidWorks 2001 CD-ROM in the computer’s CD drive and respond to the directions from the install wizard.

•

No serial number or registration code is required for a computer that is used exclusively as a server.

•

After installation, make sure that the folder containing the SolidWorks installation is shared and accessible to the client computers on the network.

Server and Client Installation - This installation is for a computer that will run the

SolidWorks 2001 application, and will also act as a server, sharing its SolidWorks installation with one or more SolidWorks client computers.

•

To do a server and client installation, insert the SolidWorks 2001 CD-ROM in the computer’s CD drive and respond to the directions from the install wizard.

•

A serial number and registration code are required.

•

After installation, make sure that the folder containing the SolidWorks installation is shared and accessible to the client computers on the network.

Client installation - The client computer runs the SolidWorks software from a server.

No executable files are installed on the client computer, but it is necessary to perform a

SolidWorks 2001 Getting Started 1-3

Mastering the Basics

SolidWorks client installation to prepare the client computer for sharing the application.

To perform a SolidWorks client installation:

Make certain that the server installation is complete on the computer from which the clients will run the SolidWorks application. Make make sure that the folder containing the SolidWorks installation is shared and accessible to the client computers on the network.

Working on the SolidWorks client computer, browse to the folder under the

SolidWorks installation directory on the server called

setup\i386

Double-click

setup.exe.

The install wizard guides you through the few steps needed to complete the client installation.

NOTE:

After installation, to learn about the new functionality in SolidWorks 2001, click

Help, SolidWorks 2001 Online User’s Guide

on the main toolbar.

SolidWorks 2001 Service Packs

If you are a SolidWorks subscription customer, you can take advantage of SolidWorks service packs that are regularly posted on the SolidWorks Web site. These service packs contain software updates and enhancements to the SolidWorks 2001 software.

To check for a new service pack:

Click

Help, Service Packs

The

Service Packs

dialog box appears.

Click Check. The software checks the SolidWorks Web site to see if you have the latest service pack installed.

To have the software automatically check the SolidWorks Web site once a week for a new service pack, click the

Check for a new service pack once a week

check box.

Click

to close the

Service Packs

dialog box.

Visiting the SolidWorks Web Site

If your computer has access to the Internet, you can visit the SolidWorks Web site after you complete the installation. You can learn more about the SolidWorks company and products by clicking in the

Help

menu on the main SolidWorks window.

1-4

To access the SolidWorks Web site:

Click

Help, About SolidWorks 2001

Click

Connect

to visit the SolidWorks Web site.

Some of the available topics are:

• News and Events

• Technical Support

• VARs and Distributors

• The SolidWorks Design Gallery

Chapter 1 Installation

SolidWorks 2001 Getting Started 1-5

Basic Functionality

SolidWorks 2001 is supported under the Microsoft Windows graphical user interface.

SolidWorks 2001 Getting Started assumes that you have used Windows before and know basic Windows skills, such as how to run programs, resize windows, and so on.

Before you begin the examples in SolidWorks 2001 Getting Started, you should read

Chapter 2, to familiarize yourself with some of the fundamentals, including: q

SolidWorks 2001 design concepts q

SolidWorks 2001 terms q

Getting Help in SolidWorks 2001

SolidWorks 2001 Getting Started 2-1

Mastering the Basics

Designing with SolidWorks 2001

As you do the examples in this guide, the design methods you use for parts, assemblies, and drawings, represent a unique approach to the design process.

With SolidWorks 2001, you create 3D parts, not just 2D drawings. You can use these 3D parts to create 2D drawings and 3D assemblies.

CAD: 2D drawings, made up of individual lines SolidWorks 2001: 3D parts q

SolidWorks 2001 is a dimension-driven system. You can specify dimensions and geometric relationships between elements. Changing dimensions changes the size and shape of the part, while preserving your design intent. For example, in this part, the boss is always half as high as the base.

2-2

Parts

Chapter 2 Basic Functionality

A SolidWorks 3D model consists of parts, assemblies, and drawings. Parts, assemblies, and drawings display the same model in different documents. Any changes you make to the model in one document are propagated to the other documents containing the model.

Drawings

Assembly q

You create sketches and use them to build most features. A sketch is a 2D profile or cross section. Sketches can be extruded, revolved, lofted, or swept along a path to create features.

Sketch Sketch extruded 10mm q

You use features to build parts. Features are the shapes (bosses, cuts, holes) and operations (fillets, chamfers, shells, and so on) that you combine to build parts.

Base feature

Boss

Cut

Fillet

SolidWorks 2001 Getting Started 2-3

Mastering the Basics

SolidWorks Terms

Document Windows

SolidWorks document windows have two panels: q

The left panel of the window contains the following:

•

The FeatureManager ® design tree lists the structure of the part, assembly, or drawing. For more information about the FeatureManager design tree, see the

"More about Basic Functionality" chapter.

•

The PropertyManager provides an alternate way of sketching and otherwise interacting with the SolidWorks 2001 application.

•

The ConfigurationManager is a means to create, select, and view multiple configurations of parts and assemblies in a document.

•

Customized third-party add-in panels.

The right panel is the graphics area, where you create and manipulate the part, assembly, or drawing.

Graphics area

Model

Left panel displaying the FeatureManager design tree

2-4

Chapter 2 Basic Functionality

Common Model Terms

You should familiarize yourself with the following terms that appear throughout the

SolidWorks documentation. For more information about terms, see the glossary in the

SolidWorks 2001 Online User’s Guide.

Origin Vertex Edge

Axis

Plane Face

Handles

Handles allow you to dynamically drag and set certain parameters without leaving the graphics area. Active handles are green, inactive handles are gray.

In the SolidWorks 2001

Getting Started book however, you set all parameters within the

PropertyManager in order to familiarize yourself with this method. After you become accustomed to the options in the

PropertyManager, you can experiment with handles on your own.

Handle

For more information about handles, see the SolidWorks 2001 Online User’s Guide.

SolidWorks 2001 Getting Started 2-5

Mastering the Basics

Toolbars

The toolbar buttons are shortcuts for frequently used commands. Some toolbars are always displayed; other toolbars display automatically when you open a document of the related type. For example, when you open an assembly document, the Assembly toolbar appears.

To display or hide individual toolbars:

Click

View, Toolbars

, or right-click the SolidWorks window frame.

A list of all the toolbars is displayed. The toolbars with a check mark beside them are visible; the toolbars without a check mark are hidden. Click the toolbar name to turn its display on or off.

For more information about customizing toolbars, see the "More about Basic

Functionality" chapter.

2-6

Chapter 2 Basic Functionality

Getting Help

If you have questions while you are using the SolidWorks software, you can find answers in several ways: q

For

Online help

, click or

Help, SolidWorks 2001 Help Topics

in the menu bar.

The online help also includes a special section, Overview of New Functionality in

SolidWorks 2001, a summary of the enhancements in SolidWorks 2001. The online help is part of the SolidWorks 2001 Online User’s Guide that provides detailed information about using the SolidWorks software.

For

What’s This help

, click on the Standard toolbar, then click a toolbar icon or a

FeatureManager item. What’s This help is also available for certain items in the graphics area.

For online tutorials that teach you how to create parts, assemblies, and drawings, click

Help, Online Tutorial

. You will also find information on basic SolidWorks software concepts.

For ideas about how to best implement your design, click

Help, Design Portfolio

. The

Design Portfolio uses sample parts to provide design ideas.

For helpful hints, click

Help, Tip of the Day

. To see a tip each time you start

SolidWorks 2001, select the

Show tips at startup

check box in the

Tip of the Day

dialog box.

For help that describes the active dialog box, and provides access to the full online help system, click the

Help

button in the dialog box or press the

key.

For

Tooltips

that identify buttons on a toolbar, point at the button, and a moment later, the tooltip pops up.

As you point at toolbar buttons or click menu items, the

Status Bar

at the bottom of the

SolidWorks window provides a brief description of the function.

For more information and the latest news about the SolidWorks software and company, visit the SolidWorks web site, http://www.solidworks.com, or click

Help

About

SolidWorks 2001

Connect

SolidWorks 2001 Getting Started 2-7

The 40-Minute Running Start

This chapter guides you through the creation of your first SolidWorks model. You create this simple part:

This chapter includes: q

Creating a base feature q

Adding a boss feature q

Adding a cut feature q

Modifying features (adding fillets, changing dimensions) q

Displaying a section view of a part

You should be able to complete this chapter in about 40 minutes.

NOTE:

Some of the illustrations in this book have been modified for clarity.

What you see on your screen may look different from the illustrations.

SolidWorks 2001 Getting Started 3-1

Mastering the Basics

Overview of the Next Four Chapters

The Mastering the Basics section contains a series of tutorial exercises designed to teach you basic SolidWorks concepts, as follows: q

Chapter 3. The 40 Minute Running Start - Create your first part.

Chapter 4. Assembly Basics - Add parts and build an assembly.

Chapter 5. Drawing Basics - Create a drawing of the parts and the assembly.

Chapter 6. Design Tables - Rename features and dimensions, and create variations of the part from Chapter 3, using a design table.

For consistency, you take the first part you create, then build your knowledge by using the same part throughout this section.

Starting SolidWorks 2001

Click the

Start

button on the Windows taskbar.

Click

Programs

SolidWorks 2001

The SolidWorks main window appears and the Welcome to SolidWorks 2001 screen opens.

NOTE:

If a dialog box appears reminding you to register your copy of SolidWorks 2001, click

Creating a New Part Document

To create a new part, click

New Document

on the Welcome to SolidWorks 2001 screen, click

New

on the Standard toolbar, or click

File

New

The

New SolidWorks Document

dialog box appears.

Click the

Tutorial

tab and select the

Part

icon.

Click

A new part window appears.

3-2

Chapter 3 The 40-Minute Running Start

Sketching the Rectangle

The first feature in the part is a box extruded from a sketched rectangular profile. You begin by sketching the rectangle.

To open a 2D sketch, click

Sketch

on the Sketch toolbar, or click

Insert

Sketch

A sketch opens on the

Front

plane.

Click

Rectangle

on the Sketch Tools toolbar, or click

Tools

Sketch Entity

Rectangle

Move the pointer to the sketch origin. You know the pointer is on the origin when the pointer changes to . Click the left mouse button and start moving the pointer to create a rectangle.

As you move the pointer, notice that it displays the dimensions of the rectangle. Click the mouse button to complete the rectangle.

For more information about inferencing pointers and lines, see the SolidWorks 2001 Online User’s Guide.

Click

Select

on the Sketch toolbar, or click

Tools

Select

The two sides of the rectangle that touch the origin are black. Because you began sketching at the origin, the vertex of these two sides is automatically related to the origin. (The vertex is not free to move.)

The other two sides (and three vertices) are blue. This indicates that they are free to move.

Click one of the blue sides, and drag the side or the drag handle at the vertex to resize the rectangle.

SolidWorks 2001 Getting Started 3-3

Mastering the Basics

Adding Dimensions

In this section you specify the size of the sketched rectangle by adding dimensions. The

SolidWorks software does not require that you dimension sketches before you use them to create features. However, for this example, you add dimensions now to fully define the sketch.

As you add dimensions to a sketch, the state of the sketch appears in the status bar. Any

SolidWorks sketch is in one of three states. Each state is indicated by a different color: q

In a fully defined sketch, the positions of all the entities are fully described by dimensions or relations, or both. In a fully defined sketch, all the entities are black.

In an under defined sketch, additional dimensions or relations are needed to completely specify the geometry. In this state, you can drag under defined sketch entities to modify the sketch. An under defined sketch entity is blue.

In an over defined sketch, an object has conflicting dimensions or relations, or both. An over defined sketch entity is red.

Click

Tools

Options

. On the

System Options

tab, click

General

, then click to clear the

Input dimension value

check box. Click

Click

Dimension

on the Sketch Relations toolbar, or click

Tools

Dimensions

Parallel

The pointer shape changes to .

Click the top edge of the rectangle, then click where you want to place the dimension.

The vertical line at the right changes from blue to black. By dimensioning the length of the top of the rectangle, you fully defined the position of the rightmost segment. You can still drag the top segment up and down.

Its blue color indicates that it is under defined.

Click the right edge of the rectangle, then click to place its dimension.

The top segment and the remaining vertices turn black. The status bar in the lower-right corner of the window indicates that the sketch is fully defined.

3-4

Chapter 3 The 40-Minute Running Start

Changing the Dimension Values

To change the dimensions, you use the

Dimensions

tool.

Double-click one of the dimensions.

The

Modify

dialog box appears. The current dimension is highlighted.

Type 120mm, then click .

The sketch changes size to reflect the new dimension. The dimension value is now 120mm.

Click

Zoom to Fit

on the View toolbar, or press the

key, or click

View

Modify

Zoom to Fit

, to display the entire rectangle at full size and to center it in the graphics area.

Double-click the other dimension and change its value to 120mm.

Click

Zoom to Fit

again to center the sketch.

SolidWorks 2001 Getting Started 3-5

Mastering the Basics

Extruding the Base Feature

The first feature in any part is called the base feature. You create this feature by extruding the sketched rectangle.

Click

Extruded Boss/Base

on the Features toolbar, or click

Insert

Base

Extrude

The

Base-Extrude

PropertyManager appears in the left panel, and the view of the sketch changes to isometric.

Under

Direction 1

, do the following:

• Set

End Condition

Blind

•

Set

Depth

to 30mm. To increment the value, either use the arrows or enter the value.

When you click the arrows, a preview of the result appears in the graphics area.

Sketch

Click

to create the extrusion.

The new feature,

Base-Extrude,

appears in the

FeatureManager design tree.

If you need to zoom to view the entire model, press

to zoom out, or press

Shift+Z

to zoom in.

Preview of the extrusion

Click the plus sign beside

Base-Extrude

in the FeatureManager design tree.

Sketch1

, which you used to extrude the feature, is now listed under the feature.

Click here

3-6

Chapter 3 The 40-Minute Running Start

Saving the Part

Click

Save

on the Standard toolbar, or click

File

Save

The

Save As

dialog box appears.

Type

Tutor1

and click

Save.

The extension

.sldprt

is added to the filename, and the file is saved to the current directory. To save the file to a different directory, use the Windows browse button to browse to that directory, then save the file.

NOTE:

File names are not case sensitive. That is, files named

TUTOR1.sldprt

Tutor1.sldprt

, and

tutor1.sldprt

are all the same part.

SolidWorks 2001 Getting Started 3-7

Mastering the Basics

Sketching a Boss

To create additional features on the part (such as bosses or cuts), you sketch on the model faces or planes, then extrude the sketches.

NOTE:

You sketch on one face or plane at a time, then create a feature based on one or more sketches.

Click

Hidden Lines Removed

on the View toolbar, or click

View

Display

Hidden Lines Removed

Click

Select

on the Sketch toolbar, if it is not already selected.

Move the pointer over the front face of the part.

The edges of the face become dotted lines to show that the face is available for selection.

The pointer changes to to show that you are selecting the face.

Click the front face of the part to select it.

The edges of the face become solid lines and change color to show that the face is selected.

Click

Sketch

on the Sketch toolbar, or right-click anywhere in the graphics area and select

Insert Sketch

A sketch opens.

Click

Circle

on the Sketch Tools toolbar, or click

Tools

Sketch Entity

Circle

Click near the center of the face and move the pointer to sketch a circle. Click again to complete the circle.

3-8

Chapter 3 The 40-Minute Running Start

Dimensioning and Extruding the Boss

To establish the location and size of the circle, add the necessary dimensions.

Click

Dimension

on the Sketch Relations toolbar, or right-click anywhere in the graphics area and select

Dimension

from the shortcut menu.

Click the top edge of the face, click the circle, then click a location for the dimension.

Notice the dimension preview as you click each entity. The preview shows you where the witness lines are attached, and that you have selected the correct entities for the dimension.

When you add a locating dimension to a circle, the witness line is attached to the centerpoint by default.

Click

Select

, double-click the dimension, then enter 60mm as the new value in the

Modify

dialog box.

Repeat the process to dimension the circle to the side edge of the face. Set this value to 60mm also.

Still using the

Dimension

tool , click the circle to dimension its diameter. Move the pointer around to see the preview for the dimension.

When the dimension is aligned horizontally or vertically, it appears as a linear dimension; if it is at an angle, it appears as a diameter dimension.

Click a location for the diameter dimension. Set the diameter to 70mm.

The circle turns black, and the status bar indicates that the sketch is fully defined.

Click

Extruded Boss/Base

on the Features toolbar, or click

Insert

Boss

Extrude.

The

Boss-Extrude

PropertyManager appears.

Under

Direction 1

, set the

Depth

of the extrusion to

25mm, leave the other items at the defaults, and click

to extrude the boss feature.

Boss-Extrude1

appears in the FeatureManager design tree.

SolidWorks 2001 Getting Started 3-9

Mastering the Basics

Creating the Cut

Next, create a cut concentric with the boss.

Sketching and dimensioning the cut

Click the front face of the circular boss to select it.

Click

Normal To

on the Standard Views toolbar.

The part is turned so that the selected model face is now facing you.

Click

Sketch

on the Sketch toolbar to open a new sketch.

Sketch a circle near the center of the boss as shown.

Click

Dimension

, and dimension the diameter of the circle to 50mm.

Adding a concentric relation

Now you add a concentric relation between the two circles.

Click

Add Relation

on the Sketch Relations toolbar, or click

Tools

Relations

Add

The

Add Geometric Relations

dialog box appears.

Select the sketched circle (the inner circle) and the edge of the boss (the outer circle).

Notice the contents of the

Selected entities

box. Only those relations that are appropriate for the selected entities are available. The most likely relation is automatically selected.

Make sure that

Concentric

is selected, click

Apply

, and click

Close

The inner and outer circles now have a concentric relation.

3-10

Chapter 3 The 40-Minute Running Start

Finishing the cut

Finally, you create the cut.

Click

Extruded Cut

on the Features toolbar, or click

Insert

Cut

Extrude

The

Cut-Extrude

PropertyManager appears.

Under

Direction 1

, set the

End Condition

Through All

, and click

Click

Isometric

on the Standard Views toolbar.

Click

Save

on the Standard toolbar to save the part

SolidWorks 2001 Getting Started 3-11

Mastering the Basics

Rounding the Corners of the Part

In this section you round the four corner edges of the part. Because the rounds all have the same radius (10mm), you can create them as a single feature.

Click

Hidden In Gray

. This makes it easier to select the hidden edges.

Click the first corner edge to select it.

Notice how the faces, edges, and vertices highlight as you move the pointer over them, identifying selectable objects. Also, notice the changing pointer shape:

Edge

Face

Vertex

Click

Rotate View

on the View toolbar, or click

View

Modify

Rotate

, and drag to rotate the part approximately as shown.

Click

Select

, then hold down the

Ctrl

key and click the four corner edges.

Select these four edges

Click

Fillet

on the Features toolbar, or click

Insert

Features

Fillet/Round

The

Fillet Feature

PropertyManager appears.

Four callouts appear that show the

Fillet Type

and

Radius

Under

Items to Fillet

, the

Edge fillet items

box shows the four selected edges.

Make sure the

Radius

the remaining items at the default values.

Click

The four selected corners are rounded. The

Fillet1

feature appears in the FeatureManager design tree.

3-12

Chapter 3 The 40-Minute Running Start

Adding More Fillets

Now add fillets and rounds to other sharp edges of the part. You can select faces and edges either before or after opening the

Fillet Feature

dialog box.

Click

Hidden Lines Removed

Click

Fillet

Click the front face of the base to select it.

Both the outside and inside edges (around the boss) are highlighted when you select the face.

The

Fillet Feature

PropertyManager appears.

The

Edge fillet items

list shows that one face is selected.

The callout indicates the

Fillet Type

and

Radius

Under

Items to Fillet

, change the

Radius

to 5mm, and click

The inside edge is filleted and the outside edge is rounded in a single step.

Click

Fillet

again.

Click the front face of the circular boss.

Change the

Radius

to 2mm, and click

Notice that the features listed in the FeatureManager design tree appear in the order in which you created them.

Click

Rotate View

and rotate the part to display different views.

Click

Save

to save the part

SolidWorks 2001 Getting Started 3-13

Mastering the Basics

Shelling the Part

Next, you shell the part. Shelling hollows out the part by removing material from the selected face, leaving a thin-walled part.

Click

Back

on the Standard Views toolbar.

The back of the part now faces towards you.

Click

Shell

on the Features toolbar, or click

Insert

Features

Shell

The

Shell1

PropertyManager appears.

Click the back face to select it.

The selected face appears under

Parameters

in the

Faces to Remove

list.

Under

Parameters

, set the

Thickness

to 2mm and click

OK .

The shell operation removes the selected face.

To see the results, click

Rotate View

and rotate the part.

You may need to drag parts to different areas of a window.

Click

Pan

on the View toolbar, or click

View

Modify

Pan

, then click the part, drag it to a new location, and release the mouse button.

Click

Pan

again to turn off the

Pan

tool.

3-14

Chapter 3 The 40-Minute Running Start

Changing a Dimension Using Feature Handles

This section illustrates a way to change the dimension of an extruded feature using feature handles.

Click

Rotate View

on the View toolbar and drag to rotate the part approximately as shown. Click

Rotate View

again to turn it off.

Double-click

Base-Extrude

in the FeatureManager design tree.

The

Base-Extrude

feature expands to show the sketch it was based on.

The feature dimensions appear in the graphics area.

Click

Move/size features

on the Features toolbar.

The feature handles for the extruded feature appear. Feature handles allow you to move, rotate, and resize some types of features.

Drag the

Resize

handle to increase the depth of the extrusion from 30mm to

50mm.

Rotate

Resize

(depth)

Watch the pointer for feedback about the dimension you are changing. When you release the pointer, the part rebuilds using the new dimension.

Click

Move/size features

to turn off the features handle display.

Click anywhere outside the part in the graphics area to hide the dimensions.

Click

Save

to save the part.

Move

For more information about feature handles, see the

SolidWorks 2001 Online User’s Guide.

NOTE:

You can also change a dimension using the

Modify

dialog box method as

discussed earlier (see page 3-5).

SolidWorks 2001 Getting Started 3-15

Mastering the Basics

Displaying a Section View

You can display a 3D section view of the model at any time. You use model faces or planes to specify the section cutting planes. In this example, you use the

Right

plane to cut the model view.

Click

Isometric

, then click

Shaded

view mode.

Click

Right

in the FeatureManager design tree.

The

Right

plane becomes highlighted.

Click

Section View

on the View toolbar, or click

View

Display

Section View

The

Section View

dialog box appears.

Select the

Preview

check box.

A section cut arrow appears.

NOTE:

When you select the

Preview

option, the view updates each time you change a value in the dialog box.

If a message appears about the model not being properly sectioned, click

Click the up arrow in the

Section Position

box to set the

Section Position

to 60mm.

A section cut plane appears. The view dynamically updates as you increment the value, which is the offset distance from the

Right

plane to the section cut plane.

The section cut arrow indicates the area of the model that will be visible, starting from the section cut plane and going in the direction of the arrow.

TIP:

Switch to

Top

Front

Section View

tool works.

Select the

Flip the Side to View

check box to flip the direction of the section cut arrow.

Click

The section view of the part is displayed. Only the display of the part is cut, not the model itself. The section display is maintained if you change the view mode, orientation, or zoom.

Click to clear

Section View

You return to a complete display of the part.

3-16

Assembly Basics

In this chapter, you build a simple assembly. This chapter discusses the following: q

Adding parts to an assembly q

Moving and rotating components in an assembly q

Specifying the assembly mating relations that make the parts fit together

SolidWorks 2001 Getting Started 4-1

Mastering the Basics

Assembly Overview

An assembly is a combination of two or more parts, also called components, within one

SolidWorks document. You position and orient components using mates. Mates form relations between faces and edges of components.

In this chapter, you create a new base part and mate it to the part you created in the

40-Minute Running Start chapter, to create an assembly.

For more information about assemblies, see the SolidWorks 2001 Online User’s Guide.

Creating the Base Feature

You can use the same methods you learned in Chapter 3 to create the base for a new part.

Open a new part from the

Tutorial

tab.

Click

Sketch

, and sketch a rectangle beginning at the origin.

Click

Dimension

, and dimension the rectangle to 120mm x

120mm.

Click

Extruded Boss/Base

, and extrude the rectangle , with an

End Condition

Blind,

to a

Depth

of 90mm.

Click

Fillet

, and fillet the four edges shown with a radius of

10mm.

Click

Shell

. Select the front face of the model as the face to remove, and set the

Thickness

to 4mm.

Save the part as

Tutor2

. (The

.sldprt

extension is added to the file name.)

4-2

Chapter 4 Assembly Basics

Creating a Lip on the Part

In this section, you use the

Convert Entities

and

Offset Entities

tools to create sketch geometry. Then a cut creates a lip to mate with the part from the previous chapter.

TIP:

Use the

Selection Filter

to make selecting the faces in this section

easier. See "Selection Filter" in "More about Basic Functionality" for

more information.

Click

Zoom to Area

, or click

View

Modify

Zoom to

Area

, and zoom in on a corner of the part, as shown. Click

Zoom to Area

again to turn off the tool.

Select the thin wall on the front face of the part, and click

Sketch

to open a sketch.

The edges of the part face are highlighted.

Click

Convert Entities

on the Sketch Tools toolbar, or click

Tools

Sketch Tools

Convert Entities

The outer edges of the selected face are projected (copied) onto the sketch plane as lines and arcs.

Click the front face again.

Click

Offset Entities

on the Sketch Tools toolbar, or click

Tools

Sketch Tools

Offset Entities

Set the

Offset Distance

to 2mm.

The preview shows the offset extending outward.

Select the

Reverse

check box to change the offset direction.

Click

A set of lines is added in the sketch, offset from the outside edge of the selected face by 2mm. This relation is maintained if the original edges change.

Click

Extruded Cut

, or click

Insert

Cut

Extrude

Under

Direction 1

, set the

Depth

to 30mm, and click

OK .

The material between the two lines is cut, creating the lip.

SolidWorks 2001 Getting Started 4-3

Mastering the Basics

Changing the Color of a Part

You can change the color and appearance of a part or its features.

Click the

Tutor2

icon at the top of the FeatureManager design tree.

Click

Shaded

Click

Edit Color

on the Standard toolbar.

The

Edit Color

dialog box appears.

Click the desired color on the palette, then click

Save the part.

Creating the Assembly

Now create an assembly using the two parts.

Tutor1.sldprt

is not open, click

Open

on the Standard toolbar and open it.

Open a new assembly from the

Tutorial

tab.

Click

Window, Tile Horizontally

to display all three windows. Close any extra windows.

Drag the

Tutor1

icon from the top of the FeatureManager design tree for

Tutor1.sldprt

, and drop it in the FeatureManager design tree of the assembly window (

Assem1

Notice that as you move the pointer into the FeatureManager design tree, the pointer changes to .

Adding a part to an assembly this way results in the part automatically inferencing the assembly origin. When a part inferences the assembly origin:

• the part’s origin is coincident with the assembly origin.

• the planes of the part and the assembly are aligned.

4-4

Chapter 4 Assembly Basics

Drag the

Tutor2

icon from

Tutor2.sldprt,

and drop it in the graphics area of the assembly window, beside the

Tutor1

part.

Notice that as you move the pointer into the graphics area, the pointer changes to .

Save the assembly as

Tutor.

(The

.sldasm

extension is added to the file name.) If you see a message about saving referenced documents, click

Yes

Drag a corner of the assembly window to enlarge it, or click

Maximize

the upper-right corner to make the window full size. You no longer need to have the

Tutor1.sldprt

and

Tutor2.sldprt

windows in view.

Click

Zoom to Fit

SolidWorks 2001 Getting Started 4-5

Mastering the Basics

Mating the Components

In this section, you define assembly mating relations between the components, making them align and fit together.

Click

Isometric

on the Standard Views toolbar.

Click

Mate

on the Assembly toolbar, or click

Insert

Mate

Click the top edge of

Tutor1

, then click the outside edge of the lip on the top of

Tutor2

The edges appear in the

Selections

list.

Select these edges

Under

Selections

, do the following:

•

Click

Coincident

as the mate type.

• Click

Closest

as the

Mate Alignment

Click

Preview

to preview the mate.

The selected edges of the two components are made coincident.

Click

Tutor1 Tutor2

The position of the

Tutor2

component in the assembly is not fully defined, as shown by the

(-)

prefix in the FeatureManager design tree.

Tutor2

still has some degrees of freedom to move in directions that are not yet constrained by mating relations.

Click

Move Component

Click the

Tutor2

component and hold down the left mouse button.

Notice the pointer shape

Drag the component from side to side to observe the available degrees of freedom, then release the left mouse button.

Click

Move Component

again to exit move mode.

4-6

Chapter 4 Assembly Basics

Adding More Mates

Select the rightmost face of one component, then hold down

Ctrl,

and select the corresponding face on the other component.

Click

Mate

Select

Coincident

and

Closest

Click

Preview

to preview the mate.

Click

Repeat Steps 1 through 5, selecting the top

faces of both components, to add another

Coincident

mate.

Select these faces

Save the assembly.

SolidWorks 2001 Getting Started 4-7

Drawing Basics

In this chapter, you create a multi-sheet drawing of the parts and assembly from the previous chapters. This chapter includes: q

Opening a drawing template and editing a sheet format q

Inserting standard views of a part model q

Adding model and reference annotations q

Adding another drawing sheet q

Inserting a named view q

Printing the drawing

SolidWorks 2001 Getting Started 5-1

Mastering the Basics

Opening a Drawing Template

First you open a drawing template.

Click

New

on the Standard toolbar.

The

New SolidWorks Document

dialog box appears.

Select the

Tutorial

tab, click the

Drawing

icon, then click

A new drawing window appears, with note text.

Preparing the Drawing Template Format

Next you prepare the drawing sheet format by changing some text properties.

Right-click anywhere in the drawing, and select

Edit Sheet Format

Click

Zoom to Area

, zoom in on the title block at the lower right, then click again to turn off

Zoom to Area

Right-click the note with the text

<COMPANY NAME>

and select

Properties

The

Properties

dialog box appears.

Change the

Note text

to the name of your company.

Click

Font

The

Choose Font

dialog box appears.

Choose a different font, style, or size, then click

Click

to close the

Properties

dialog box.

Right-click in the graphics area, and select

Edit Sheet

to exit the edit sheet format mode.

Next you save the updated drawing sheet format.

To replace this format as the standard

Format.

A-Landscape

format, click

File, Save Sheet

The

Save Sheet Format

dialog box appears.

Click

OK.

5-2

Chapter 5 Drawing Basics

Click

Yes

to confirm that you want to overwrite the existing sheet format. When you choose this format for your own drawings, you will not need to perform these edits again.

NOTE:

To save the sheet format with a new name and to not overwrite the standard sheet format, click

File, Save Sheet Format, Custom Sheet Format

. Click

Browse

and navigate to the directory where you want to save the format.

Type a name and click

Save

. Click

to close the dialog box.

Setting the Detailing Options

Next, set the default dimension font, and the style of dimensions, arrows, and other detailing options. For this chapter, use the settings described below. Later, you can set the

Detailing

options to match your company’s standards.

Click

Tools

Options

On the

Document Properties

tab, click

Detailing

. In the

Dimensioning Standard

section, in the

Trailing Zeroes

box, select

Remove

Under

Detailing,

click

Dimensions

. Click Font.

The

Choose Font

dialog box appears.

In the

Height

box, click

Points

, and type or select 16.

Click

Under

Detailing,

click

Arrows

, and review the default styles and sizes.

Notice the different attachment styles for edges, faces, and unattached items.

Click

to close the

Options

dialog box.

For more information about these options, see the SolidWorks 2001 Online User’s Guide.

SolidWorks 2001 Getting Started 5-3

Mastering the Basics

Creating a Drawing of a Part

Open

Tutor1.sldprt

if it is not open. Then return to the drawing window.

Click

Standard 3 View

on the

Drawing toolbar, or click

Insert

Drawing

View

Standard 3 View

Drawing View2 Drawing View3

Notice the pointer .

The

Standard View

Property Manager displays a message explaining four methods to select a model.

From the

Window

menu, select

Tutor1.sldprt

The

Tutor1.sldprt

window appears.

Click in the graphics area of the part window. The drawing window reappears with the three views of the selected part.

Drawing View1

TIP:

Another method of creating a Standard 3 View is to tile the windows, and drag the part from the part document to the graphics area of the drawing.

Moving Drawing Views

To move a view, click inside its boundary.

When the pointer is at the border, it changes to , and you can drag the view in its allowed directions.

Click

Drawing View2

, then drag it up and down.

Click

Drawing View3

, then drag it left and right.

Drawing View2

and

Drawing View3

are aligned to

Drawing View1,

and only move in one direction to preserve the alignment.

Click

Drawing View1

and drag it in any direction to move all the views at the same time.

Move the views on the drawing sheet to the approximate positions shown.

5-4

Chapter 5 Drawing Basics

Adding Dimensions to a Drawing

Drawings contain 2D views of models. You can choose to display dimensions specified in the model in all of the drawing views.

With nothing selected, click

Insert

Model Items

The

Insert Model Items

dialog box appears. You can select which types of dimensions, annotations, and reference geometry to import from the model.

Make sure that

Dimensions

and

Import items into all views

are selected, and click

Dimensions are imported into the view where the feature they describe is most visible.

Only one copy of each dimension is imported because the

Eliminate duplicate model dimensions

check box is selected.

Drag the dimensions to position them.

TIP:

Select a drawing view, then click

Zoom To Selection

zoom the view to fill the screen. Click

Zoom to Fit

to see the entire drawing sheet.

Click

Save

, and save the drawing document as

Tutor1

The default extension is

.slddrw

SolidWorks 2001 Getting Started 5-5

Mastering the Basics

Modifying Dimensions

When you change a model dimension in the drawing view, the model is automatically updated to reflect the change, and vice versa.

Drawing View2

, double-click the dimension for the depth of the boss extrusion.

The

Modify

dialog box appears.

Change the value from 25mm to

40mm, and press

Enter

Click

Rebuild

on the Standard toolbar, or click

Edit

Rebuild

The part rebuilds using the modified dimension. Both the drawing and the part model are updated.

Click

Window

, and select the

Tutor1.sldprt

window.

Double-click

Boss-Extrude1

in the

FeatureManager design tree to display the dimensions of the feature.

Double-click this dimension

Notice that the depth dimension is 40mm.

Return to the drawing window, and save the drawing.

The system notifies you that the model referenced in the drawing has been modified, and asks if you want to save it.

Click

Yes

to save both the drawing and the updated model.

Now rebuild the assembly that contains the modified part.

Open

Tutor.sldasm

if it is not still open.

If a message appears asking you if you want to rebuild the assembly, click

Yes

The assembly rebuilds with the new dimensions.

Return to the drawing window.

5-6

Chapter 5 Drawing Basics

Adding Another Drawing Sheet

Now you create an additional drawing sheet for the assembly. You then use the

Insert

From File

command to insert an assembly document into the drawing.

Click

Insert, Sheet

The

Sheet Setup

dialog box appears.

Under both

Paper size

and

Sheet Format

, select

B-Landscape

, and click

Sheet2 opens and is added to the drawing document.

Click

Standard 3 View

, right-click in the graphics area, and select

Insert From

File

The

Insert Component

dialog box appears.

Set

Files of type

Assembly Files (*.asm, *.sldasm)

, navigate to

Tutor.sldasm

, and click

Open

The Standard 3 Views of the assembly appear on the drawing sheet.

Reposition the views on the sheet if needed.

SolidWorks 2001 Getting Started 5-7

Mastering the Basics

Inserting a Named View

You can add named views to drawings, showing the model in different orientations. You can use:

•

A standard view (

Front

Top

Isometric

, and so on)

•

A named view orientation that you defined in the part or assembly

•

The current view in the part or assembly document

Zoom levels are ignored, however, and the entire model is always displayed in the selected orientation.

In this section you add an isometric view of the assembly.

Click

Named View

, or click

Insert

Drawing View

Named View

The

Named View

PropertyManager appears.

The pointer indicates that you may select a model to display in the drawing.

Right-click in the graphics area, and select Insert From File.

The

Insert Component

dialog box appears.

Navigate to

Tutor.sldasm

, and click

Open

The

Named View

PropertyManager appears. Note its similarity to the

Orientation

dialog box.

The pointer indicates that you may select a location in the drawing to place the named view.

Click where you want to place the view.

Double-click

*Isometric

from the list to switch to an isometric view.

5-8

Chapter 5 Drawing Basics

Printing the Drawing

Click

File, Print

The

Print

dialog box appears.

Set

Print range

All

, and make sure that the

Scale to fit

check box is selected.

Click

to close the

Print

dialog box and print the drawing.

Click

Save

The system notifies you that the model referenced in the drawing has been modified, and asks if you want to save it.

Click

Yes

, then close the drawing.

SolidWorks 2001 Getting Started 5-9

Design Tables

In this chapter you use a design table to create several variations of the part you designed

in Chapter 3, “The 40-Minute Running Start.” To use a design table, you must have

Microsoft Excel on your computer. For more information, see Chapter 1, “Installation.”

This exercise demonstrates the following: q

Renaming features and dimensions q

Displaying feature dimensions q

Linking values of model dimensions q

Verifying geometric relations q

Creating a design table q

Displaying part configurations

SolidWorks 2001 Getting Started 6-1

Mastering the Basics

Renaming Features

It is a good practice to give meaningful names to the features in your parts, especially when you plan to use a design table. This can save confusion in complex parts, and it is helpful to other people who use the parts later.

Open

Tutor1.sldprt

that you created in Chapter 3.

Change the generic name

Base-Extrude

to something more meaningful.

NOTE:

Feature names cannot contain the @ character.

4 a) b)

Click-pause-click on

Base-Extrude

in the FeatureManager design tree (do not double-click).

Type the new name,

Box

, and press

Enter

Rename these other features:

•

Boss-Extrude1 => Knob

•

Cut-Extrude1 => Hole_in_knob

•

Fillet1 => Outside_corners

Save the part as

Tutor3.sldprt

TIP:

To give descriptive names to features as you create them, click

Tools,

Options

. On the

System Options

tab, click

FeatureManager

, then select the

Name feature on creation

check box. Each time you create a new feature, the name of the new feature in the FeatureManager design tree is automatically highlighted, and ready for you to type a new name.

Displaying Dimensions

You can display or hide all the dimensions for all the features of the part. Then you can turn the display of dimensions on and off, either individually, or on a feature-by-feature basis.

Right-click the

Annotations

folder in the FeatureManager design tree, and select

Show Feature Dimensions

All the dimensions for the part appear. Notice that the dimensions that are part of a feature’s definition (such as the depth of an extruded feature) are blue.

Right-click the

Fillet2

Fillet3

, and

Shell1

features in the FeatureManager design tree or in the graphics area, and select

Hide All Dimensions

All the dimensions for these features are hidden.

6-2

Chapter 6 Design Tables

Right-click one of the dimensions set to

60,

and select

Hide

This individual dimension is hidden. It belongs to the

Knob

feature.

NOTE:

To restore hidden dimensions, right-click the feature in the

FeatureManager design tree whose dimensions are either partially or completely hidden, and select

Show All Dimensions

Click

Tools, Options

. On the

System Options

tab, click

General

, then select the

Show dimension names

check box, and click

The dimension names appear below the values in the model.

Dimension names appear with default names. You can rename dimensions, similar to renaming features. You will rename dimensions later in this chapter.

Linking Values

Linking values is a way to control values that are not part of a sketch, such as the depth of two extruded features.

You link dimensions by assigning them the same variable name. Then you can modify the value of any of the linked dimensions, and all of the other dimensions with the same variable name change accordingly.

You can unlink any of the dimensions without affecting the ones that you want to remain linked.

For this example, you set the extrusion depth of the

Box

and the

Knob

to be equal:

Right-click the dimension for the extruded depth (50mm) of the

Box

, and select

Link

Values

The

Shared Values

dialog box appears.

Type

depth

in the

Name

box, and click

Right-click the dimension for the depth (40mm) of the

Knob

, and select

Link Values

Click the arrow beside the

Name

box, select

depth

from the list, and click

. (Each time you define a new

Name

variable, it is added to this list.)

Notice that the two dimensions now have the same name,

depth

. They use the dimension value of the first dimension you clicked (50mm).

Click

Rebuild

to rebuild the part.

The

Knob

changes to 50mm depth.

SolidWorks 2001 Getting Started 6-3

Mastering the Basics

Renaming Dimensions

You can change individual dimension names. Renaming dimensions is a good practice, and it is especially useful when you plan to use a design table. You use the dimension names to identify the elements you plan to change, and as headings in the design table worksheet.

Change the name of the knob diameter dimension:

a) b) c)

Right-click the

(70mm), and select

Properties

The

Dimension Properties

dialog box appears.

Select the text in the

Name

box and type in a new name,

knob_dia

Notice that the

Full name

box is updated as you type.

Click

Knob

diameter dimension

Rename the height of the box (120mm) to

box_height

Rename the width of the box (120mm) to

box_width

Rename the diameter of the hole in the knob (50mm) to

hole_dia

Rename the radius of the outside corners (10mm) to

fillet_radius

Save the part.

6-4

Chapter 6 Design Tables

Verifying Relations

Before you proceed, you should define some geometric relations that ensure that the knob is positioned correctly with respect to the center of the box, regardless of the size.

Relations add to the integrity of the design, and they are often the most effective way to convey the design intent accurately.

In the FeatureManager design tree or the model, right-click the

Knob

feature, and select

Edit Sketch

Click

Hidden Lines Removed

, and click

Normal To

The front of the model now faces towards you.

Delete the dimensions (60mm) between the circle and the sides of the box.

Click the centerpoint of the circle, and drag the circle to one side.

Click

Centerline

, or click

Tools

Sketch

Entity

Centerline

, and sketch a diagonal centerline as shown. Press

Esc

to exit the

Centerline

tool.

Add a relation between the midpoint of the centerline and the centerpoint of the circle:

Click

Add Relation

Relations

Add

, or click

Tools

b) c)

The

Add Geometric Relations

dialog box appears.

Click the centerpoint of the circle and the centerline.

Click

Midpoint

, and click

Apply.

The circle turns black, indicating the sketch is now fully defined.

Click

Close

Now verify the relations in this sketch:

Click

Display/Delete Relations

click

Tools

Relations

Display/Delete

Relations

, or

The

Display/Delete Relations

dialog box appears.

Click

Next

Previous

the relations in the sketch.

to review all

SolidWorks 2001 Getting Started 6-5

Mastering the Basics

As you display each relation, the entities are highlighted in the graphics area.

NOTE:

If a sketch entity is selected when you click

Display/Delete Relations

, only the relations on the selected entity are listed. Click a different entity to display its relations. You can change the

Criteria

in the

Display relations by

box to specify the types of relations (

All, Dangling

, and so on) that are displayed.

Click the

Entities

tab for more information about the highlighted entities.

Click

Close

to close the

Display/Delete Relations

dialog box.

Click

Sketch

to close the sketch.

Save the part.

6-6

Chapter 6 Design Tables

Inserting a New Design Table

If you have Microsoft Excel on your computer, you can use it to embed a new design table directly in the part document. A design table allows you to build several different

configurations of a part by applying the values in the table to the dimensions of the part.

First you should prepare to insert the design table.

Click

Tools, Options

. On the

System Options

tab, click

General

Make sure that the

Edit design tables in a separate window

check box is not selected, and click

Click

Isometric

Press

to zoom out or

Shift+Z

to zoom in and resize the part so you can see all of the part’s dimensions in the graphics area. Use the

Pan

tool , if necessary, to move the part to the lower right corner of the window.

Click

Select

to deselect any active View tool.

Now you are ready to insert a new design table.

NOTE:

If you accidentally click outside the worksheet before entering all the values, click

Edit

Design Table

to redisplay the design table.

Click

Insert, New Design Table

An Excel worksheet appears in the part document window. Excel toolbars replace the

SolidWorks toolbars. By default, the first row (cell A3) is named

First Instance

, and column header cell B2 is active.

Double-click the

box_width

dimension value (120) in the graphics area.

Notice that the pointer changes to when it is over a dimension value.

The dimension name and value are inserted in cell B3

The adjacent column header cell, C2, is activated automatically.

TIP:

To uncover dimensions hidden by the design table, point at the Excel worksheet’s outer dashed border and drag the worksheet to another location in the graphics area. To resize the worksheet, drag the handles at the corners or sides.

SolidWorks 2001 Getting Started 6-7

Mastering the Basics

Double-click each dimension value in the graphics area to insert the rest of the dimension names and values, as shown in the illustrations in steps 4 and 5. Do not include depth@Box (50mm).

NOTE:

If you see

$STATE@

followed by a feature name in a column header cell, you selected a face instead of a dimension value in the graphics area. To replace a feature name with a dimension name, click the cell in the worksheet, then double-click the correct dimension value in the graphics area.

Name the rows (cells A4:A6)

blk2

through

blk4

. These are the names of the configurations that the design table produces.

Type the following dimension values into the worksheet:

Click anywhere outside the worksheet in the graphics area.

The worksheet closes. An informational dialog box appears, listing the new configurations that the design table created.

Click

to close the dialog box.

The design table is embedded and saved in the part document.

Save the part.

If a message appears asking if you want to rebuild the part, click

Yes

6-8

Chapter 6 Design Tables

Viewing the Configurations

Now look at each of the configurations generated by the table.

Click

Shaded

Click the ConfigurationManager tab at the bottom of the FeatureManager design tree.

The list of configurations appears.

Double-click the name of a configuration.

As you display each of the configurations, the part rebuilds using the dimensions for the selected configuration.

SolidWorks 2001 Getting Started 6-9

Mastering the Basics

Editing the Design Table

To make changes to the design table:

Click

Edit, Design Table

Make the desired changes.

To close the design table, click anywhere in the graphics area outside the design table.

The configurations update as needed to reflect the changes.

TIP:

When using this or any other OLE object, you may need to click

Zoom to Fit

when returning to the SolidWorks window.

Deleting the Design Table

To delete the design table, click

Edit, Delete Design Table

. Deleting a design table does

not delete the configurations associated with it.

6-10

More about Basic Functionality

The Mastering the Basics chapters introduce you to many functions available with

SolidWorks 2001. The following pages highlight some additional SolidWorks functionality. For more information, see the SolidWorks 2001 Online User’s Guide.

Accessing SolidWorks Documents Using Windows Explorer

Windows Explorer offers you the following functionality: q

Thumbnail images. View thumbnail images of SolidWorks parts and assemblies. The graphic is based on the view orientation of the model when the document was saved. q

Opening documents. Open a part, drawing, or assembly document.

Drag and drop. You can drag and drop:

•

Any SolidWorks document from Windows Explorer into an empty area of the

SolidWorks window, not occupied by another document window.

•

A part or assembly from Windows Explorer to an open SolidWorks assembly window to add an instance of the part or sub-assembly to the assembly.

•

A part or assembly from Windows Explorer to an open and empty SolidWorks drawing document to create the standard three views.

Accessing SolidWorks Documents Using Internet Explorer

Internet Explorer version 4.0 or later offers you drag and drop functionality.

You can drag and drop hyperlinks that jump to SolidWorks part files from the Internet

Explorer window to:

•

The Feature Palette™ window

•

A new, empty part document

•

A drawing or assembly document

•

An empty area of a SolidWorks window

More about Basic Functionality

Setting Up Different Views of SolidWorks Documents

There are several ways you can view SolidWorks documents.

Multiple Views of Different Documents. You can have multiple part, assembly, and drawing document windows open at the same time.

Part Sub-assembly

Assembly

Multiple Views of the Same Document. You can open additional views of the same document. Selecting an item in one view selects it in all views. For example, when creating a fillet you could select edges on the front of the model in one view and edges on the back in another view.

Split Window View. You can use split controls to split the window into two or four panes. You can zoom, rotate, and set the view mode for each of these views independently.

Window size control

SolidWorks 2001 Getting Started

Horizontal Split control

Vertical

Split control

More about Basic Functionality

Orientation Dialog Box

. You can use the

Orientation

dialog box to:

• Create your own named views.

• Switch to any of the standard views, or to two additional views,

*Trimetric

and

*Dimetric

• Change the orientation of all the standard views.

• Restore all of the standard views to their default settings.

Duplicate Panel Display

You can display a split instance of the panel adjacent to the graphics area, usually the

FeatureManager design tree. A split display is not limited to duplicate FeatureManager design trees. You can select any combination of the following: q

FeatureManager design tree q

PropertyManager q

ConfigurationManager q

Third party applications that use the panel

This option is available either alone or in conjunction with

Window

New Window

Without opening a new window, you can display the same part, assembly or drawing, along with any combination of the panels. With complex designs, for example, you can: q

Display different sections of the part, drawing, or assembly, expanded or collapsed q

View different details for configurations q

Pick different selections from each panel

FeatureManager Design Tree

The FeatureManager design tree and the graphics display window are dynamically linked.

You can select features, sketches, drawing views, and construction geometry in either pane.

FeatureManager design tree

Rollback bar

Tabs Graphics area

The FeatureManager design tree offers you the following functionality: q

Feature order. Change the order in which features are rebuilt.

Feature names. Change feature names.

Moving and copying features. You can move features by dragging them in the model.

For example, you can move a hole to a different face. You can also copy or move a fixed-radius fillet or a chamfer using drag-and-drop. q

Dragging and dropping between open documents. You can drag a part or assembly name from the FeatureManager design tree to a drawing document. q

Suppress/Unsuppress. Suppress or unsuppress selected features.

Dimensions. Display and control the dimensions of a feature.

Annotations. Filter, scale, and control the display of annotations using the

Annotations

folder.

Lighting. Adjust the kind and amount of lighting that illuminates a shaded part or assembly using the

Lighting

folder. q

Rollback bar. Temporarily roll the model or assembly back to an earlier state using the

rollback bar.

Equations. Add a new equation, edit, or delete an equation using the

Equations

folder.

SolidWorks 2001 Getting Started

More about Basic Functionality

Tabs. Use the tabs at the bottom of the FeatureManager design tree to show you the current FeatureManager function.

A part or a sketch document is open for editing and viewing.

An assembly is open for editing, adding components, creating configurations, and viewing.

A drawing document is open for viewing or editing.

The PropertyManager functionality is in use.

The ConfigurationManager tab is in use, where you create, select, and view the configurations of a part or assembly. q

Symbols. View symbols to get information about:

• Any parts or features with external references. An external reference is a dependency on geometry that exists in another document.

• The state of sketches (over defined, under defined, not solved).

• The state of assemblies and assembly mates.

Rebuild Icon. The rebuild icon appears when you are required to rebuild a part.

Customizing Toolbars

You can customize your toolbar display.

Displaying toolbars. Some toolbars are always displayed; other toolbars display automatically when you open a document of the related type. For example, when you open an assembly document, the Assembly toolbar appears.

Moving toolbar buttons. You can move toolbar buttons to different toolbars, change menus, or reset shortcut keys.

Rearranging toolbars. You can rearrange toolbars in the SolidWorks window. You can dock them at the edge of the window, or make them floating palettes.

Customizing SolidWorks Functionality Using the Options Dialog Box

The SolidWorks 2001 application lets you customize functionality to suit your needs.

System Options

tab. Set options, such as system colors and spin box increments, that are stored in the registry and affect all current and future documents. q

Document Properties

tab. Set options, such as grid/snap and units, that apply only to the current document. This tab is available only when you have a document open.

Document Templates

Templates are documents (parts, drawings, and assemblies) that include user-defined parameters. Templates allow you to maintain as many different documents for parts, drawings or assemblies as you need. A template can be a blank document, or it can be a part, drawing, or assembly that you saved as a template. For example, you can create: q

A document template using millimeters and another template using inches q

A document template using ANSI and another template using ISO dimensioning standard q

A base part in a document that you use for mold design

When you open a new part, drawing, or assembly, the

New SolidWorks Document

dialog box appears. The dialog box has tabs for you to organize templates, shows you a preview of templates, and allows you to configure the display of templates for any of the tabs. You can also create additional tabs.

SolidWorks 2001 Getting Started

More about Basic Functionality

Keyboard Shortcuts

Keyboard shortcut keys are available for many menu items. Look for the underlined letters in the main menu bar.

Also, look for the underlined letter for each of the menu items. When the menu is pulled down, pressing an underlined letter activates the related command.

Some commands also have shortcut keys that are displayed on the menu beside the command. For example, the combination

Ctrl + N

opens a new file.

You can customize the keyboard shortcut keys to suit your style of working.

The following table lists the default keyboard shortcuts for rotating and viewing your model

Action

Rotate the model:

Key Combination

• horizontally or vertically

• horizontally or vertically 90 degrees

• clockwise/counterclockwise

Scroll the model

Orientation dialog box

Zoom in

Arrow

keys

Shift + Arrow

keys

Alt +

left or right

Ctrl + Arrow

keys

Spacebar

Shift + Z

Zoom out

Zoom to fit

Rebuild the model

Ctrl + B

Force rebuild the model and all its features

Ctrl + Q

Arrow

keys

Redraw the screen

Ctrl + R

Shortcut Menus

Whether you are working with a sketch, a part, an assembly, or a drawing, you have access to a wide variety of tools and commands from the shortcut menu accessed by pressing the right-mouse button.

As you move the pointer over geometry in the model or over items in the FeatureManager design tree, right-clicking pops up a shortcut menu of commands that are appropriate for whatever you clicked on.

For example, with the shortcut menu, you can: q

Select a sketch tool.

Open and close sketches.

Change or view the properties of an item.

Give a new name to a feature or dimension using the

Properties

dialog.

Hide

Show

a sketch, plane, axis, or assembly component.

Open an assembly component for editing. q

Access the dimension tools and an annotations menu when in a drawing.

Find an item in the FeatureManager design tree.

ConfigurationManager Shortcut Menu Options

When you hold down the right mouse button in a blank area with the

ConfigurationManager active, you can: q

Open the

Add Configuration

dialog box.

Open the

Document Properties

tab from the

Options

dialog box directly.

Additional Shortcut Menu Options

You have additional shortcut menu functions, if you prefer using the right mouse button rather than the menu bar. These added functions appear where appropriate. They include: q

Delete

- delete a feature or portion of sketch q

Suppress/Unsuppress

- suppress or unsuppress a feature or a component q

Edit Equation

- edit an equation when you select the driven dimension in the sketch q

Delete

- delete a Bill of Materials (BOM) in a drawing q

Open

- open a part file or a top-level assembly over drawings q

Mate

- mate components in an assembly q

Move Component

- move a component in an assembly

SolidWorks 2001 Getting Started

More about Basic Functionality

Middle Mouse Button Functions

With a three-button mouse, you can dynamically use the following view commands: q

Pan all document types - Click the middle mouse button and hold down

Ctrl

Rotate part or assembly - Click the middle mouse button.

Zoom all document types - Click the middle mouse button and hold down

Shift

NOTE:

In an active drawing, to pan you can use the middle mouse button with or without holding down

Ctrl

If you use a three button mouse, you may need to install the appropriate software or configure the device through Windows

Program Manager. Consult the documentation included with your mouse.

Working with Dimensions

The following dimensioning tips may save you some time.

Using the

Modify

box as a calculator. You can type values and arithmetic symbols directly into the box to calculate the dimension.

NOTE:

You do not have to type the units, such as mm or in. q

Editing dimension positions. You can:

• Hide a dimension.

• Move or copy a dimension to another view in a drawing.

• Center the dimension text between the witness lines.

Editing circular feature dimensions. You can:

•

Change a radius dimension to a diameter dimension.

• Display a diameter dimension as a linear dimension.

Display As Radius

(default)

Display As Diameter Display As Linear

Handle q

Modifying leaders, text, and arrows. You can modify the appearance of leaders, text, and arrows.

Preparing to Print Using Page Setup

Use

File

Page Setup

to set the margins and page orientation that works best with your printer or plotter. This setting applies for all SolidWorks documents that you print, until you change the setup. You can specify the following print options: q

Paper margins

Line weights

Page orientation

Scale - Drawings

and

Parts/Assemblies

Print drawings in color

You can also use

Page Setup

to create custom headers and footers for individual documents before printing. Options include: q

Select a predefined header or footer q

View your selection in the

Preview

boxes q

Select

Custom Header

Custom Footer

Select a

Font

style and size for customcreated headers and footers q

Include the following in a header or footer:

•

Page Number

•

Number of Pages

•

Date

•

Time

•

Filename

View changes before printing the document

Page

Number

Number of

Pages

Date

Time

Filename

SolidWorks 2001 Getting Started

More about Basic Functionality

What’s Wrong?

The SolidWorks application offers a “What’s Wrong” functionality. With this function, you can view information about any errors that occur when rebuilding a part or assembly.

A red circle with a down-pointing arrow next to the part or assembly name at the top of the FeatureManager design tree alerts you that there is a problem. An exclamation mark (

) indicates the item responsible for the error.

Some common errors in rebuilding include: q

Dangling dimensions or relations – dimensions or relations to an entity that no longer exists q

Features that cannot be rebuilt, such as a fillet that is too large

The

Rebuild Errors

dialog box displays the rebuild error information.

Selection Filter

To make it easier to select specific items, you can set the

Selection Filter

to the kind of item that you want to select. The Selection Filter toolbar offers many selection options.

For example, when you are working with parts, you can set the filter to select only faces, edges, or vertices.

You can also set the

Selection Filter

for reference geometry, sketch entities, or dimensions and annotations.

With the filter set, the kinds of items that you specified are identified when you pass the pointer over them. Sometimes they are highlighted, and sometimes the pointer changes shape. This makes it easy for you to select only the items that you intend to select.

Face

Selection

Edge

Selection

Vertex

Selection

Working with Features and Parts

Revolve and Sweep Features

Loft Features

Pattern Features

Fillet Features

More about Features and Parts

SolidWorks 2001 Getting Started

Revolve and Sweep Features

In this chapter, you create the candlestick shown here. This chapter demonstrates: q

Creating a revolved feature q

Sketching and dimensioning arcs and an ellipse q

Creating a sweep feature q

Using relations q

Creating an extruded cut feature with a draft angle

SolidWorks 2001 Getting Started 7-1

Working with Features and Parts

Sketching a Revolve Profile

You create the base feature of the candlestick by revolving a profile around a centerline.

Click

New

, select the

Tutorial

tab, and doubleclick the

Part

icon to open a new part.

Click

Sketch

to open a sketch on the

Front

plane.

Click

Line

Sketch a vertical line through the origin, and sketch the two horizontal lines as shown.

Click

Dimension

or right-click and select

Dimension

from the shortcut menu. Dimension the lines as shown.

Now sketch and dimension the arcs and lines needed to complete the profile.

Click

3 Pt Arc

Tools, Sketch Entity, 3 Point

Arc

, and point at the endpoint of the top horizontal line.

a) b) c)

Drag an arc downward for a length of approximately 20mm (L=20), and release the pointer.

Then drag the highlighted point to adjust the angle of the arc to 180° (A=180°) and the radius to 10mm (R=10). Notice that the center point of the arc snaps to the vertical inferencing line.

Release the pointer.

7-2

TIP:

Watch the pointer for feedback and for inferencing. As you sketch, inferencing pointers and lines help you align the pointer with existing sketch entities and model geometry. For more information about inferencing, see the SolidWorks 2001 Online User’s Guide.

Chapter 7 Revolve and Sweep Features

Click

Line

or right-click and select

Line

, then sketch a vertical line starting at the lower endpoint of the arc.

Do not dimension the line at this time.

Click

3 Pt Arc

or right-click and select

3 Point

Arc

, and sketch an arc with the following measurements: length of 40mm, angle of 180°, and radius of 20mm.

Sketch the arc so that the arc endpoints are coincident with the line.

Click

Trim

or , and point at the sketch segment between the endpoints of the arc.

The sketch segment is highlighted. Click the highlighted segment to delete it.

Right-click and select

Dimension

from the shortcut menu. Dimension the upper vertical line to 40mm.

Click

Add Relation

or .

The

Add Geometric Relations

dialog box appears.

a) b) c)

Click the vertical lines on each side of the arc.

Select

Equal

in the

Add Geometric Relations

dialog box.

Click

Apply

, then click

Close

Click

Tangent Arc

or , and point at the endpoint of the lower vertical line. Drag the arc until the angle is 90° and the radius is

60mm. Release the pointer.

Sketch another tangent arc. Drag the arc until the endpoint is coincident with the endpoint of the bottom horizontal line.

SolidWorks 2001 Getting Started 7-3

Working with Features and Parts

Dimension the rest of the sketch as shown.

When you are done dimensioning, the sketch is fully defined. (All lines and endpoints are black.)

Click

Centerline

Sketch Entity, Centerline

, and sketch a vertical centerline through the origin.

This centerline is the axis around which the profile revolves.

Creating the Revolve Feature

Click

Revolved Boss/Base

on the

Features toolbar, or

Insert, Base,

Revolve

The

Base-Revolve

PropertyManager appears.

Leave the default values of

Revolve

Type

One-Direction

, and

Angle

360°.

Click

OK .

Save the part as

Cstick.sldprt

7-4

Chapter 7 Revolve and Sweep Features

Sketching the Sweep Path

A sweep is a base, boss, or cut created by moving a section along a path. In this example, you create the candlestick handle by using a sweep.

First, you sketch the sweep path. The path can be an open curve, or a closed, non-intersecting curve. Neither the path nor the resulting sweep may self-intersect.

Click the

Front

plane in the FeatureManager design tree, then click

Sketch

to open a new sketch.

Click

Front

on the Standard Views toolbar, and click

Hidden Lines

Removed

on the View toolbar.

Click

View, Temporary Axes

. Notice that the temporary axis of the revolved base appears.

Right-click and select

Line

. Point at the temporary axis.

The pointer changes to indicating that the pointer is exactly on the temporary axis.

Sketch a horizontal line as shown, and dimension the line to 60mm.

Select

Tangent Arc

from the shortcut menu, and sketch an arc. Dimension the arc to a radius of

150mm.

TIP:

If the centerpoint of a radial dimension is out of view, right-click the dimension, and select

Properties

. Select the

Foreshortened radius

check box, then click

Select the endpoints of the tangent arc, and set the vertical dimension to

65mm.

TIP:

As you move the pointer, the dimension snaps to the closest orientation. When the preview indicates the dimension type and location you want, right-click to lock the dimension type. Click to place the dimension.

SolidWorks 2001 Getting Started 7-5

Working with Features and Parts

Select

Tangent Arc

from the shortcut menu, and sketch another arc as shown.

Dimension it to a radius of 20mm.

7-6

9 a) b) c)

Click

Add Relation

or . The

Add Geometric Relations

dialog box appears.

Click the endpoints of the tangent arc you just sketched.

Make sure that

Horizontal

is selected in the

Add Geometric Relations

dialog box.

Click

Apply

, then click

Close

The dimensions and relations prevent the sweep path from changing size and shape when moved.

Click

Display/Delete Relations

or .

The

Display/Delete Relations

dialog box appears. It lists all of the relations in the current sketch, including relations that are added automatically as you sketch and relations that you add manually.

In the

Display relations by

box, make sure that

Criteria

is selected, and that

All

is selected in the

Criteria

box.

Using the

Next Previous

buttons, view each relation.

When

Type

Coincident,

click the

Entities

tab, then click each item listed beneath

Entity

The coincident relation was added automatically between the sweep path and the revolved base. The line entity is related to an entity outside the current sketch. The

External information

section lists the external entity to which the line entity has a relation. The point entity exists in the current sketch.

Click

Close

Chapter 7 Revolve and Sweep Features

Next, dimension the sweep path with respect to the revolved base.

Dimension the horizontal line of the sweep path and the bottom edge of the revolved feature to

10mm.

The sweep path is fully defined.

Close the sketch.

Sketching the Sweep Section

Select the

Right

plane from the FeatureManager design tree, then click

Sketch

to open a new sketch.

Click

Normal To

on the Standard Views Toolbar.

Click

Ellipse

Tools, Sketch Entity, Ellipse,

and sketch an ellipse anywhere.

TIP:

To sketch an ellipse, drag horizontally from the center point of the ellipse to set the width of the ellipse, release the pointer, then drag vertically to set the height.

Dimension the ellipse as shown.

Click

Add Relation

Tools, Relations, Add

Click both side points of the ellipse and add a

Horizontal

relation. This relation ensures that the ellipse is not slanted.

Click

Isometric

SolidWorks 2001 Getting Started 7-7

Working with Features and Parts

Click the center point of the ellipse and the endpoint of the horizontal line of the sweep path. Click

Coincident

, click

Apply

, and click

Close

This coincident relation ensures that the center point of the sweep section lies on the plane of the sweep path.

Click

View, Temporary Axes

to hide the temporary axis.

Close the sketch.

Creating the Sweep

Now you combine the two sketches to create the sweep.

Click

Sweep

or ,

Boss

Sweep

The

Base-Sweep

PropertyManager appears.

Under

Profile and Path

, make sure the ellipse,

Sketch3,

appears in

Profile

. If it is not displayed, click the ellipse in the graphics area.

Click

Path

.and select the path,

Sketch2

, in the graphics area.

Note how the colors in

Profile and Path

match those in the graphics area.

Under

Options

, make sure the

Orientation/twist control

is set to

Follow Path

Click

to create the sweep.

The candlestick’s handle is complete.

Save the part.

7-8

Creating the Cut

Create a cut to hold a candle.

Click the top face of the revolved base feature, then click

Sketch

Click

Normal To

Click

Circle

Entity, Circle

, and point at the sketch origin. Sketch and dimension a circle as shown.

Click

Extruded Cut

Extrude

. Under

Direction 1

, do the following:

• Leave

End Condition

Blind

• Set

Depth

to 25mm.

• Click

Draft While Extruding

, and specify an

Angle

of 15°.

Click

To see the angled cut, click

Hidden

In Gray

, and rotate the part using the arrow keys.

Chapter 7 Revolve and Sweep Features

SolidWorks 2001 Getting Started 7-9

Working with Features and Parts

Adding the Fillets

Add fillets to smooth some of the edges on the part.

TIP:

Use the

Selection Filter

to make selecting the edges in this section easier.

Click

Front

, and click

Hidden

Lines Removed

Click

Fillet

Insert, Features,

Fillet/Round

The

Fillet Feature

appears.

PropertyManager

Select these four edges

Under

Fillet Type

, leave the default

Constant radius

Under

Items to Fillet

set

Radius to

10mm.

Click the four edges indicated.

Notice the list of edges in the

Edge fillet items

box. If you click the wrong edge accidentally, click the edge in the graphics area again to deselect it, or select the name of the edge in the

Edge fillet items

box and press

Delete

Click

Fillets are added to each of the selected edges.

Click

View Orientation

, and double-click

*Trimetric

in the

Orientation

dialog box.

Click

Shaded

Save the part.

7-10

Loft Features

In this chapter, you create this chisel using loft features.

A loft is a base, boss, or cut created by connecting multiple cross sections, or profiles.

This exercise demonstrates the following: q

Creating planes q

Sketching, copying, and pasting the profiles q

Creating a solid by connecting the profiles (lofting)

SolidWorks 2001 Getting Started 8-1

Working with Features and Parts

Setting Up the Planes

To create a loft, you begin by sketching the profiles on faces or planes. You can use existing faces and planes, or create new planes. For this example, you use one existing plane and create several new planes.

Click

New

, select the

Tutorial

tab, and double-click the

Part

icon to open a new part.

By default, the planes in a SolidWorks model are not visible. However, you can display them. For this example, displaying the

Front

plane is helpful.

Click

View

, make sure

Planes

is selected, then right-click the

Front

plane in the

FeatureManager design tree. Select

Show

from the shortcut menu. (To make it easier to see the planes as you add them, click

View Orientation

, and double-click

*Trimetric

With the

Front

plane still selected, click

Plane

on the Reference Geometry toolbar, or click

Insert, Reference Geometry, Plane

Select

Offset

and click

Next

Set the

Distance

to 25mm, and click

Finish

A new plane,

Plane1

, is created in front of the

Front

plane.

The planes used in a loft do not have to be parallel, but for this example they are.

With

Plane1

still selected, click

Plane

again, and add another offset plane at a distance of 25mm (this is

Plane2

Another way to create an offset plane is to copy an existing plane. Select

Plane2

in the graphics area, hold down

Ctrl

, and drag to a location in front of

Plane2

. Drag the edge or the label, not the handles. (Dragging the

handles changes the size of the plane display.)

Another offset plane,

Plane3

, is created.

To set the offset distance for the new plane, double-click

Plane3

, change the dimension value to 40mm, and click

Rebuild

8-2

Chapter 8 Loft Features

Sketching the Profiles

You create the chisel handle by lofting between simple profile sketches.

Click the

Front

plane either in the FeatureManager design tree or the graphics area, and click

Sketch

. Change the view orientation to

Front .

Sketch and dimension a 60mm square as shown.

TIP:

To center the dimension text between the witness lines, right-click the dimension, and select

Display options, Center text

If you move the dimension, the text remains centered (unless you drag the text outside the witness lines).

Exit the sketch.

Open a sketch on

Plane1

, and sketch a circle, centered on the origin.

It appears as though you are sketching on top of the first sketch. However, the first sketch is on the

Front

plane, and it is not affected by sketching on

Plane1

, a parallel plane in front of it.

Dimension the circle to 50mm in diameter.

Exit the sketch.

Open a sketch on

Plane2

, and sketch a circle, centered on the origin. As you drag, make the diameter of the circle coincident with the vertex of the square. (Watch for the pointer.)

Exit the sketch.

SolidWorks 2001 Getting Started 8-3

Working with Features and Parts

Copying a Sketch

You can copy a sketch from one plane to another to create another profile.

Click

Isometric

to see how the sketches line up.

TIP:

If a sketch is on the wrong plane, you can change the plane. Right-click the sketch, select

Edit Sketch Plane

, then click the new plane for the sketch in the FeatureManager design tree.

Click

Sketch3

(the larger circle) in the

FeatureManager design tree or the graphics area.

Click

Copy

on the Standard toolbar, or click

Edit, Copy.

Click

Plane3

in the FeatureManager design tree or the graphics area.

Click

Paste

on the Standard toolbar, or click

Edit, Paste

When you paste a sketch on a plane, a new sketch is created automatically on that plane.

Save the part as

loft.sldprt

8-4

Chapter 8 Loft Features

Create the Loft

Now use the

Loft

command to create a solid feature based on the profiles.

Click

Loft

or .

In the graphics area, select each sketch.

Click near the same place on each profile

(the lower-right side, for example), and select the sketches in the order you want to connect them.

A preview shows you how the profiles will be connected; the system connects the points or vertices on the profile closest to where you click.

Examine the preview.

• If the sketches appear to be connected in the wrong order, you can use the

Down

buttons in the

Loft

dialog box to rearrange the order.

• If the preview indicates that the wrong points will be connected, right-click in the graphics area, select

Clear

Selections

, and select the profiles again.

Click

to create a solid base feature.

Preview shows how profiles will be connected

SolidWorks 2001 Getting Started 8-5

Working with Features and Parts

Creating a Boss Loft

For the pointed end of the chisel, you create another loft.

If the

Front

Plane is not displayed in the graphics area, click the

Front

plane in the

FeatureManager design tree. Hold down

Ctrl

, and drag the

Front

plane to create an offset plane behind the original

Front

plane.

Right-click the new plane,

Plane4

, and select

Edit Definition

. In the

Offset Plane

dialog box, set the

Distance

to 200mm, make sure that

Reverse Direction

is selected, and click

Finish

Open a sketch on

Plane4

. Sketch and dimension a narrow rectangle as shown.

Exit the sketch.

Change to

Isometric

view, and click

Loft

, Insert, Boss, Loft

Right-click the side of the loft, and click

Select

Other

to pick the square, as shown. Then click the lower part of the narrow rectangular sketch.

Examine the preview to verify that the correct vertices will be connected.

TIP:

To select an edge or face that is behind the near surface (a hidden edge or face), rightclick and choose

Select Other

from the shortcut menu.

The

Yes/No

pointer appears. When you point and right-click

(N)

, you cycle through the edges or faces under the pointer, highlighting each of them in turn.

When the edge or face that you want is highlighted, click

(Y)

Click

and save the part.

8-6

Pattern Features

In this chapter, you learn how to create a linear pattern and a circular pattern. A linear pattern is a one- or two-dimensional array of features. A circular pattern is a circular array of features.

The steps include: q

Creating a revolved base feature q

Using mirroring to create a feature q

Creating a linear pattern q

Deleting and restoring an instance of the linear pattern q

Creating a circular pattern q

Using an equation to drive the circular pattern

SolidWorks 2001 Getting Started 9-1

Working with Features and Parts

Creating the Revolved Base Feature

In this example you create a housing for a microphone. Because the housing is cylindrical, you can create the housing as a revolved feature.

Click

New

, select the

Tutorial

tab, and double-click the

Part

icon to open a new part.

Open a sketch on the

Front

plane.

Sketch and dimension the profile as shown.

Click

Fillet

on the Sketch Tools toolbar.

a) b) c) d)

Set

Radius

to 30mm.

Leave

Keep constrained corners

selected so that the corner dimensions and relations are retained to a virtual intersection point.

Select the endpoint of the 50mm vertical line that is coincident with the endpoint of the diagonal line.

Click

Close

The corner is filleted away.

9-2

Sketch a vertical

Centerline

through the origin.

The centerline is the axis around which the profile revolves.

Click

Revolved Boss/Base

on the

Features toolbar, or click

Insert, Base,

Revolve

Under

Revolve Type

leave the value as

One-Direction,

and under

Direction 1

, leave the value of 360°

Click

to create the revolved base.

Click

Hidden Lines Removed

Click

Save

, and save the part as

Mhousing.sldprt

Chapter 9 Pattern Features

SolidWorks 2001 Getting Started 9-3

Working with Features and Parts

Extruding a Thin Feature

Now, create a thin-walled extrusion for the microphone capsule.

Select the top face and open a sketch.

Click

Top

to change the view orientation.

Click

Offset Entities

Under

Parameters

, do the following:

a) b)

Set the

Offset Distance

to 2mm.

Select the

Reverse

check box to offset the edge to the inside.

Click

to exit the

Offset Entities

PropertyManager.

Click

Extruded Boss/Base

Extrude

Under

Direction 1

do the following:

a) b)

Leave

End Condition

Blind

Specify a

Depth

of 5mm.

Select the

Thin Feature

check box and do the following:

a) b) c)

Click

Reverse Direction

to extrude the wall to the inside.

Leave

Type

One-Direction

Set

Wall Thickness

to 3mm.

Click

Save the part.

to create the thin-walled extrusion.

9-4

Chapter 9 Pattern Features

Shelling the Part

Hollow out the part by removing the top and bottom faces.

Click

Hidden In Gray

Click

Shell

or .

Under

Parameters

, do the following:

a) b)

Set

Thickness

to 3mm.

Click the

Faces to remove

, then click the top and bottom faces as shown. Use

Select Other

from the shortcut menu to select the lower face.

Select these faces

Click

To see the shelled part better, click

Shaded

and rotate the part.

SolidWorks 2001 Getting Started 9-5

Working with Features and Parts

Creating an Oblong Cut

Next you create a profile of an oblong on a reference plane. Use mirroring to take advantage of symmetry and to decrease the number of relations needed to fully define the sketch.

Click

Hidden Lines Removed

Open a sketch on the Front plane, and click

Normal To

Click

Centerline

, and sketch a vertical centerline through the origin.

Click

Line

, and sketch two horizontal lines of equal length, beginning at the centerline.

Watch for the on-curve pointer that indicates when you are exactly on the centerline.

Click

3 Pt Arc

or right-click and select

3 Point Arc.

Create a 3-point arc as shown.

Adjust the angle of the arc to 180°. Then press

Esc

to deselect the 3-point arc tool.

9-6

Chapter 9 Pattern Features

Mirror the sketch entities.

a) b)

Hold down

Ctrl

, and select the centerline, both horizontal lines, and the 3-point arc.

Click

Mirror

on the Sketch Tools toolbar, or click

Tools, Sketch Tools,

Mirror

Dimension the oblong as shown.

Now that the sketch is fully defined, create the cut.

Click

Isometric

Click

Extruded Cut

or .

The

Cut-Extrude

PropertyManager appears.

Under

Direction 1

, set

End Condition

Through

All

Click

to create the cut.

SolidWorks 2001 Getting Started 9-7

Working with Features and Parts

Creating the Linear Pattern

Next create a linear pattern of the oblong cut. You use a vertical dimension to specify the direction in which to create the linear pattern.

Double-click

Cut-Extrude1

in the FeatureManager design tree.

The dimensions of the

Cut-Extrude1

feature appear in the graphics area.

Click

Linear Pattern

on the Features toolbar, or click

Insert, Pattern/Mirror,

Linear Pattern

Under

Direction 1

, set the following:

a) b) c) d)

In the graphics area, click the 60mm dimension as the

Pattern Direction

If necessary, click

Reverse Direction

so the arrow in the graphics area points up.

Set

Spacing

to 10mm. This value is the distance from a point on one instance of the patterned feature to the corresponding point on the next instance.

Set the

Number of instances

to 4. This value includes the original cut-extrude feature.

Under

Features to Pattern

, make sure that

Cut-Extrude1

is listed.

Under

Pattern Options

, select the

Geometry pattern

check box.

The Geometry pattern option speeds up the creation and rebuilding of the pattern. Individual instances of the feature are copied, but not solved.

For more information about

Geometry pattern

, see

“Features” in the SolidWorks 2001 Online User’s

Guide.

Click

to create the linear pattern.

Save the part.

9-8

Chapter 9 Pattern Features

Creating a Circular Pattern of a Linear Pattern

Now create a circular pattern of the linear pattern, using a temporary axis as the axis of revolution.

Click

View, Temporary Axes

Click

Circular Pattern

on the Features toolbar, or click

Insert, Pattern/Mirror, Circular

Pattern

The

Circular Pattern

PropertyManager appears.

Under

Pattern Parameters

, set the following:

In the graphics area, click the temporary axis that passes through the center of the revolved feature.

b) c)

Axis <1>

appears in the

Pattern Axis

box. If necessary, click

Reverse Direction

so the arrow in the graphics area points up.

Set

Spacing

to 120°.

Set

Number of Instances

to 3.

Under

Features to Pattern

, make sure that

LPattern1

is listed.

Under

Pattern Options

, select the

Geometry pattern

check box.

Click

to create the circular pattern.

A circular pattern of the linear pattern is created around the part’s axis of revolution.

Click

View, Temporary Axes

to turn off the display of axes, then click

Shaded

NOTE:

If you need to use a circular pattern in a part that does not have a temporary axis in the desired place, you can create an axis, or you can use a linear edge as an axis. For more information about creating an axis, see “Reference

Geometry,” in the SolidWorks 2001 Online User’s Guide.

SolidWorks 2001 Getting Started 9-9

Working with Features and Parts

Using an Equation in the Pattern

You can use an equation to drive the circular pattern. In this example, the equation calculates the spacing angle by dividing 360° by the number of instances desired. This creates a full circle of equally spaced patterns.

In the FeatureManager design tree, double-click

CirPattern1.

Two values appear on the part: 3 (total instances) and 120° (spacing angle).

Click

Equations

on the Tools toolbar, or click

Tools, Equations

Click

Add

in the

Equations

dialog box.

Click the spacing angle value (120) on the part. (You may have to move the dialog boxes to uncover the dimension.)

The name of the value,

D2@CirPattern1

(the second dimension in the circular pattern), is entered the

New Equation

dialog box.

Using the calculator buttons in the

New Equation

box, enter

= 360 /

(or type

=360/

Click the total instances value (3).

D1@CirPattern1

is added to the equation.

The equation should look as follows:

“D2@CirPattern1” = 360 / “D1@CirPattern1”

Click

to complete the equation, and click

again to close the

Equations

dialog box.

Equations

folder is added to the FeatureManager design tree. To add, delete, or edit an equation, right-click the folder, and select the desired operation.

Now test the equation.

Increase the total instances of the circular pattern from three to four.

a) b)

Double-click the total instances value (3).

Set the value in the

Modify

dialog box to 4.

Click in the

Modify

dialog box to rebuild the model, then click to save the current value and to close the

Modify

dialog box.

– or –

Press

Enter

, then click

Rebuild

on the Standard toolbar, or click

Edit, Rebuild.

Save the part.

9-10

Fillet Features

This chapter describes how to use different types of fillets. In this example, you create a knob by: q

Using relations in your sketches q

Adding draft angles to extruded features q

Adding fillets

•

face blend

•

constant radius

•

variable radius fillets

Using mirroring to assure symmetry q

Using circular patterns with equal spacing

SolidWorks 2001 Getting Started 10-1

Working with Features and Parts

Creating the Base

You can capture the symmetry of the knob in the design intent of the part. You build one half of the part, then mirror the model to create the other half. Any changes you make to the original half are reflected in the other half.

When you relate features to the origin and the planes, you need fewer dimensions and construction entities. You can more easily modify the part when you build it this way.

Click

New

, select the

Tutorial

tab, and double-click the

Part

icon to open a new part.

Open a sketch on the Front plane .

Sketch a centerpoint arc.

a) b) c)

Click

Centerpoint Arc

on the Sketch Tools toolbar, or click

Tools, Sketch

Entity, Centerpoint Arc

Drag downward from the origin. A circumference guideline appears.

Drag an arc 180° counterclockwise around the origin.

TIP:

The pointer changes to when a 180° arc exists.

10-2

Connect the arc endpoints with a vertical line.

Dimension the arc radius to 15mm.

Select the line, hold down

Ctrl

, click the origin, click

Add

Relation

, and add a

Midpoint

relation.

Click

Extruded Boss/Base

Under

Direction 1

do the following:

a) b)

Set

End Condition

Blind.

Set

Depth

10mm.

Click

to create the extrude.

Chapter 10 Fillet Features

Creating the Grip

Now, create the grip of the knob.

Change the view orientation to

Right

Click the

Right

plane, and open a sketch.

Sketch four lines as shown to create the profile.

Do not create any inferenced perpendicular relations between lines.

Add a

Collinear

relation between the vertical sketch line and the model edge.

Profile

Collinear

Dimension as shown.

Click

Extruded Boss/Base

Extrude

Under

Direction 1

do the following:

a) b)

Set

End Condition

Blind.

Set

Depth

to 5mm.

Click

to create the extrude

SolidWorks 2001 Getting Started 10-3

Working with Features and Parts

Adding Draft to the Grip

Change the view orientation to

*Dimetric.

Click

Draft

on the Features toolbar, or click

Insert, Features, Draft

•

Leave

Type of draft

Neutral Plane.

•

Set

Draft angle

to 10°.

• Select the

Right

plane as

Neutral plane

•

Click

Faces to draft

, and select the three faces shown.

Click

to create the drafts and to close the dialog box.

Select these faces

Creating a Face Blend Fillet

Next, blend some of the faces using a face blend fillet with a hold line. This type of fillet removes the faces that share an edge with the hold line. The distance between the hold line and the selected edges determines the radius of the fillet.

Click

Fillet

Under

Fillet Type

select

Face fillet

Under

Items to fillet

, do the following:

a) b)

Click

Face set 1

, and select the face labeled

Face set 1

Click

Face set 2

, and select the face labeled

Face set 2

Under

Fillet options

, click

Hold lines

, and select the edge labeled

Hold line

Click

Face set 1

Face set 2

Hold line

Save the part as

Knob.sldprt

10-4

Chapter 10 Fillet Features

Creating Constant Radius Fillets

Now, round some of the edges using a series of constant radius fillets.

Click

Fillet

Fillet/Round

a) b) c) d)

Select the edge of the grip labeled

5.00mm

Under

Fillet Type

leave as

Constant

Radius

Under

Items to fillet

, set

Radius

5mm.

Click

5mm

2mm

0.5mm

Repeat Step 1 to add fillets to the edges labeled

2mm

and

0.5mm

. Change the radius values to match the values of the labels.

TIP:

When filleted edges intersect, it is good practice to add the larger fillet first.

SolidWorks 2001 Getting Started 10-5

Working with Features and Parts

Creating a Variable Radius Fillet

Click

Fillet

Fillet/Round

Under

Fillet Type

select

Variable Radius

Select the four edges shown here.

Under

Variable radius parameters

, set the radius values for the five vertices as shown in the illustration.

a) b)

Click

in .

Change the value in the

Radius

box to match the value of the label.

The value for

appears in the list.

Click each vertex in the

Vertex List

, and change the value to match the label.

Click

to close the

Fillet Feature

dialog box.

TIP:

To verify the radius values, double-click

VarFillet1

in the

FeatureManager design tree.

Save the part.

Select these edges

R1.5

10-6

Chapter 10 Fillet Features

Mirror the Model

To take advantage of the part’s symmetry and to finish the part, mirror the part about the planar face that is coincident with the

Right

plane.

Change the view orientation to

Left

Click

Insert, Pattern/Mirror, Mirror All

Select the planar face shown.

Click

A mirror image of the original part is joined to the part at the selected face to make a complete, symmetrical part.

Select this face

Fillet the Parting Line

When you mirrored the drafted grip, it created a parting line along the top of the grip.

Smooth the parting line by adding a constant radius fillet.

Change the view orientation to

*Dimetric.

Click

Fillet/Round.

a) b) c)

Fillet

Select the edge shown.

Under

Fillet Type

leave as

Constant

Radius

Under

Items to fillet

, set

Radius

5mm.

Select this edge

3 d)

Make sure

Tangent propagation

is selected.

The fillet extends along all of the segments of the edge.

Click

SolidWorks 2001 Getting Started 10-7

Working with Features and Parts

Creating a Thin-Walled Body

Now remove material from the round base of the knob to create a thin-walled body.

Change the view orientation to

Back

Select the back face of the knob, and open a sketch.

With the back face still selected, click

Offset

Entities

Under

Parameters

, set

Offset

to 1mm, and select

Reverse

to offset the edge to the inside.

Select this face

Click

Change the view orientation to

Isometric

Click

Extruded Cut

Extrude

Under

Direction 1

, do the following:

a) b) c)

Set

End Condition

Surface.

Offset From

Click

Face/Plane

and select the face shown.

Set

Offset distance

to 1mm.

Click

TIP:

Using

Offset Entities

and

Offset

From Surface

ensures that the wall thickness remains 1mm, even if you change the base diameter or base depth.

To examine the part, click

Rotate View

and rotate the part.

Save the part.

Offset from this face

10-8

Chapter 10 Fillet Features

Using Equal Spacing in a Circular Pattern

To add a pattern of bosses inside the knob, use a circular pattern with equal spacing. With the equal spacing option, you specify the number of instances and the total angle, and the software calculates the spacing.

Change the view orientation to

Back and open a sketch on the narrow circular face.

Sketch a horizontal centerline through the left side of the narrow circular face and the origin, and click

Mirror

or .

Sketch a line from the inner edge of the narrow circular face towards the origin, at a slight angle, as shown.

Click

Mirror

to turn mirroring off, and sketch a vertical line to connect the two endpoints closest to the origin.

Click the inside edge of the circular face and click

Convert Entities

Tools, Convert Entities.

Click

Trim Tools, Sketch Tools, Trim

and select the large arc to trim the circle.

Dimension as shown.

Extrude the sketch as a boss using the

Boss-

Extrude

PropertyManager.

Under

Direction 1

, do the following:

a) b)

Set

End Condition

Up to Surface

Click

Face/Plane

, and click the inner circular face in the graphics area.

Click

Rotate View

to slightly rotate the part to see the extrusion.

Click

View, Temporary Axes

SolidWorks 2001 Getting Started 10-9

Working with Features and Parts

Make sure the boss is selected and click

Circular Pattern

Mirror, Circular Pattern

b) c) d)

Under

Pattern Parameters

, do the following:

Click the

Pattern Axis

box, then click the axis through the origin in the graphics area.

Set

Spacing

to 360°.

Set

Number of Instances

Click the

Equal Spacing

check box.

Under

Features to Pattern

, make sure

Boss-

Extrude2

is displayed.

Under

Pattern Options

, click to clear

Geometry pattern

, if necessary.

Click

and save the part.

For more information about

Geometry pattern

, see “Features” in the SolidWorks 2001

Online User’s Guide.

10-10

More about Features and Parts

The section “Working with Features and Parts” introduces you to many functions available with SolidWorks 2001. The following pages highlight some additional

SolidWorks functionality. For more information, see the SolidWorks 2001 Online User’s

Guide.

Parts

Parts are the basic building blocks of the SolidWorks mechanical design software. This section highlights some ways to work with parts.

Derived Parts

You can select which configuration of the original part to use for a derived part. The three types of derived parts are:

Base Part

Mirror Part

, and

Derived Component Part

Check Entity

The check entity function allows you to verify the integrity of a part.

•

Check All - choose to check the entire body, only the solid model, or only the surface bodies

•

Check Selected items - select to check more than one entity (face, edge, or surface body) at the same time

•

Maximum edge gap and Maximum vertex gap - report the maximum tolerance between the edges and vertices in the selected items.

The Found column displays the number of items found with the specified error, and the

Result list box displays the items that are either invalid or too short.

More about Features and Parts

Mass Properties

Displays the density, mass, volume, surface area, center of mass, inertia tensor, and principal axes of inertia of a part or assembly model. Capabilities include:

•

Density - change the density of a part from the

Measurement Options

dialog box.

•

Units - enter the value using any units, and the software converts the value to the document’s units.

•

Updates - update the mass properties information when you save a document.

•

Coordinate Systems - calculate mass properties using a coordinate system. The moments of inertia are calculated at the origin of the coordinate system, using its axes.

Section View of a Model

You can display a view of the model cut through the part or the assembly by identifying any combination of planes and planar model faces as section planes.

Lighting

With Lighting (in the FeatureManager design tree), you can adjust the direction, intensity, and color of the light in the shaded view of the model. As you change the properties of light, a graphical representation of the light source is displayed and the model is updated.

The available light properties depend on the type of light source. Light sources include: q

Ambient

Directional

Point

Spot

The sample below displays how you can manipulate

Intensity

properties for a

Directional

light source.

Brightness

controls the amount of light.

Specularity

controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them.

Higher values for

Ambient

and

Brightness

Higher value for

Specularity

Reference Geometry

Reference geometry defines the shape or form of a surface or solid. Reference geometry includes planes, axes, coordinate systems, and 3D curves.

Planes

You can create any of the following types of planes to facilitate your design intent: q

Offset - a plane parallel to a plane or face, offset by a specified distance q

At Angle - a plane through an edge, axis, or sketch geometry at an angle to a face or a plane q

Three Point Plane - a plane through three points (vertices, points, or midpoints) q

Parallel Plane at Point - a plane through a point parallel to a plane or face q

Line and Point - a plane through a line, axis, or sketch line and a point q

Perpendicular to Curve at Point - a plane through a point and perpendicular to an edge, axis, or sketch curve q

On Surface - a plane on a non-planar surface

You can do the following to any type of plane: q

Move, resize, and copy q

Change the name q

Hide or show q

Change the plane of a sketch

SolidWorks 2001 Getting Started

More about Features and Parts

Coordinate System

You can define a coordinate system for a part or assembly. You can also edit the definition or move the coordinate system to a new location. Use a coordinate system as follows:

•

Measure

- enables you to measure the size of, or the distance between, entities.

•

Mass Properties

- displays density, mass, volume, surface area, center of mass, inertia tensor, and principal axes of inertia of a part or assembly model.

Curves

A curve is a type of geometry. Using various methods, you can create several types of 3D curves. One method is the

Projected Curve

. The example below displays how you can create a projected curve using sketches on intersecting planes.

Create sketches on two intersecting planes

Align sketch profiles projected normal to their sketch planes and create projected curve

Create profile sketch Sweep profile sketch along curve

You can also create 3D curves by using the following methods:

•

Composite

- combining curves, sketch geometry, and model edges into a single curve

•

Helix/Spiral

- specifying values such as pitch and revolutions for a helix or spiral

•

Split Line -

projecting sketched curves onto selected model faces

•

Curves Through Reference Points

- creating 3D spines through points on one or more planes

•

Curves Through Free Points

- using a point list to create a 3D curve

Features

Features are the individual shapes that, when combined, make up the part. This section describes several SolidWorks features.

Using additional functionality to some familiar features (such as Loft or Chamfer ) q

Creating patterns that are table driven and sketch driven q

Applying more complex fillets including, multiple radius fillets, round corner fillets, and setback fillets q

Using uniform and non-uniform scaling to edit models

Loft

You can create lofts using various options. For example, you can create a loft using:

•

Planar or non-planar profiles

•

Parallel or-non parallel planes for the profiles

•

Guide curves to connect and control intermediate profiles

•

Center line to act as a guide curve, with all profile planes normal to the center line

•

Tangency options to control the tangency at the starting and ending profiles

The sample displays combining a non-planar profile and two planar profiles sketched on offset planes.

Non-planar profile

Planar profile

SolidWorks 2001 Getting Started

More about Features and Parts

Chamfer

Chamfer creates a beveled edge on the selected edges, faces, or both. You can select from several chamfer types (as shown below), and specify the necessary parameters.

Angle-Distance Distance-Distance Vertex-Chamfer

Rib

Rib is a special type of extruded feature created from an open sketched contour. It adds material of a specified thickness in a specified direction between the contour and an existing part. You can create a rib using either closed or open sketch elements

Closed contour

Open contour

Fillets

There are many different types of fillets. Some of the fillet features not covered in the section “Working with Features and Parts” include:

• Multiple radius fillets

•

Setback fillets

•

Round corner fillets

Multi-radius Round corner

Setback radius

Sketch Driven Patterns

Using sketch points within a sketch, you can specify a feature pattern. You can use sketch driven patterns for holes or other feature instances. Sketch driven patterns use:

•

Seed features - representing the geometry you want to replicate.

•

Reference point - using a reference point such as a vertex or a centroid as an origin.

•

Reference Sketch - representing a sketch on a face of the original part or assembly, sketch points designate the pattern propagation.

Initial pattern instance

Sketch points for

Completed pattern

SolidWorks 2001 Getting Started

More about Features and Parts

Table Driven Patterns

Using X-Y coordinates, you can specify a feature pattern. Hole patterns using X-Y coordinates are a common application for table-driven patterns. However, you can use other features, such as a boss, with table-driven patterns. You can also save and retrieve the X-Y coordinates of a feature pattern. Like sketch driven patterns, table driven patterns use seed features and reference points. Table driven patterns also use:

•

Coordinate system - using a coordinate system to act as the point of origin, and defining the X-Y coordinates that populate the table.

•

X-Y points - designating X-Y coordinates (both positive and negative) in the table, with each coordinate set representing an instance of the pattern.

Scaling

You can select to scale using a coordinate system, the origins or the centroid. You can also select a non-uniform scaling factor by entering X-Y-Z coordinates. For example, you can apply non-uniform scaling by specifying the X-Y-Z coordinates to vary the cavity in a mold.

Results of

Uniform Scaling

Normal Part

Results of Non-uniform

Scaling

Surfaces

Surfaces are a type of geometry. You can create surfaces, use surfaces to manipulate features, or manipulate the surfaces themselves.

Creating Surfaces

You create surfaces with many of the same tools and principles used to create solids, including:

•

Extrude

- extrude sketch profile

•

Loft

- use multiple, parallel or non-parallel planes, with or without guide curves

(see the sample below)

•

Sweep

- create planes to sketch a sweep profile, sweep path, and guide curves

•

Offset

- offset surface from a lofted model surface (see the example below)

Offset Surface

•

Radiate

- create surfaces by radiating a parting line, an edge, or a set of contiguous edges inwards or outwards, and parallel to a selected plane (see the example below)

Guide curve

Radiate Surface with a Split Line

Guide curve loft

•

Revolve - use a surface and revolve about an axis.

SolidWorks 2001 Getting Started

More about Features and Parts

Manipulate Features with Surfaces

You can use surfaces to create and manipulate features. This includes:

•

Fill volumes between surfaces - create a solid body by lofting between two surfaces

•

Thicken surface - create model geometry by thickening the surface

•

Cut part with surface - use surfaces to cut parts (see example below)

Selected surface

Direction of cut

Feature section removed

Results after the cut

Manipulate Surfaces

You can also manipulate surfaces. Some ways of manipulating surfaces include:

• Trim - use a surface to trim another surface where they intersect, or use multiple surfaces as mutual trim tools.

Surface trim

Surface using mutual trim

•

Knit - combine two or more surfaces or faces into one.

•

Fillet - smooth the edge between adjacent faces in a surface. You can also use

Face Blend to combine multiple surface bodies, or Multiple radius fillet to assign multiple radius values.

Surfaces before adding the face blend fillet

Surfaces after adding the face blend fillet

• Extend - extend a surface body by selecting one or more edges or faces.

Surface extend using Linear

Surface extend using

Same Surface

SolidWorks 2001 Getting Started

Surface extend using Face

SolidWorks 2001 Getting Started

Working with Assemblies

Assembly Mates

Advanced Design Techniques

More about Assemblies

This chapter guides you through the creation of the universal joint assembly shown here, and demonstrates the following: q

Bringing parts into an assembly q

Using these assembly mating relations:

•

Coincident

•

Concentric

•

Parallel

•

Tangent q

Using SmartMates q

Testing mating relations q

Exploding and collapsing the assembly

Assembly Mates

SolidWorks 2001 Getting Started 11-1

Working with Assemblies

Introduction

This assembly uses the following parts and assembly, located in the installation

directory\

samples\tutorial\universal_joint

folder.

yoke_male.sldprt

spider.sldprt

crank-assy.sldasm

u-joint_pin1.sldprt

bracket.sldprt

u-joint_pin2.sldprt

yoke_female.sldprt

11-2

Chapter 11 Assembly Mates

Setting the Assembly Load Option

You can load an assembly with its active components fully resolved or lightweight.

•

Fully resolved

. All model information is loaded in memory.

•

Lightweight

. A subset of model information is loaded in memory. The remaining model information is loaded if the component is selected or if the component is affected by changes that you make in the current editing session.

You can improve the performance of large assemblies significantly by using lightweight components.

The assembly you build in this chapter includes a sub-assembly whose parts could be loaded lightweight. However, there are no significant benefits in using lightweight parts, for these reasons:

• The sub-assembly is small, consisting of only three simple components.

• You select two of the three components as you build the assembly, thereby resolving them anyway.

Before you open the assembly document, click

Tools, Options

. On the

System

Options

tab, click

Performance

Under

Assemblies

, click to clear the

Automatically load parts lightweight

check box, then click

For more information about lightweight parts, see the SolidWorks 2001 Online User’s

Guide.

SolidWorks 2001 Getting Started 11-3

Working with Assemblies

Inserting the First Part into the Assembly

This section describes how to insert a part into the assembly.

Click

File, Open

, and open

bracket.sldprt

Open a new assembly from the

Tutorial

tab and click

View, Origins

to show the origin.

Tile the windows so that you can see both the part window and the assembly window.

Click the part name,

bracket

, at the top of the FeatureManager design tree in the

bracket.sldprt

window. Drag

bracket

into the

Assem1

window, and drop it on the assembly origin in the graphics area. As you drag, watch for the pointer shown here. This pointer indicates an inference to the assembly origin.

When you place a component this way, the component origin is located coincident with the assembly origin, and the planes of the part and the assembly are aligned. This procedure, while not required, helps you establish an initial orientation for the assembly.

NOTE:

You can create this type of inference with any component as you add it to the assembly. You can also create the inference to the assembly origin by dropping the component in the FeatureManager design tree of the assembly window.

Close the

bracket.sldprt

window, and maximize the

Assem1

window.

Notice that the FeatureManager design tree contains the feature

(f)bracket<1>

. Because this is the first component inserted into the assembly,

bracket

is fixed

(f)

. It cannot be moved or rotated unless you float (unfix) it. The

<1>

means that this is the first

instance of

bracket

in the assembly.

The assembly also contains an empty

MateGroup1

feature.

This feature is a placeholder for the mates that you add later.

Click

Isometric

, and click

Hidden Lines Removed

11-4

Chapter 11 Assembly Mates

Bringing More Components into the Assembly

Another way to add components to the assembly is to drag them in from Windows

Explorer.

Start Windows Explorer (if it is not already running).

Navigate to the \installation directory\

samples\tutorial\universal_joint

folder.

Click each of the items listed below individually, and drag it into the graphics area of

Assem1

. Place them approximately as shown.

•

yoke_male.sldprt

•

yoke_female.sldprt

•

spider.sldprt

Examine the FeatureManager design tree, and expand each item to see the features used to make the components.

Notice that each of the new components has the prefix

(-)

before its name, indicating that its location is under defined. You can move and rotate these components.

yoke_male spider bracket yoke_female

To collapse the entire FeatureManager design tree in one step, right-click

Assem1

in the FeatureManager design tree and select

Collapse Items

Practice moving and rotating the individual components using the following tools on the Assembly toolbar:

Click

Move Component

, click one of the component’s faces, then move the component.

Click

Rotate Component

, click one of the component’s faces, then rotate the component.

Both the

Move Component

and

Rotate Component

tools remain active so that you can move other non-fixed components in succession.

Save the assembly as

U-joint.sldasm

SolidWorks 2001 Getting Started 11-5

Working with Assemblies

Mating the Bracket with the Male Yoke

The following pages describe how to add various types of assembly mating relations.

First, mate the bracket and the male yoke.

Click

Mate

or ,

Mate

The

Mate

PropertyManager appears.

Click the cylindrical face of the boss on the male yoke and the cylindrical inside face of the top hole in the bracket.

NOTE:

You can also select the items to mate before opening the

Mate

PropertyManager. Hold down

Ctrl

as you select the items.

Click

Concentric ,

click

Preview

to check the mate, and click

The boss of the male yoke and the bracket hole are now concentrically mated.

To test the mate, click

Move Component

, and drag the male yoke. You can only drag up and down, following the axis of the concentric mate. (The yoke may spin as it moves.)

Select these faces

Click

Mate

or ,

Mate

again.

Click

Keep Visible

in the

Mate

PropertyManager.

The

Mate

PropertyManager stays open as you continue to add mates.

11-6

Click the top inside face of the bracket and the top face of the male yoke.

TIP:

To select the top inside face of the bracket without rotating the bracket, right-click the top of the bracket, and click

Select Other

. Click

until the correct face is highlighted, then click

Chapter 11 Assembly Mates

Select these faces

Click

Coincident Mate

PropertyManager, click

Preview

, and click

The top of the yoke is now inserted into the bracket hole.

SolidWorks 2001 Getting Started 11-7

Working with Assemblies

Mating the Male Yoke with the Spider

Select the inside faces of one pin hole on the male yoke and one spider pin hole.

Click

Concentric

, click

Preview

, and click

The spider and the male yoke are now concentrically mated.

Select the flat spider face that contains the hole you selected in Step 1 and the inside face of the male yoke.

Use

Select Other

or rotate the assembly if necessary.

NOTE:

To move and rotate components while the

Mate

PropertyManager is open, use the

Pan Rotate View

tools on the View toolbar. To exit from move or rotate mode, click the tool again or press

Esc

so you do not clear the

Selected Items

list.

Click

Coincident

, then click

Preview

The spider should be placed inside the male yoke as shown.

• If the mate looks correct, click

• If the mate looks wrong, click

Undo

, select the correct faces, and click

Click

Cancel

to close the

Mate

PropertyManager.

11-8

Mating the Female Yoke and the Spider

Using the tools on the Assembly toolbar (see

page 11-5), move and rotate the female yoke to

approximately the position shown here.

Click

Mate

Insert, Mate

, then click

Keep Visible

in the

Mate

PropertyManager.

Select the inside face of the pin hole of the female yoke and one of the visible spider pin holes.

Click

Concentric

, click

Preview

, and click

The spider and the female yoke are concentrically mated.

Select the flat spider face that contains the hole

you used in Step 3, and the inside face of the

female yoke.

Chapter 11 Assembly Mates

Click

Coincident

, click

Preview

, and click

The female yoke should be positioned as shown.

The rotation may be different in your assembly because it is based on the initial position of the two components before mating.

SolidWorks 2001 Getting Started 11-9

Working with Assemblies

Mating the Female Yoke with the Bottom of the Bracket

Select the bottom face of the female yoke and the top slanted face of the bracket.

Click

Parallel

, and click

Preview

The female yoke is aligned to the bracket.

If the female yoke is upside down, change the

Mate

Alignment

, and click

Preview

again.

•

Aligned

means that the normal vectors for the selected faces point in the same direction.

•

Anti-Aligned (On)

means that the normal vectors for the selected faces point in opposite directions.

•

Closest

means that the selected faces may be either aligned or anti-aligned, depending on the positions they occupy when selected.

Click

, then close the

Mate

PropertyManager.

Save the assembly.

11-10

Chapter 11 Assembly Mates

Mating the Small Pins to the Female Yoke

Another way to add components to an assembly is to use the

Insert

menu.

Click

Insert, Component, From File

, then navigate to installation

directory\

samples\tutorial\universal_joint

Select

u-joint_pin2.sldprt

, then click

Open

Click the pointer in the graphics area where you want to place the component.

The

u-joint_pin2<1>

component is added to the assembly.

Click

Mate

or then click

Keep Visible

in the

Mate

PropertyManager.

Select the cylindrical face of the pin and an inside face of a pin hole on the female yoke.

Add a

Concentric

mate.

Select the end face of the pin and the outside face of the female yoke.

Click

Tangent

and click

Preview

. If the alignment is incorrect, change the

Mate

Alignment

and click

Preview

again.

You use

Tangent

(instead of

Coincident

) for this mate because one face is flat and the other face is cylindrical.

Click

, then close the

Mate

PropertyManager.

Hold down

Ctrl

, then drag the

u-joint_pin2<1>

icon from the FeatureManager design tree into the graphics area.

A copy of the component is added to the assembly,

u-joint_pin2<2>

.The

<2>

notation indicates the second instance of this part in the assembly.

Repeat Steps 4 through 9 to mate the second instance of the pin to the other hole in the

female yoke.

Save the assembly.

SolidWorks 2001 Getting Started 11-11

Working with Assemblies

Using SmartMates to Mate the Large Pin

For some mates, you can create mating relationships automatically using SmartMates.

You can inference the geometry of existing components as you drag and drop new components into the assembly.

In this section, you create a concentric mate automatically. For more information about

SmartMates, see the SolidWorks 2001 Online User’s Guide.

Click

File, Open

, and open

u-joint_pin1.sldprt

Tile the windows so that you can see the part and the assembly windows.

Change the view orientation of the part to

Isometric

necessary.

Change the view mode in the assembly window to

Shaded

, and change the view orientation to

Isometric

. Zoom in on the pin hole in the male yoke.

Shaded

mode allows you to see the preview of SmartMates better.

Select the cylindrical face of the pin, and drag the pin into the assembly. Point at an inside face of the pin hole on the male yoke in the assembly window. (The pin may disappear behind the assembly.)

When the pointer is over the pin hole, the pointer changes to . This pointer indicates that a concentric mate will result if the pin is dropped at this location. A preview of the pin snaps into place.

Preview of pin

If the preview indicates that you need to flip the alignment condition, press the

Tab

key to toggle the alignment

(aligned/anti-aligned).

Drop the pin.

A concentric mate is added automatically.

Close the

u-joint_pin1.sldprt

window, and maximize the assembly window.

11-12

Click

Mate

or , then select the end face of the pin and the outside face of the male yoke as shown.

Chapter 11 Assembly Mates

Select these faces

Add a

Tangent

mate.

Save the assembly.

SolidWorks 2001 Getting Started 11-13

Working with Assemblies

Mating the Handle to the Assembly

Click

Hidden Lines Removed

Drag

crank-assy.sldasm

from Windows Explorer and drop it into the assembly window.

Click

Mate

Insert, Mate

Select the outside face of the crankshaft and the

cylindrical face of the male yoke boss (not the flat face on the boss).

Add a

Concentric

mate and click

Click

Move Component

, and drag the crankshaft above the male yoke boss.

Click

Mate

or , and click

Keep Visible

Mate

PropertyManager.

Click

Hidden In Gray

, then click

Zoom to

Area

and zoom in on the crankshaft and male yoke boss.

Select the flat face of the male yoke boss and the flat face on the inside of the crankshaft. Use

Select Other

to more easily select any hidden faces.

Add a

Parallel

mate.

11-14

Select the bottom face of the crankshaft and the top face of the bracket. Add a

Coincident

mate.

Close the

Mate

PropertyManager, and save the assembly.

Chapter 11 Assembly Mates

Click

Isometric

, then click

Shaded

The completed assembly should appear as shown.

SolidWorks 2001 Getting Started 11-15

Working with Assemblies

Click the beside

MateGroup1

of the assembly (not the

crank-assy

sub-assembly) to see the mates.

NOTE:

If you have added or deleted mates, the names of the mates in your assembly may differ from those shown here.

Each mate is identified by the type and a number, and the names of the components involved are shown.

As you pause over each mate, the entities involved are highlighted in the graphics area.

You can rename the mates in the same way that you rename the features of a part, if desired.

Rotating the Crank Handle

You can turn the crank of the assembly by selecting the sub-assembly, and moving the handle.

Click

Move Component

. rotate crank

Click a face on one of the components of the crank sub-assembly.

Drag the pointer vertically in the graphics area.

The crank turns and rotates the male and female yokes. All of the mating relationships are maintained.

11-16

Chapter 11 Assembly Mates

Exploding the Assembly

You can create an exploded view of the assembly. An exploded view consists of one or more explode steps. In this section, you define the first step in an exploded view.

Click

Insert, Exploded View

In the

Assembly Exploder

dialog box, in the

Step editing tools

box, click

New

The

Assembly Exploder

dialog box expands.

Click a vertical edge on the bracket to set the

Direction to explode along.

If the preview arrow is pointing down, select the

Reverse direction

check box.

Click a face of a component of the crank assembly in the graphics area, or click the

crank-assy

component in the

FeatureManager design tree for the

Components to explode

box.

Examine the contents of the boxes under

Step parameters

. Make sure that the

Entire sub-assembly

option is selected. If you need to make any other changes:

• Select and delete the contents of the

Components to explode

box.

– or –

• Click the

Components to explode

box, right-click in the graphics area, select

Clear

Selections

, and select again.

Click

Apply

Notice the arrow-shaped handle in the graphics area.

Drag the green handle up and down until the crank assembly is positioned at a reasonable distance from the bracket. (You can specify the position by using the

Distance

box if you prefer.)

Click

Apply

again to confirm the new distance value in the step.

Do not click

yet. Leave the

Assembly Exploder

dialog box open, so you can continue adding steps to the exploded view. You click

only when all the steps in the view are completed.

SolidWorks 2001 Getting Started 11-17

Working with Assemblies

Adding Explode Steps

Now add explode steps for other components.

Click

New

to create the next explode step.

Click a horizontal edge on the bracket.

Click the male yoke, the female yoke, the spider and the pins (either in the graphics area or the

FeatureManager design tree).

Verify the

Step parameters

, and click

Apply

Adjust the distance as desired.

Click

Apply

Click

to save the exploded view with its two steps.

Click a blank area in the graphics area to deselect all the selected items.

To collapse the assembly, restoring it to its previous condition, right-click anywhere in the graphics area and select

Collapse

11-18

Chapter 11 Assembly Mates

Editing the Exploded View

You can edit the explode steps, or add new ones if needed. You access the exploded view from the ConfigurationManager tree.

Click the ConfigurationManager tab to change to the configuration view.

Double-click

Default

, or click the to expand the view.

If you are asked to confirm showing the configuration, click

Double-click

ExplView1

to explode the assembly again (or right-click

ExplView1,

and select

Explode

Right-click

ExplView1

, and select

Edit Definition

Using the

Previous Step

and

Next Step

buttons

, or the

Explode steps

list, review each of the steps in the exploded view. Edit any step as desired, then click

Apply

before editing or adding another step.

Click

New

to create a new explode step, then practice exploding more of the assembly. Remember to click

Apply

each time you complete a step.

When you are satisfied with the entire exploded view, click

To collapse the entire assembly, right-click the assembly name at the top of the ConfigurationManager tree, and select

Collapse

Save the assembly. You will use this assembly later in

Chapter 14, “Bill of Materials.”

SolidWorks 2001 Getting Started 11-19

Advanced Design Techniques

Suppose that you want to design a hinge assembly that you can modify easily to make similar assemblies. You need an efficient way to create two matching hinge pieces and a pin for a variety of hinge assembly sizes.

Some analysis and planning can help you develop a design that is flexible, efficient, and well defined. You can then adjust the size as needed, and the hinge assembly will still satisfy the design intent.

This chapter discusses: q

Analyzing the assembly to determine the best approach q

Using a layout sketch q

Suppressing features to create part

configurations

Creating a new part in the context of the assembly

This chapter assumes that you know how to perform basic assembly operations, such as moving and rotating components, and adding mates. (These topics are covered in Chapters 3 and 11 of this guide.)

SolidWorks 2001 Getting Started 12-1

Working with Assemblies

Analyzing the Assembly

Successful customers tell us that the key to using the SolidWorks software effectively is planning. By performing a careful analysis, you can design better, more flexible, functional models. Before you begin, analyze the assembly with the following considerations in mind: q

Consider dependencies between the components of an assembly. This will help you decide on the best approach:

• Using bottom-up design, you build the parts independently, then insert them into the assembly.

•

Using top-down design, you may begin with some ready-made parts. Then you create other components in the context of the assembly. You reference the features of some components of the assembly to drive the dimensions of the other components.

Identify the features that make up each individual part. Understand the dependencies between the features of each part. Look for patterns, and take advantage of symmetry whenever possible.

Consider the order in which the features are created, and keep in mind the manufacturing processes that will be used to make the parts.

Dependencies in the Assembly

The hinge pieces

The two pieces of the hinge are alike: the size and thickness of the body, the barrel that receives the pin, and the placement of the screw holes. The only differences between the two pieces are the cuts and tabs on the barrel, where they fit together.

There are several ways to approach this task: q

Copy. You could make one piece, make a copy of it, then modify the copy as needed for the second piece. However, if you wanted to make another assembly in a different size, you would need to edit both pieces. This is not the best approach; it leaves room for error because the pieces are independent of each other.

Derive. You could create a base part consisting of only the common elements, then

derive the two pieces from it (using

Insert, Base Part

Insert, Mirror Part

). To make changes to the common dimensions, you edit the original, and the derived parts are updated automatically. This behavior is useful in some circumstances, but it has drawbacks for this application. You do not have access to the driving dimensions of the original part when editing a derived part, so you cannot reference those dimensions when creating the features that differ.

12-2

Chapter 12 Advanced Design Techniques

Configure. The method that you use for this example is to make two different

configurations of the same part. This is the best way to ensure that you always have matching pieces, because a single part document is used to create the two pieces. The part document contains all the possible features to be used. Then you create configurations by suppressing selected features, removing them from the active configuration.

The pin

You need to know the dimensions of the barrel to create a pin that is exactly the right size for the assembly. By creating the pin in the context of the assembly, you can accomplish this for any size hinge.

Conclusion

For this assembly, it makes sense to use a combination of design methodologies. First, design the hinge pieces, including the necessary configurations, and insert them in an assembly (bottom-up design). Then design the pin in the context of the assembly

(top-down design), referencing the model geometry of the hinge pieces as necessary.

Analysis of the Individual Parts

Now that you understand the dependencies between components, take a look at the parts individually.

The common features of the hinge pieces

The base feature is a flat rectangle, with a round barrel along one edge. The diameter of the barrel is dependent on the thickness of the base. Each piece has four countersunk holes. The position of the holes is symmetric with respect to the midpoint of the long edge.

As the size of the hinge changes, you want the holes to remain properly spaced along the length and width.

The different features of the hinge pieces

The cuts (and corresponding tabs) along the barrel are the features that distinguish the two pieces. One piece has three cuts, and the other has two cuts. The placement is symmetric with respect to the midpoint of the long edge. Each cut should be slightly larger than the corresponding tab, so the hinge will not bind when assembled.

The pin

The pin is dependent on the hinge pieces for its length and diameter dimensions. The domed head of the pin should match the outer diameter of the barrel.

SolidWorks 2001 Getting Started 12-3

Working with Assemblies

Feature Order

Now, outline the features you will use and decide on the order to create them.

Base feature – extrude as a thin feature. Because the part has symmetric features, use a mid-plane extrusion. Then you can use the mid-plane as a plane of symmetry for mirroring other features.

Barrel – sweep a circular profile along the long model edge. Then extrude a cut, concentric with the boss.

Countersunk holes – use the

Hole Wizard

to create a complex hole profile, then use equations and mirroring to position several copies.

Cuts for tabs – create a layout sketch, referencing the dimensions of the base. Use the sketch to extrude two different cut features, one with three tabs, one with two tabs.

Configurations – define the two configurations used in the assembly by suppressing one cut feature in each configuration.

Assembly – insert and mate the hinge pieces (one of each configuration).

Pin – insert a new part while in the assembly. Reference the geometry of the hinge piece to sketch a profile and a path. Then use a sweep to create the base feature.

Pin head – convert the barrel profile to create a sketch, then extrude it. Finally, add a dome to the flat surface of the head.

A Final Word

This may seem like a great deal of planning to develop a simple assembly. However, it is a worthwhile exercise if it helps you discover the best approach to building the parts before you start designing them. By thoroughly analyzing the issues before you begin, you can create a flexible, fully parametric model. When you change any of its parameters, the others update accordingly.

For more examples that showcase design intent and implementation, view the SolidWorks

Design Portfolio by clicking

Help

Design Portfolio

12-4

Chapter 12 Advanced Design Techniques

Creating the Basic Hinge Piece

Open a new part from the

Tutorial

tab and open a sketch on the

Front

plane.

Sketch a vertical line and dimension it to 60mm in length.

Click

Extruded Boss/Base

or to extrude the sketch:

Under

Direction 1

, do the following:

•

Set

End Condition

Mid Plane

•

Set

Depth

120mm.

Under

Thin Feature

, do the following:

•

Leave

Type

One-Direction

•

Set

Direction 1 Thickness

to 5mm.

Click

Open a sketch on the narrow vertical face. Sketch a circle at the upper edge, with its center at the front vertex.

Add a coincident relation between the edge of the circle and the back vertex to fully define the sketch. Close the sketch.

Click

Sweep

. Select the circle as the

Profile

. Select the

Path Boss-Sweep

PropertyManager and click one of the long model edges. Click

Cut a hole through the barrel:

a) b) c)

Open a sketch on the narrow face.

Sketch and dimension a small circle as shown, and add a concentric relation to the outside edge of the barrel.

Click

Extruded Cut

or .

Set

End

Condition

Through All

, and click

Save the part as

Hinge.sldprt

SolidWorks 2001 Getting Started 12-5

Working with Assemblies

Adding the Screw Holes

In this section, you add holes for screws. To position each hole, one dimension is fixed, and the other is driven by an equation.

Click the large model face, then click

Hole Wizard

on the Features toolbar, or click

Insert, Features, Hole, Wizard

On the

Countersink

tab of the

Hole Definition

dialog box, set the following values:

•

Standard

Ansi Metric

•

End Condition & Depth

Through All

•

Hole Fit & Diameter

Normal

and 8mm.

•

C’Sink Diameter & Angle

to 15mm and 82°.

Click

Next

, then click on the large model face to add the center point for a second hole.

Hole1 Hole2

Click

Select

and drag the points to the approximate location on the face shown here. Click

Finish

Right-click the under defined sketch containing the points for

Hole1

, and select

Edit Sketch

. Dimension the points to the edges of the hinge as shown. Do not close the sketch.

c) d) e)

Add an equation to control the location of one of the points:

a) b)

Click

Equations

on the Tools toolbar or

Tools,

Equations

, then click

Add

Clear the default text in the

New Equation

dialog box, if necessary.

Select the 30mm dimension, then type

Double-click the base to expose its dimensions then select the 60mm dimension.

Type

to complete the dimension and click

to close the

New Equation

dialog box.

This sets the distance between the point and the bottom edge to one-half the height

(60mm) of the hinge.

12-6

Chapter 12 Advanced Design Techniques

8 a) b) c) d) e)

Add an equation to control the location of the other point:

Click

Add

in the

Equations

dialog box.

Clear the default text in the

New Equation

dialog box, if necessary.

Select the 40mm dimension then type

Double-click the base to expose its dimensions then select the 120mm dimension.

Type

to complete the dimension and click

to close the

New Equation

dialog box.

The distance between the point and the side edge equals one-third of the length

(120mm) of the hinge.

Click

to close the

Equations

dialog box, then close the sketch.

Mirror the holes:

a) b)

Click

Mirror Feature

on the Features toolbar, or click

Insert, Pattern/Mirror, Mirror Feature

Click the

Front

plane in the FeatureManager design tree.

Front

appears in the

Mirror plane

box.

Click the hole feature in either the FeatureManager design tree or in the graphics area.

Hole1

appears in the

Features to mirror

box.

Click

Save the part.

Creating a Layout Sketch for the Cuts

The layout sketch you create in this section divides the length of the hinge into five equal parts. Using equations and mirroring ensures that the five parts remain equal when you change the overall length of the hinge. You use this layout as a guide for making the cuts in the sections that follow.

Open a sketch on the large model face, and name it

layout for cuts

Click the lower edge of the sweep feature and click

Offset

Entities

a) b) c) d)

Set

Offset Distance

to 1mm.

Select the

Reverse

check box if necessary to offset

below the selected edge

Click to clear the

Select chain

check box.

Click

SolidWorks 2001 Getting Started 12-7

Working with Assemblies

Select the edges shown, then click

Convert

Entities

Click these edges

Click

Extend

in the Sketch Tools toolbar, or click

Tools, Sketch Tools, Extend

, then click the converted edges. Each vertical line is extended to meet the nearest sketch entity, in this case, the offset horizontal line.

Sketch a horizontal line to connect the two converted edges across the top.

Sketch two vertical lines as shown, and dimension them.

As you sketch the lines, be sure that you do not inference the geometry of the holes. Also, because the dimensions will be driven by an equation, the values of the dimensions do not matter at this time.

Add the equations:

a) b) c)

Click the FeatureManager tab , right-click the

Equations

folder , and select

Add Equation

Add equations that set each dimension to one-fifth of the dimension of the overall length.

"D2@layout for cuts" = "D1@Base-Extrude-Thin" / 5

"D3@layout for cuts" = "D1@Base-Extrude-Thin" / 5

Click

to close the

Equations

dialog box.

Sketch a vertical centerline across the midpoint of the part. Select the two vertical lines and the centerline, and click

Mirror

The sketch is complete and should be fully defined.

Close the sketch.

Save the part.

12-8

Chapter 12 Advanced Design Techniques

Cutting the Hinge (3Cuts)

Now you can reference the

layout for cuts

sketch to create the first set of cuts. Because each cut should be slightly wider than the corresponding tab on the other half of the hinge, you use offsets from the layout sketch entities.

Open a sketch on the large model face.

Click the bottom line in the layout sketch, and click

Convert Entities

. In the

Resolve Ambiguity

box, click

closed contour

, and click

. This copies the entire outside contour into the current sketch.

Click one of the vertical lines near the edge of the part, click

Offset

Entities

and do the following:

a) b) c)

Set

Offset Distance

to 1mm.

Select the

Reverse

check box if necessary to offset the line towards the middle of the part.

Make sure that

Select chain

is not selected, and click

Repeat for the vertical line near the opposite edge of the part.

Click one of the vertical lines near the center of the part, and offset the line by

1mm toward the outside of the part

(making the center cut wider). Repeat for the remaining vertical line.

Segments in current sketch

Click

Trim

, then trim the horizontal lines as indicated, leaving three closed rectangles.

Trim these segments

Click

Extruded Cut

Extrude

. Select

Through All

End

Condition

for both

Direction 1

and

Direction 2

Click

Rename the cut feature

Save the part.

3Cuts

SolidWorks 2001 Getting Started 12-9

Working with Assemblies

Cutting the Hinge (2Cuts)

Now you use the same methods to create the cuts for the other half of the hinge.

Roll back the design to the

3Cuts

feature by dragging the rollback bar to just below the

layout for cuts

sketch.

Rollback bar

Repeat Steps 1 and 2 from the previous section.

Click one of the vertical lines near the edge of the part, click

Offset Entities

, and do the following:

a) b) c)

Set the

Offset Distance

to 1mm.

Offset it towards the outside of the part.

Make sure that

Select chain

is not selected. and click

Segments in current sketch

Repeat for the vertical line near the opposite edge of the part.

Click one of the vertical lines near the center of the part, and offset it by 1mm toward the middle of the part. Repeat for the remaining vertical line.

Click

Trim

. the three segments at each end and the two segments in the middle, leaving two closed rectangles.

Extrude the cut as described in the previous section.

Rename this cut feature

2Cuts

Right-click the

layout for cuts

sketch, and select

Hide

Trim these segments

12-10

Chapter 12 Advanced Design Techniques

Creating the Part Configurations

Roll the design forward by dragging the rollback bar all the way to the bottom of the

FeatureManager design tree.

The part now has the entire barrel removed by the two cut features. This is the default configuration, which includes all the features. In this section, you make two more configurations of the part by suppressing selected features.

The OuterCuts configuration

Click the ConfigurationManager tab

ConfigurationManager view.

at the bottom of the window to change to the

Right-click the part name at the top of the ConfigurationManager tree, and select

Add

Configuration

Enter a

Configuration Name

, such as

OuterCuts

, in the box and click

Click the FeatureManager tab at the bottom of the window to switch back to the

FeatureManager view. Notice the configuration name beside the part name at the top of the tree:

Hinge (OuterCuts)

Click the

2Cuts

feature, then click

Suppress

on the Features toolbar, or click

Edit,

Suppress

The

2Cuts

feature is unavailable in the FeatureManager design tree, and is inactive in the current configuration.

The InnerCuts configuration

Repeat Steps 1 and 2 from the previous section.

Enter a

Configuration Name

, such as

InnerCuts

, in the box, then click

Switch back to the FeatureManager view. Notice the configuration name:

Hinge

(InnerCuts)

Click the

3Cuts

feature, then click

Suppress

. (Now both cuts are suppressed.)

Click the

2Cuts

feature, then click

Unsuppress

Edit, Unsuppress

The

3Cuts

feature is unavailable in the FeatureManager design tree, and the

2Cuts

feature is active in the current configuration.

Save the part.

SolidWorks 2001 Getting Started 12-11

Working with Assemblies

Inserting and Mating the Parts in an Assembly

Now you can begin creating the assembly.

Open a new assembly from the

Tutorial

tab and click

View, Origins

to show the origins.

Tile the windows, and drag the

Hinge

from the top of the FeatureManager design tree of the open part window into the assembly window. Inference the assembly origin while you place the component to align the planes of the assembly and the component.

Maximize the assembly window.

Right-click the component, and select

Component Properties

. Under

Referenced configuration

, notice that

Use named configuration

and

InnerCuts

are selected by default.

InnerCuts

is the active configuration name of the part added in Step 2. Click

to close the dialog box.

Hold down

Ctrl

, then drag the

Hinge

from either the graphics area or the FeatureManager design tree, and drop it beside the first one to create another instance.

Use

Move Component

and

Around Axis

to turn the second

Hinge

so that it faces the first one.

To change the named configuration, edit the component properties of the second

Hinge

. Click

Use named configuration

, select

OuterCuts

from the list, and click

Create a

Coincident

mate between the narrow front faces of the components. Create a

Concentric

mate between the cylindrical faces of the barrels.

Coincident mate

Concentric mate

12-12

Chapter 12 Advanced Design Techniques

You should be able to open and close the hinge assembly using

Move Component

Save the assembly as

Hinge.sldasm

Creating a New Part in the Assembly

Now you add the pin. The pin references the inner diameter of the barrel and the overall length of the hinge pieces. Once you reference an entity of one part (the barrel) to create an entity in another part (the pin), you create a reference in the context of the assembly. If you modify the referenced entity, the new entity updates to reflect that change.

Click

Insert, Component, New Part

. Select a new part from the

Tutorial

tab. Enter a name for the new component, such as

Pin.sldprt

, and click

Save

The pointer changes to .

Click the narrow model face on the front of the assembly. The new part will be positioned on this face, with its location fully defined by an

InPlace

mate.

A sketch is opened automatically on the selected face.

Notice that

Edit Part

in the Assembly toolbar is selected, and that the pin component is displayed in pink in the FeatureManager design tree.

Click the inner circular edge of the barrel, then offset it to the inside by 0.25mm.

Exit the sketch.

SolidWorks 2001 Getting Started 12-13

Working with Assemblies

In the FeatureManager design tree, expand the

pin

component, click the

Right

plane, and open a sketch. Click one of the long edges of the model, then click

Convert Entities

Exit the sketch.

Click

Sweep

. Use the circle (Sketch1) as the

Profile

and the line

(Sketch2) as the

Path

, and click

create the base feature of the pin.

Notice that the part you are editing is pink in the graphics area, and the status bar in the lower-right corner indicates that you are still editing the part.

Convert a long edge

12-14

Chapter 12 Advanced Design Techniques

Adding a Head to the Pin

Now reference the barrel of the hinge to create the head of the pin.

Open a sketch on the flat end of the pin, and sketch a circle anywhere.

Select the circle and the outer circular edge of the barrel, and add a

Coradial

relation.

Click

Extruded Boss/Base

End Condition

Blind

, set

Depth

to 3mm, and click

To add a dome to the head of the pin, click

Dome

on the Features toolbar, or click

Insert, Features, Dome

Click the flat face of the pin, set

Height

to 3mm. Observe the preview of the dome. Click

. This completes the pin.

Right-click in the graphics area, and select

Edit Assembly: Hinge

. Alternatively, you can click

Edit Part

on the Assembly toolbar to return to editing the assembly.

Save the assembly.

SolidWorks 2001 Getting Started 12-15

Working with Assemblies

Changing the Color of a Component

For easier viewing, you can change the color of assembly components.

Click one of the assembly components in either the

FeatureManager design tree or in the graphics area, then click

Edit Color

Choose a color from the palette, then click

Editing the Hinge Components

Now you can make this same hinge assembly in a different size.

In the FeatureManager design tree, expand the hinge component that uses the

InnerCuts

configuration. Double-click the

Base-Extrude-Thin

feature to display its dimensions.

Double-click any of the dimensions. The

Modify

dialog box appears.

Change the dimension value, and make sure that

All configurations

is selected.

Click to close the

Modify

dialog box.

If desired, repeat Steps 2 through 4 to change another value.

Click

Rebuild

or . All of the components in the assembly update automatically. (If you see a message indicating that the pin has rebuild errors, click

Rebuild

again.)

12-16

More about Assemblies

You can do much more with assemblies than what is shown in the examples of the

SolidWorks 2001 Getting Started. The following pages provide a brief introduction to this additional functionality. For more information, see the SolidWorks 2001 Online User’s

Guide.

SmartMates

In addition to the SmartMates you added in Chapter 11, “Assembly Mates,” you can add

other types of SmartMates. You can add feature-based mates between conical or cylindrical features. You can add a pattern-based mate to align two components using the circular patterns in the components.

Components to mate

Result of pattern-based mate

Working with Sub-assemblies

You can form a sub-assembly from components that are already in the assembly.

You can dissolve a sub-assembly into individual components, thereby moving the components into the parent assembly.

You can move components into or out of sub-assemblies.

More about Assemblies

Interference Detection, Collision Detection, and Dynamic Clearance

In a complex assembly, it may be difficult to visually determine whether components interfere with each other. In some cases, it becomes more difficult when you move components in the assembly. You can use the following tools to determine interference: q

Interference Detection. You can determine the interference between components and examine the resulting interference volumes.

Collision Detection. You can detect collisions with other components when moving or rotating a component.

Dynamic Clearance. You can dynamically detect the clearance between components when moving or rotating a component. As you move or rotate a component, a dimension appears indicating the minimum distance between the selected components.

Assembly Envelopes

You can select components based on their positions with respect to an assembly envelope.

An assembly envelope is a reference component, and it is ignored in global assembly operations (Bill of Materials, Mass Properties, and so on.) You can perform various editing operations (hide, suppress, copy, or delete) on components that are inside, outside, or crossing the assembly envelope.

Component Selection by Properties

You can select components for editing operations based on properties. Once you select those components that match the properties you specify, you can perform the desired editing operation, such as suppress, hide, or copy.

Component Patterns

You can define a pattern for placing components in an assembly in much the same way as you define a feature pattern in a part. You can also place a pattern of components in an assembly based on a feature pattern of an existing component. For example, you can insert a set of screws in a pattern of holes on a part.

Assembly Features

While in an assembly, you can create cut or hole features that exist in the assembly only.

You determine which of the assembly components you want the feature to affect. This is useful for creating cuts or holes that are added after the components are assembled.

Layout Sketches

You can design an assembly from the top-down using layout sketches. You can construct one or more sketches showing where each assembly component belongs. Then, you can create and modify the design before you create any parts. In addition, you can use the layout sketch to make changes in the assembly at any time.

Joining Parts

You can join two or more parts to create a new part. The join operation removes surfaces that intrude into each other’s space, and merges the part bodies into a single solid volume.

Weld Beads

You can add a variety of weld types to an assembly. The software prompts you for the weld type, the surface type, and the surfaces you want to weld together. When you create a weld, a weld symbol is automatically attached to the weld bead component in the assembly.

SolidWorks 2001 Getting Started

Working with Drawings and Detailing

Advanced Drawings and Detailing

Bill of Materials

More about Drawings and Detailing

SolidWorks 2001 Getting Started

Advanced Drawings and Detailing

Drawing Basics (Chapter 5) introduced the Standard 3 Views and Named Views. In this chapter, you learn about using SolidWorks software to create the following: q

Section View q

Detail View q

Ordinate Dimensions q

Annotations

Exploded View q

Notes

SolidWorks 2001 Getting Started 13-1

Working with Drawings and Detailing

Starting the Drawing with Named Views

Open a drawing and insert a

Named

view.

Open a new drawing from the

Tutorial

tab.

Right-click anywhere on the drawing sheet and select

Properties

The

Sheet Setup

dialog box appears.

Change

Scale

to 2:1, then click

Click

Named View

Right-click in the graphics area, and select

Insert From File

In the

Insert Component

dialog box, navigate to

connector.sldprt

in directory

\installation directory

\samples\tutorial\handle,

and click

Open

The

Named View

PropertyManager appears.

Click to place the view at the upper left of the drawing.

With the view selected, double-click to choose

*Right

from the

View Orientation

list.

NOTE:

You can change the view orientation at any time by selecting the view and choosing a different item from the

View Orientation

list.

Repeat steps 4 through 6. Place this view at the lower left of the drawing and select

*Isometric

from the

View

Orientation

list.

Click

Save

The

Save As

dialog box appears with

connector.slddrw

as the default name.

Type

Adv-Drawing

, then click

Save

If you see a message asking if you want to update any referenced models, click

Yes

13-2

Chapter 13 Advanced Drawings and Detailing

Adding a Section View

You add a

Section View

by cutting a view with a section line.

Double-click the view at the top left, or right-click the view and select

Activate View

Click

Centerline

the Sketch Tools toolbar, or click

Tools

Sketch Entity

Centerline

NOTE:

You can sketch the section line with either the

Centerline

tool or the

Line

tool. If you intend to use the

Line

tool, you can select the

Section View

tool first. The

Line

tool is activated automatically.

Hold the pointer over the center of the part until the pointer changes to indicating that the pointer is exactly on the temporary axis. Starting above or below the part, sketch a centerline vertically through the part.

With the section line still selected, click

Section View

on the Drawing toolbar, or click

Insert

Drawing View

Section

As you move the pointer, a preview of the view position is displayed. By default, the view is aligned in the direction of the cut.

Click the graphics area to place the view to the right of the original view.

Notice the arrows indicating the direction of the cut. You can doubleclick the section line, or select the

Change direction

check box in the

PropertyManager, to reverse the direction of the arrows, if necessary.

TIP:

If you reverse the direction of the section line arrows, the

Section

View

is marked with a crosshatch pattern. This crosshatch indicates that the view is out of date. Right-click the view and select

Update

View

to update the view only, or click

Rebuild

to rebuild the entire drawing.

SolidWorks 2001 Getting Started 13-3

Working with Drawings and Detailing

Adding a Detail View

Detail View

shows a portion of another view, usually at an enlarged scale.

To set the scale for detail views:

Click

Tools

Options

. On the

System Options

tab, click

Drawings

Make sure that

Detail view scaling

is 2X, then click

The Detail View is scaled relative to the drawing sheet scale, which appears in the lower right corner of the status line. The scale for this drawing sheet is 2:1. Because the

Detail View scaling is 2X, the Detail View is drawn at 4:1.

You sketch a profile to specify the area to be shown in the Detail

View. The profile can be any shape but it is usually a circle.

To create a detail view:

Double-click the

Activate View

Section View

, or right-click and select

Click

Circle

or click

Tools, Sketch Entity, Circle.

Sketch a circle on the

Section View

at the upper right.

With the circle still selected, click

Detail View

on the Drawing toolbar, or click

Insert, Drawing View, Detail

When you move the pointer, a preview of the view is displayed. The detail view is not aligned to any other view. You can move it freely to any location on the drawing sheet.

Click the graphic area to place the view.

The view letter and scale are displayed.

Click in the graphic area to close the PropertyManager.

Repeat steps 1 through 6, sketching a circle at the lower right corner of the connector shaft and placing the view at the lower right.

Select one of the profile circles in the

Section View

Increase and decrease the size of the circle by dragging the circumference. Drag the center of the circle to move the circle. Notice that the

Detail View

changes as the circle changes.

NOTE:

The view label letter increments automatically. To set the label letter for the next view, right-click the graphics area and select

Properties

Edit the text in

Next view label

To edit the current view label, select the Detail View circle. In the

Detail View

PropertyManager, you can edit the label text, change the text

Font

, select a circle

Style

, choose

View Options

, and set

Custom Scale

13-4

Chapter 13 Advanced Drawings and Detailing

Inserting Ordinate Dimensions

To insert ordinate dimensions:

Click

Dimension

, right-click in the graphics area and select

Ordinate Dimension

from the shortcut menu, or click

Tools, Dimensions, Ordinate

In the

Section View

, click the bottom horizontal line.

The first line you click becomes the zero position. Its label is 0. The other dimensions are calculated from this position.

Click again to place the ordinate.

Click the other horizontal lines in the view.

The leaders jog automatically to prevent overlapping text. You can drag the dimensions left and right as a group.

To modify the ordinate dimensions:

Click

Select

, then right-click the top dimension and select

Display Options, Jog

The dimension is selected, and handles appear on the leader.

Drag the dimension (not the handles) upwards.

The dimensions remain aligned vertically.

Right-click the second dimension (20) and select

Display Options, Jog

The check mark next to

Jog

is cleared and the jog in the leader is straightened.

To remove the chain arrows:

Right-click one of the dimensions in the ordinate group, and select

Properties

Clear the

Display as chain dimension

check box.

Click

To add other dimensions to the drawing:

Click

Dimension

then click the lines to be dimensioned.

Click to place the dimension.

NOTE:

The dimensions that you add to drawings are reference dimensions.

They are gray and appear in parentheses. You cannot edit the values.

However, the values of reference dimensions change when the model dimensions change.

SolidWorks 2001 Getting Started 13-5

Working with Drawings and Detailing

Adding Annotations

You can create several types of annotations in drawings.

You can specify a surface texture with a

Surface Finish Symbol

. You define a symbol that specifies the values and options for the finish you want, then attach it to an object.

Click

Surface Finish Symbol

on the Annotations toolbar, or click

Insert,

Annotations, Surface Finish Symbol

The

Surface Finish Symbol Properties

dialog box appears.

Notice the preview of the symbol as you set the following options:

•

Symbol

- select

Basic

from the list

•

Direction of lay

- select

Circular

from the list

•

Roughness, Maximum

- type 32

•

Leader

- select

Always show leaders

, click to clear the

Smart

check box, and select the filled round

Arrow style

from the list.

Click in the graphics area to place the leader on the isometric view, then click again to place the symbol.

You can place as many symbols as you wish without closing the dialog box.

Click

to close the

Surface Finish Symbol Properties

dialog box.

You can drag the symbol and leader to any location. To edit the symbol, double-click the symbol, or right-click and select

Properties

You can attach a

Datum Feature Symbol

to a surface that appears as an edge, and then add a

Geometric Tolerancing

symbol.

Click

Datum Feature Symbol

on the Annotations toolbar, or

Insert, Annotations, Datum Feature

Symbol.

The pointer changes to .

The

Properties

dialog box appears.

Click the bottom horizontal line in the section view, then drag the symbol into position and click to place it.

The datum letters are assigned alphabetically.

Click

to close the

Properties

dialog box.

Click

Geometric Tolerance

Annotations

Geometric Tolerance

Insert

The

Geometric Tolerance

dialog box appears.

Build the symbol as follows. As you add items, a preview of the resulting symbol is displayed in the preview box.

13-6

Chapter 13 Advanced Drawings and Detailing

•

In the first row of the

Feature control frames

section, click

GCS (Geometric

Characteristic Symbol)

. In the

Symbols

dialog box, under

Symbol library

, select

Perpendicularity

. Click

•

Enter a tolerance value of 0.005 in the

Tolerance 1

box.

•

Enter

in the

Primary

field.

Click on the centerline of the Section View to place the arrow, then click again to place the symbol.

You can place as many symbols as you wish without closing the dialog box.

Click

to close the

Geometric Tolerance

dialog box.

Click

Save

to save the drawing.

Drawing an Exploded View

On a new sheet, add an assembly, showing the assembly in an exploded configuration.

To add a new sheet to the drawing:

Click

Insert, Sheet

, or right-click the sheet tab at the bottom of the window, and select

Add Sheet

In the

Sheet Setup

dialog box:

•

Paper size

select

A-Landscape

•

Scale

- set to 1:2

•

Sheet Format

- select

None

Click

This drawing sheet is blank.

To add an exploded assembly:

Click

Named View

View, Named View

The

Named View

PropertyManager appears.

Open the file

Handle.sldasm

in directory

\installation directory

\samples\tutorial\handle.

Click the ConfigurationManager tab at the bottom of the window to change to the ConfigurationManager view.

Expand the

Default

configuration.

Right-click

ExplView1

and select

Explode

Click in the graphics area of the assembly to select the view.

Return to the drawing and select

Current

from the

View Orientation

list.

Click in the graphics area of the drawing to place the view.

SolidWorks 2001 Getting Started 13-7

Working with Drawings and Detailing

Adding Notes

A note can be free floating or placed with a leader. You can create multiple notes without closing the dialog box.

To start adding notes, without leader:

Click

Note

on the Annotation toolbar, or click

Insert, Annotations, Note

The

Note Properties

dialog box appears.

• Type a title, such as

Handle Assembly

, in the

Note text

box.

•

In the

Leader

section, select

No leaders

•

In the

Text justification

box, select

Center

from the list.

• In the

Font

section, click to clear the

Use document’s font

check box.

•

Click

Font

, select a

Font

, a

Font Style

, and a

Points

setting from the lists, and click

Click in the graphics area to place the note.

To add more notes, with leaders:

With the

Note Properties

dialog box still open, edit the text and select options for the next note.

•

Type a title, such as

connector

, in the

Note text

box.

• Select the

Always show leaders

check box.

•

Arrow style as Smart

•

In the

Text justification

box, select

Left

from the list.

•

In the

Font

section, select the

Use document’s font

check box.

Click in the graphics area to place the leader, and again to place the note.

Repeat steps 1 and 2 to place notes for all the assembly components.

Click

to close the

Note Properties

dialog box.

TIP:

To edit note text, double-click the note.

To edit properties of a note, right-click the note and select

Properties

You can also edit the text in the

Properties

dialog box.

Click

Save

to save the drawing.

13-8

Bill of Materials

In this chapter, you add a Bill of Materials (BOM) and balloons to a drawing of the universal joint assembly.

NOTE:

You must have the Microsoft® Excel 97 or later spreadsheet program installed on your computer to insert a bill of materials into a drawing.

This chapter demonstrates: q

Setting Drawing and Detailing Options q

Inserting a Bill of Materials q

Anchoring a Bill of Materials q

Moving a Bill of Materials q

Editing a Bill of Materials q

Annotating the drawing with Balloons q

Saving a Bill of Materials for use with other applications

SolidWorks 2001 Getting Started 14-1

Working with Drawings and Detailing

Starting a Drawing

The universal joint assembly that you created in the “Assembly Mates” chapter is the basis for working with the bill of materials in this chapter.

Open

u-joint.sldasm

in directory \install_dir

\samples\tutorial\universal_joint

Open a new drawing from the

Tutorial

tab.

Right-click anywhere on the drawing sheet and select

Properties

. Set

Scale

to 1:2, then click

Insert a

Named View

of the isometric view of the

U-joint.sldasm

assembly.

Save the drawing as

U-joint.slddrw

Drawing and Detailing Options

Click

Tools, Options

. On the

System Options

tab, click

Drawings

Make sure that the

Automatic update of BOM

check box is selected.

If this check box is not selected, you must delete and re-insert a BOM to update it.

Changes that affect a BOM include adding, deleting, or replacing components, changing component names or custom properties, and so on.

On the

Document Properties

tab, under

Detailing

, click

Balloons

In the

Single balloons

section, in the

Style

box, select

Circular Split Line

from the list.

In the

Balloon text

section, the

Upper

box is

Item Number

, and the

Lower

box is

Quantity

Click

Detailing, Annotations Display

Make sure that

Display all types

is selected.

Click

to close the

Options

dialog box.

14-2

Chapter 14 Bill of Materials

Inserting a Bill of Materials

Because a drawing can contain views of different parts and assemblies, you must pre-select the view for which you want to create a bill of materials.

Select the drawing view.

Click

Insert, Bill of Materials

The

Select BOM Template

dialog box appears.

Click

Open

to use the default bill of materials template,

Bomtemp.xls

The

Bill of Materials Properties

dialog box appears.

Set the following items:

• Click to clear the

Use the document’s note font when creating the table

check box. The table uses the font in the template.

• Select

Show assemblies and parts in an indented list

. Both the subassembly and its components appear in the bill of materials. The other choices are:

Show parts only

- parts and sub-assembly components are listed, but not the subassemblies

Show top level subassemblies and parts only

- the parts and subassemblies are listed, but not the subassembly components

• In the

Anchor Point

section, make sure that the following are selected:

Use table anchor point

check box

Top Left

from the

Anchor point coincident to

list

Click

to close the

Bill of Materials Properties

dialog box.

A bill of materials is displayed. It lists the parts and subassembly in the universal joint assembly.

SolidWorks 2001 Getting Started 14-3

Working with Drawings and Detailing

Anchoring a Bill of Materials

An anchor point is a point in the sheet format which you can set and to which you anchor a bill of materials. In the bill of materials, you can select the corner of the bill of materials to be coincident with the anchor point.

Right-click the BOM, and select

Anchor, Top Right

The BOM moves so that the top-right corner coincides with the anchor.

In the FeatureManager design tree, expand the

Sheet Format1

icon

Right-click the

Bill of Materials Anchor1

icon , and select

Set Anchor

Click the top left corner of the inside border of the drawing sheet format, to set the anchor.

The anchor point is highlighted. You are in the

Edit Sheet Format

mode.

Right-click the graphics area, and select

Edit Sheet

The BOM is anchored at the inside border.

Right-click the BOM, and select

Anchor, Top Left

Moving a Bill of Materials

You can unlock the BOM from the anchor point and then move it to a new location.

Right-click the bill of materials and select

Anchor, Unlock from Anchor

Move the pointer over the bill of materials.

The pointer changes to the move shape .

Drag the table to a new location.

Right-click the bill of materials and select

Anchor, Lock to Anchor

The bill of materials returns to the anchor.

14-4

Chapter 14 Bill of Materials

Editing a Bill of Materials

Next, enter descriptions for the items.

Right-click the bill of materials and select

Edit Bill of Materials

, or double-click the bill of materials.

While the bill of materials is active, it is displayed with shaded borders and row and column headers. Excel toolbars replace the SolidWorks toolbars.

To see all the rows, drag the lower-right corner of the border and resize the table.

You can also resize the columns and rows as in any Excel worksheet.

Click in cell

, type a description, then press

Enter

Continue to add descriptions.

a) b) c)

You can also resize the text, change the font, and so on.

Select the text

Set the font size to 16 points

Click

Format, Row, AutoFit

and

Format, Column, AutoFit Selection

to adjust the column and row sizes.

Click outside the bill of materials to close it.

SolidWorks 2001 Getting Started 14-5

Working with Drawings and Detailing

Inserting Balloons

Balloon callouts label the parts in an assembly drawing and relate them to item numbers on the bill of materials.

Click

Balloon

on the Annotations toolbar, or click

Insert, Annotations

Balloon

Click a component in the drawing view.

A balloon attaches to the component. The numbers correspond to the item numbers

(upper) and quantities (lower) in the bill of materials.

Click

Select

or press

Esc

to turn off the balloon tool.

To move the balloon or leader arrow, select and drag the balloon, or drag the leader by the handle.

Saving a Bill of Materials

You can save the bill of materials as an Excel file for use with other applications.

Select the bill of materials.

Click

File, Save As

The

Save Bill of Materials Table

dialog box is displayed. Notice that the

Save as type

is set to

Excel Files (*.xls)

by default.

Type

Ujoint_BOM

File name

box and click

Save

The extension

.xls

is added to the filename, and the file is saved to the current directory. If you wish, you can navigate to a different directory, then save the file.

NOTE:

The Excel file is not linked to the bill of materials in the drawing. If assembly components change, the bill of materials automatically updates, but the Excel file does not.

For more information about adding a bill of materials, see bill of materials in the

SolidWorks 2001 Online User’s Guide.

14-6

More about Drawings and Detailing

You can do much more with drawings than what is introduced in the examples in this guide. The following pages highlight additional SolidWorks functionality in drawings and detailing. For more information, see the SolidWorks 2001 Online User’s Guide.

Drawings

In drawings, you have many options, formats, and views to consider.

Options for Drawings

The

Options

dialog box on the

Tools

menu contains many options for controlling aspects of drawings. In addition to the default sheet scale and detail view scaling, you can specify the type of projection, detail item snapping, default edge display, and many types of automatic placement, display, and updates.

Templates and Drawing Sheet Formats

When opening a new drawing, you can choose from standard templates, custom templates, or a blank template. You can add customized templates for drawings to the

SolidWorks system, and you can add tabs to the

New SolidWorks Document

dialog box.

When adding a sheet to a drawing, you select a sheet size and format. You can customize a sheet format (to match your company’s standard, for example), including text content and font, bill of materials anchor point, and bitmaps of your company logo. Then you can save the sheet format for future use.

You can modify the current drawing sheet, including such properties as sheet name, paper size, sheet scale, sheet format, type of projection, and the next view label. Sheet properties such as name, size, number, and scale have system-defined names that you can link to note text in the sheet format.

More about Drawings and Detailing

Views

The chapters on drawings in this guide introduced the

Standard 3 View, Named View, Section View, and Detail

View. Other possible views include the following:

•

Projection

- a projection of an orthogonal view

•

Auxiliary

- a projection unfolded normal to a reference edge in an existing view. You can select an edge, a silhouette edge, an axis, or a sketched line as the reference edge. You can toggle the view orientation while dragging the view and after placing the view.

Projection view

Broken view

•

Broken

- an interruption of a long part that has a uniform cross-section

•

Relative to Model

- an orthographic view defined by two orthogonal faces or planes in the model

•

Aligned Section

- a section view aligned to a sketched section line

•

Section View of Assembly

- similar to a section view of a part, but with the option of excluding components from being sectioned

Aligned section view

•

Crop

- crops the view outside a closed profile such as a circle. You can crop any view except a

Detail View.

Crop view

•

Detail

- The profile for a Detail View can be any closed sketch. You can choose to display either the profile or its circle in the parent view. If you select

Circle

, you can choose a style for the detail note. You can drag the note anywhere except inside the circle.

Detail profile, detail circle, note style with leader, and detail view

Other aspects of drawing views that you can control include:

• Editing View Properties, including scale, orientation, configuration, exploded state, and type of dimensions (projected or isometric).

•

Turning off the automatic view update mode option so that performance is faster, then manually updating individual views, or all views at once, as necessary.

•

Breaking the alignment of views that are automatically aligned. You can also align one drawing view with another.

• Rotating a drawing view around an edge or around its center point. You can copy and paste views, hide or show a view, and change the display mode of a view.

Show/Hide

You can show or hide views, components, and hidden edges in components.

• When you hide or show a view that has related views

(

Auxiliary

Detail

, and so on), you are given the option of hiding or showing those related views also.

•

In addition to hiding or showing components individually, you can hide as many components as you wish on the

Hide/

Show Components

tab in the

Drawing View Properties

box.

Hide Behind Plane

is a quick method of hiding a number of components. The hidden components are listed on the

Hide/Show Components

tab.

•

Show Hidden Edges

is available for individual components from the shortcut menu when the view is in Hidden Lines

Removed mode. Any number of components can be specified on the

Show Hidden Edges

tab in the

Drawing

View Properties

dialog box.

Complete assembly

Hide Component

Layers

Hide Behind Plane

Layers in drawings assign line color, thickness, and style for entities in the layers. You can hide or show individual layers. New entities are automatically added to the active layer.

You can add dimensions, annotations, and sketch entities to layers. You can add components to layers, in both part and assembly drawings. Many dialog boxes

(

Component Display Properties

Note Properties

Geometric Tolerance Properties

, and so on) include a

Layer

list for selecting a named layer for the entity.

Layer information is included when importing or exporting files in

.dxf

.dwg

format.

2D Sketching

Sketch tools and sketch relations work the same way in a drawing document as they do in a part or assembly document.

SolidWorks 2001 Getting Started

More about Drawings and Detailing

RapidDraft Drawings

RapidDraft™ drawings have a format designed so you can open and work in drawing files without the model files being loaded into memory.

•

When you open a new drawing document, a

Create RapidDraft Drawing

check box appears in the

New SolidWorks Document

dialog box.

•

When you open an existing drawing that is not a RapidDraft drawing, a

Convert to

RapidDraft

check box appears.

•

Once a drawing is converted to RapidDraft format, it cannot be converted back.

When you convert a drawing to RapidDraft, the drawing and model are both loaded into memory. When the conversion is complete, save the drawing. Close the drawing, which also closes the model, then open the drawing again. The drawing is now in RapidDraft mode.

•

View borders in RapidDraft drawings are blue.

•

If a part or assembly is needed for an operation in a RapidDraft drawing, you are prompted to load the model file. You can also load the model manually by rightclicking a view and selecting

Load Model

•

Some changes, such as changes to a section line or detail profile, require a view update. When a drawing view requires an update, the view is displayed with a gray crosshatch pattern.

You can send RapidDraft drawings to other SolidWorks users without sending the model files. Other advantages include the following:

•

Some engineers can work on the model while others add details and annotations to the drawing. When the drawing and model are synchronized, all the details and dimensions added to the drawing update to any geometric or topological changes in the model.

•

The time required to open a drawing in RapidDraft format is significantly reduced because the model files are not loaded into memory. More memory is available to process drawing data.

•

The RapidDraft format requires storing less surface data but more edge data. File size is directly related to the number of visible edges in the drawing.

Operations available in RapidDraft drawings when the model is not loaded include:

•

Saving and opening drawings

•

Adding dimensions, annotations, balloons, and empty views

•

Changing scales, line formats, and view alignments

•

Selecting edges, planes, sketches, origins, and axes

•

Updating the drawing

Detailing

You can include items such as dimensions, notes, and symbols in part and assembly documents, and then import these dimensions and annotations from the model into a drawing. Once in the drawing, you can add other annotations and reference dimensions.

Options for Detailing

The

Options

dialog box on the

Tools

menu includes detailing options for setting the dimensioning standard, whether to show trailing zeros, details of center marks, witness lines, center lines, and fonts. You can control details of dimensions, notes, balloons, arrows, and virtual sharps.

Dimensions in Drawings

You can import dimensions from the model into all the drawing views at once, or into selected drawing views. The dimensions are imported only once for a part. In the drawing, you can add parallel, horizontal, and vertical reference dimensions in the same way as in model sketches. Silhouette edges and midpoints of linear edges are available for dimensioning.

Either an edge or a vertex can be the baseline for dimensions.

You can align dimensions in either a linear or radial direction, and you can distribute parallel and concentric dimensions so they are spaced uniformly. You can center dimension text between witness lines and offset dimension text from its arrows.

Vertex as baseline

Depending on the type of dimension (linear, radius, reference, driving), you can also modify the following properties: driven, read only, dual dimension, arc condition, foreshortened radius, inside or outside arc, ordinate dimension as chain, and as inspection dimension.

Concentric alignment

Some of the dimension properties you can modify are: value, name, arrow style and placement, font, precision, witness lines, tolerance, units, and leader style. Many dimension properties are available in the PropertyManager.

Many display options are available on the dimension shortcut menu. Depending on the type of dimension selected, the

Display Options

menu includes items for slanting witness lines, centering or offsetting text, showing parentheses, showing as an inspection dimension, jogging or re-jogging ordinate, aligning ordinate, and adding to ordinate dimensions.

Leader options

SolidWorks 2001 Getting Started

More about Drawings and Detailing

Dimension arrows have circular handles. When you click a handle, the arrows flip outside or inside. When you right-click a handle, a menu of arrowhead styles appears for changing the style of the dimension arrowhead individually.

Annotations

You can add many types of annotations to drawings. Functionality includes:

• Multiple annotations and multiple leaders

• Alignment tools, snap to grid, and inferencing for alignment

• Double-click to edit in place

• Link notes to document properties and embed hyperlinks in notes

Flip arrows with dimension handles

In addition to the surface finish symbol, geometric tolerancing symbols, bill of materials, and balloons discussed in the “Advanced Drawings and Detailing” and “Bill of Materials” chapters, you can insert the following types of annotations into drawings:

•

Center Marks

- to silhouette edges as well as circles and arcs

•

Hole Callouts

- dimensions update if the model changes

•

Datum Targets

- with targets as points, circles, or rectangles

•

Weld Symbols

- including secondary weld fillets

•

Area Hatch

- on faces or in closed profiles

•

Cosmetic Threads

- including conical threads

•

Stacked Balloons

- with one leader for the set

Center mark

Hole callout

Datum target

Area hatch Weld symbol

Stacked balloons

Properties of a bill of materials available for editing include the configurations specified at the time of creation, which items to include in the table, how row numbers are assigned, and split tables. You can edit and format the text, specify how to list component configurations, add custom columns, and edit the item number in a balloon.

SolidWorks 2001 Getting Started

Special Topics

Sheet Metal Part

Mold Design

3D Sketching

Importing Files / Using FeatureWorks Software

Learning to Use PhotoWorks

SolidWorks Animator

More about SolidWorks Functionality

Sheet Metal Part

In this chapter, you create the sheet metal part shown here. This chapter demonstrates: q

Creating a base flange q

Adding a miter flange q

Mirroring the part and creating new bends q

Adding and bending a tab q

Folding and unfolding a single bend as well as the entire part q

Adding a cut across a bend q

Creating a sheet metal drawing

For more information about SolidWorks sheet metal functions, see the SolidWorks 2001

Online User’s Guide.

SolidWorks 2001 Getting Started 15-1

Special Topics

Creating the Base Flange

When developing a sheet metal part, you generally design the part in the folded state. This allows you to capture the design intent and the dimensions of the finished part.

To create a sheet metal part of uniform thickness, sketch an open profile and use the base

flange feature to create the thin feature and the bends.

Open a new part from the

Tutorial

tab and open a sketch on the

Front

plane.

Placing the lower left corner of the sketch on the origin, sketch and dimension the profile as shown. Add an

Equal

relation between the two vertical lines.

Click

Base-Flange/Tab

on the Sheet Metal toolbar, or click

Insert

Features

Sheet Metal

Base Flange

NOTE:

If the Sheet Metal toolbar is not visible, click

View

Toolbars

Sheet Metal

The

Base Flange

PropertyManager appears.

Under

Direction1

, leave

End Condition

Blind

and set the

Depth

to 75mm.

Under

Sheet Metal Parameters

, do the following:

a) b)

Set

Thickness

to 3mm.

Set

Bend Radius

to 1mm. This is the default bend radius.

Click

The sketch is extruded and the bends are automatically added.

Examining the FeatureManager Design Tree

A base flange feature creates three new features in the FeatureManager design tree. The following are the three new features:

Sheet-Metal1

. The Sheet-Metal feature contains the default bend parameters. To edit the default bend radius, bend allowance, or default relief type, right-click the Sheet-

Metal feature and select

Edit Definition

Base-Flange

. The Base-Flange feature is the first solid feature of this sheet metal part.

Flat-Pattern1

. The Flat-Pattern feature flattens the sheet metal part. Notice it is suppressed by default as the part is in its bent state. Unsuppress the feature to flatten the sheet metal part.

When the Flat-Pattern feature is suppressed, all new features that you add to the part are automatically inserted above the Flat-Pattern feature in the FeatureManager design tree. When the Flat-Pattern feature is unsuppressed, new features go below it in the

FeatureManager design tree and are not shown in the folded part.

15-2

Chapter 15 Sheet Metal Part

Adding a Miter Flange

You can add flanges to your sheet metal part with corners that are automatically mitered.

Select the inside vertical edge approximately as shown and click

Sketch

to open a new sketch.

Vertex

A sketch plane is created normal to the selected edge with its origin at the closest endpoint of the edge.

Sketch a horizontal line starting from the inside vertex shown extending towards the middle of the part.

Dimension the line to 8mm.

Click

Miter Flange

on the Sheet Metal toolbar, or click

Insert

Features

Sheet Metal

Miter Flange

Edge

The

Miter Flange

PropertyManager appears.

Click the handle that appears on the selected edge.

The five tangent edges appear in the

Along edges

box under

Miter Parameters

Also, a preview of the miter flange appears on the model.

Click

The flange is added to the selected edges. Notice the bend reliefs are automatically added to allow the miter flanges to fold and unfold.

Save the part as

Cover.sldprt

Mirroring the Sheet Metal Bends

When you mirror a sheet metal part, many of the bends are mirrored as well. The only bends that are not mirrored are those that are normal to and coincident to the mirror plane; those bends are extended.

Click

Hidden in Gray

Click

Insert

Pattern/Mirror

Mirror All

The

Mirror All

dialog box appears.

Select one of the back planar faces as the

Mirror Plane

Use

Select Other

from the shortcut menu if necessary.

SolidWorks 2001 Getting Started 15-3

Special Topics

Click

and click

Shaded

The entire part is mirrored as well as the sheet metal bends from the miter flange.

Expand the

Mirror1

feature in the FeatureManager design tree and notice that there are new bends to include the mirrored geometry.

Adding a Tab

Open a sketch on the vertical face shown.

Sketch a rectangle above the sheet metal body with its lower edge coincident to the edge shown.

Dimension the rectangle to 50mm high and

100mm wide.

Add a coincident relation between the midpoint of one of the horizontal lines of the rectangle and the

Front

plane.

Edge

TIP:

To select the midpoint of a line or edge, right-click the line or edge and click

Select Midpoint

The sketch should look like this when you are done.

Click

Base-Flange/Tab

The tab is added to the part. You do not need to specify a depth because the SolidWorks software links the thickness of the tab to the thickness of the base flange.

Face

15-4

Chapter 15 Sheet Metal Part

Bending the Tab

Once you add a tab, you must specify how to bend it.

Select the same vertical face from the previous section and open a sketch.

Sketch a horizontal line of any length. Dimension it to 30mm below the top of the tab as shown.

The bend line for a Sketched Bend does not have to be the exact length of the faces you are bending.

Click

Sketched Bend

on the Sheet Metal toolbar, or click

Insert

Features

Sheet Metal

Sketch Bend

The

Sketched Bend

PropertyManager appears.

Under

Bend Parameters

, do the following:

• Select the vertical face that you are sketching on as the

Fixed face

• Set

Bend position

Bend outside

• Make sure

Bend Angle

is set to 90° and the

Use default radius

check box is selected.

Click

Save the part.

Adding a Cut Across a Bend

To cut across a bend, you start by unfolding only the bend that you want to cut across.

Click

Unfold

on the Sheet Metal toolbar, or click

Insert

Features

Sheet Metal

Unfold

The

Unfold

PropertyManager appears.

Select the face shown as the

Fixed face

and the bend shown as the

Bends to unfold

Notice that you can only select bends when the

Bends to unfold

box is active.

Face

Bend

SolidWorks 2001 Getting Started 15-5

Special Topics

Click

The selected bend only is unfolded.

Next, you create a sketch and cut through the bend.

Open a sketch on the face shown, and sketch and dimension a rectangle as shown. The 60mm dimension goes from the left edge of the rectangle to the origin.

Click

Extruded Cut

or . Select

Through All

End Condition

, then click

The cut goes through the bend region.

15-6

Now that you made your cut, fold the bend back to its bent state.

Click

Fold

on the Sheet Metal toolbar, or click

Insert

Features

Sheet Metal

Fold

The

Fold

PropertyManager appears.

Select the bottom face of the sheet metal part as the

Fixed face

Click

Collect All Bends

to collect all the unfolded bends.

The unfolded bend appears in the

Bends to fold

box.

Click

The part returns to its fully bent state with the cut across the bends.

Chapter 15 Sheet Metal Part

Folding and Unfolding the Entire Part

You can flatten all the bends of your sheet metal part at once.

Select the

Flat-Pattern1

feature in the

FeatureManager design tree and click

Flattened

on the Sheet Metal toolbar.

The flattened sheet metal part appears with all of the bend lines shown.

To fold the part back up, select the

Flat-Pattern1

feature again and click

Flattened

again.

Save the part.

Creating a Sheet Metal Drawing

Now create a drawing of the cover. Start with a view of the folded model, and then add a view of the unfolded model.

Open a new drawing from the

Tutorial

tab.

Click

Named View

, or click

Insert

Drawing View

Named View

The

Named View

PropertyManager appears.

The pointer indicates that you may select a model to display in the drawing.

Tile the windows so you can see the cover and the drawing

Click anywhere in the

Cover.sldprt

window.

The pointer indicates that you may select a location in the drawing to place the named view.

Click where you want to place the view in the drawing.

The

Named View

PropertyManager appears. Note its similarity to the

Orientation

dialog box.

Select

*Isometric

from the list to switch to an isometric view.

Maximize the drawing window.

SolidWorks 2001 Getting Started 15-7

Special Topics

Next, add the view of the unfolded model. A flat pattern view is automatically added when you create a sheet metal part.

Click

Named View

again.

Select the isometric view as the model you want to use.

Click where you want to place the view in the drawing.

In the

Named View

PropertyManager, do the following:

a) b)

Select

Flat pattern

from the

View Orientation

list.

Select the

Custom Scale

check box and set the scale to 1:3.

Click in the graphics area to see the changes take effect.

Save the drawing as

Cover.slddrw

15-8

Mold Design

In this chapter, you create a design part, then you develop a mold from which the part can be formed. This chapter discusses the following topics: q

Linking dimension values q

Creating an interim assembly from a design part and a mold base part q

Editing in context by inserting a cavity q

Deriving component parts q

Understanding external references

SolidWorks 2001 Getting Started 16-1

Special Topics

Creating the Design Part

The first step is to create the part for which you want to make a mold. You create it as a solid model, just as you do any other part.

Open a new part from the

Tutorial

tab and open a sketch.

Sketch a horizontal centerline through the origin.

Click

Mirror

or ,

Sketch Tools

Mirror

Sketch a sloping line on one side of the centerline as shown.

Click

Mirror

again to turn mirroring off.

Click

Tangent Arc

Tools, Sketch

Entity, Tangent Arc.

Sketch and dimension the two arcs as shown. To dimension the distance between the arcs, select anywhere on the arcs.

Click

Extruded Boss/Base

or ,

Base

Extrude

In the

Base-Extrude

PropertyManager, under

Direction 1

•

Set

End Condition

Mid Plane

and

Depth

to 60mm.

•

Click

Draft On/Off

, and set

Angle

to 10°.

•

Click to clear the

Draft Outward

check box, if necessary.

Click

16-2

Chapter 16 Mold Design

Adding Bosses

Open a new sketch on the front face of the part, and click

Normal To

Sketch two circles approximately as shown.

Add a coradial relation to align the center points of the large circle and the large arc, making them the same size:

a) b) c) d)

Click

Add Relation

Tools

Relations

Add.

Select the circle and the inside edge of the larger arc (the drafted edge).

Select

Coradial

Click

Apply

Add a coradial relation between the smaller circle and arc, then close the

Add Geometric

Relations

dialog box.

Coradial relation

Click

Extruded Boss/Base

, and do the following:

• Set

End Condition

Blind

with a

Depth

of 20mm.

• Click

Draft On/Off

Angle

to 30°.

• Click to clear the

Draft Outward

check box, if necessary.

Click

SolidWorks 2001 Getting Started 16-3

Special Topics

Linking Dimension Values

You can make the draft angles of the boss and the base equal by linking the dimension values. Then, if you change the value of either draft angle, the other draft angle updates accordingly.

In the FeatureManager design tree, right-click the

Annotations

folder , and select

Show Feature

Dimensions

Right-click the dimension of the draft angle of the base

(10°), and select

Link Values

Type

draft

in the

Name

box, then click

Right-click the dimension of the draft angle of the boss

(30°), and select

Link Values

Click the arrow beside the

Name

box, select

draft

from the list, and click

Each time you create a new

Name

variable, it is added to this list.

Click

Tools, Options

. On the

System Options

tab, click

General

Select the

Show dimension names

check box, then click

. Notice that the draft angles have the same name.

Click

Rebuild

or . The part rebuilds with the boss extrusion at the same draft angle as the base.

Double-click the draft angle of either the base or boss, and change it to 5°.

Click

Rebuild

. The draft angle changes on both the base and the boss.

To turn off the visibility of the dimensions, right-click the

Annotations

folder , and deselect

Show Feature

Dimensions

Save this part as

Widget.sldprt.

16-4

Chapter 16 Mold Design

Rounding the Edges

Click

Fillet

Fillet/Round

Select the two faces and three edges shown.

Set the

Radius

5mm.

Select the

Tangent propagation

check box.

Select these faces

Select these edges

Click

Save the part.

Creating the Mold Base

The next step is to create the mold base part, a solid block large enough to accommodate the design part (the part to be molded).

Open a new part from the

Tutorial

tab and open a sketch.

Sketch a rectangle starting at the origin and dimension it to 300mm by 200mm.

Click

Extruded Boss/Base

or ,

Base

Extrude

. Extrude the rectangle with

End Condition

Blind

and

Depth

of 200mm.

Save the part as

Box.sldprt

SolidWorks 2001 Getting Started 16-5

Special Topics

Creating an Interim Assembly

This section describes how to create an interim assembly, bringing together the design part and the mold base.

Open a new assembly from the

Tutorial

tab and click

View, Origins

to show the origins.

Tile the windows. (Click

Window, Tile Horizontally

Tile Vertically

There should be three windows open:

Widget.sldprt

Box.sldprt

, and

Assem1

. (Close any other windows.)

In the

Box.sldprt

window, click on the part name

Box

in the FeatureManager design tree, drag it into the

Assem1

window, and drop it on the origin in the graphics area.

Watch for the pointer. The planes of the box are aligned to the planes of the assembly, and the component is fixed in place.

Drag the widget from the graphics area of the

Widget.sldprt

window, and drop it in the assembly window beside the box in the graphics area.

Maximize the assembly window, and change the view orientation to

Isometric

In the FeatureManager design tree, click the beside each component to expand the view of the features.

Centering the Design Part in the Mold Base

Now you need to position the design part to center it within the mold base. You can place the widget roughly where you want it by dragging. Position the part more precisely by using distance mates between the planes of the components.

To see the widget inside the box, use

Hidden In Gray

Wireframe

display mode. Or, you can make the box transparent to see the widget inside, even in

Shaded

mode.

Right-click the

Box

component in the FeatureManager design tree, and select

Component Properties

. Click

Color

, then click

Advanced

In the

Advanced Properties

dialog box, drag the slider for

Transparency

to the right, a little less than halfway. Click

to close each of the dialog boxes.

16-6

Chapter 16 Mold Design

Click

Move Component

, and click the widget component in the graphics area. Drag the widget into the box. Notice how you can see through the box. Change the view orientation, and continue to move the widget until it is roughly in the center of the box.

Click

Mate

or ,

Mate

The

Mate

PropertyManager appears.

Click the FeatureManager tab to access the flyout FeatureManager design tree.

Click the

Front

plane of the

Box

and the

Front

plane of the

Widget

. Click

Distance

, specify 100mm, and click Preview.

Click

Rotate View

, and rotate the assembly to check the position of the widget. If necessary, click to clear the

Flip dimension

check box, and click

Preview

again.

Click the pushpin in the

Mate

PropertyManager to keep it in place for the next few steps.

Click

Add another distance mate, this time between the

Top

plane of the

Box

and the

Top

plane of the

Widget

. Specify a distance of 100mm, click

Preview

, and click to clear the

Flip dimension

check box if necessary.

Repeat for the

Right

plane of the components, with a distance of 150mm.

The widget should be centered in the box.

Close the

Mate

PropertyManager.

Save the assembly as

Mold.sldasm

Creating the Cavity

In this section, you edit the mold base component

Box

in the context of the assembly. You change the box from a solid block to a block with a cavity in the middle, shaped like the design component

Widget

Click

Hidden in Gray

Click the

Box

component in the FeatureManager design tree or the graphics area, and click

Edit Part

on the Assembly toolbar.

The

Box

component changes to pink in the graphics area and in the FeatureManager design tree. The status bar in the lower-right corner displays “Editing Part.”

NOTE:

It is important to be aware that you are editing the part, not the assembly, because the changes you make are reflected in the original part document,

Box.sldprt

SolidWorks 2001 Getting Started 16-7

Special Topics

Click

Cavity

on the Mold Tools toolbar, or click

Insert, Features, Cavity

The

Cavity

dialog box appears.

Select

Widget

in the FeatureManager design tree.

The name of the part appears in the

Design component

box.

Set

Type

Component Centroids

Scaling Factor in %

to 2, and make sure the

Uniform

check box is selected.

These settings control how the cavity is enlarged to compensate for material shrinkage.

Click

to create a cavity in the shape of the

Widget

part.

Return to assembly editing mode by clicking

Edit Part

Save the assembly.

Listing External References

Examine the FeatureManager design tree. The

(f)Box<1> ->

component contains a

Cavity1 ->

feature. The

arrow indicates an external reference. This occurs when you reference one part (or feature) to create a feature in another part. The new feature is dependent on the referenced feature of the other part.

A cavity has an external reference to the design part on which it is based. Therefore, if you modify

Widget

, the

Cavity1

feature of

Box

updates to reflect that change. Notice the

Update Cavity1 in Box

feature at the bottom of the design tree.

To list the external references, right-click the part or feature with the arrow, and select

List External Refs

External References

NOTE:

External references update automatically only if all of the documents involved are open when a change is made. Otherwise, the references are considered to be out-of-context. To update out-of-context references, you must open and rebuild the document where the reference was created (in this example, the mold assembly).

16-8

Chapter 16 Mold Design

Cutting the Mold

The last step is to cut the box in half to make the pieces of the mold. You derive the parts of the mold from the edited

Box

component.

Select the

Box

component, either in the graphics area or the FeatureManager design tree, and click

File

Derive Component Part

A part window appears for the derived part. A derived part always has another part as its first feature. The first feature has an arrow

after the name, because it has an external reference to the part from which you derived it. You can list the external references as described in the previous section.

Click

Isometric

, then click either

Hidden in Gray

Wireframe

to see the cavity inside the box.

Select the narrow face of the box closest to you, and open a new sketch.

Select this edge

Select the edge of the cavity closest to the end of the box.

This edge is on the plane where you want to separate the mold.

Click

Convert Entities

Tools

Sketch

Tools

Convert Entities

to project the edge onto the sketch plane.

Click the line and drag each endpoint so that the line is wider than the box.

Select this face

Click

Extruded Cut

or ,

Cut

Extrude

. In the

Cut-Extrude

PropertyManager:

•

Make sure

End Condition

is set to

Through

All

• Leave the

Flip side to cut

check box cleared.

Notice the direction of the arrow in the graphics area. It points to the side where the material will be removed.

SolidWorks 2001 Getting Started 16-9

Special Topics

Click

OK .

Click

Shaded

, and rotate the part to see the cavity.

Save this half of the mold as

Top_mold.sldprt

To create the other half of the mold, return to the

Mold

assembly window and repeat Steps 1 through 7.

Reverse the direction of the cut by selecting the

Flip side to cut

check box in the

Cut-Extrude

PropertyManager.

Save this half of the mold as

Bottom_mold.sldprt

16-10

3D Sketching

Using SolidWorks 2001, you can create 3D sketches. You can use a 3D sketch as a sweep path, as a guide curve for a loft or sweep, a centerline for a loft, or as one of the key entities in a piping system. (For more information about the SolidWorks Piping add-in, see the SolidWorks 2001 Online User’s Guide.)

This chapter introduces you to 3D sketching and describes the following concepts: q

Sketching relative to coordinate systems q

Using the space handle q

Dimensioning in 3D space q

Relations available in 3D sketching

SolidWorks 2001 Getting Started 17-1

Special Topics

3D Sketching

To begin a 3D sketch, click

3DSketch

on the Sketch toolbar, or click

Insert, 3D

Sketch

. The sketch tools that are available in 3D sketching are

Line

Centerline

Fillet

Chamfer

Point

Spline

Convert Entities

Intersection Curve

Face Curves

Trim,

Extend

, and

Construction Geometry

3D sketching consists of lines and arcs in series. You use

Line

for sketched lines, and use

Fillet

to round the intersections of sketched lines. To create an arc, select the

Fillet

tool and click two intersecting line segments, or click their common point.

You can use

Centerline Point

for construction geometry.

The coordinate system.

By default, you sketch relative to the default coordinate system in the model.

• To switch to one of the other two default planes, click the desired sketch tool, and press the

Tab

key. The origin of the current sketch plane is displayed.

•

To change the coordinate system for your 3D sketch, click the desired sketch tool, hold down the

Ctrl

key, and click a plane, a planar face, or a user-defined coordinate system.

•

If you select a plane or a planar face, the 3D sketch planes rotate so that the XY sketch plane is aligned with the selected item.

• If you select a coordinate system, the 3D sketch planes rotate so that the XY sketch plane is parallel to the XY plane of the coordinate system.

Space Handle.

A graphical assistant helps you maintain your orientation while you sketch on several planes. This assistant is called a space

handle. The space handle appears when the first point of a line is defined on a selected plane. Using the space handle, you can select the axis along which you want to sketch. q

Dimensioning

. You can sketch lines to the approximate length, and then dimension them exactly.

•

Create a length dimension by selecting two points, a line, or two parallel lines.

•

Create an angular dimension by selecting either three points or two lines.

Geometric Relations.

You can add relations to points and lines in a 3D sketch, using

Add Relations

. Also, relations are automatically added for 3D sketch lines.

•

As you sketch a line, the line snaps to one of the major directions, X, Y, or Z, if applicable, and is constrained as

Horizontal

Vertical

, or

Along Z

, respectively. The relations are added with respect to the current coordinate system for the 3D sketch.

•

You are not restricted to drawing lines along one of the three major directions. You can sketch in the current sketch plane at an angle to one of the major directions, or you can sketch out-of-plane if the endpoint of the line snaps to existing model geometry.

17-2

Chapter 17 3D Sketching

Line snap.

During the creation of a line, you can snap the line to geometry that already exists in the part, such as model surfaces or vertices, and sketch points.

•

Snap is not enabled if you are sketching in one of the major coordinate directions.

•

If you are sketching on a plane, and the system infers a snap to a non-planar point, a temporary 3D graphics box is displayed to indicate an off-planar snap.

Virtual sharps.

When you create an arc with the

Fillet

tool, the original common point of the lines is displayed as a virtual sharp. To change the display of the virtual sharp, click

Tools

Options

. On the

Document Settings

tab, under

Detailing

, select

Virtual

Sharps

. Choose one of the styles that are depicted.

•

You can add dimensions and relations to virtual sharps in a 3D sketch.

•

If you delete an arc, the lines extend to meet at the virtual sharp.

•

If you delete a line used to create a fillet, any arc it was joined with remains. The virtual sharp becomes a sketch point.

Using a 3D Sketch to Create an Oven Rack Frame

The outer frame of a wire oven rack is built by sweeping a circle along a 3D sketch.

After you complete half of the rack, then you can take advantage of the part’s symmetry and use the

Mirror All

function to finish the model.

Outer frame

To create the 3D sketch of the outer frame:

Open a new part on the

Tutorial

tab, and click

Isometric

to change the view orientation.

TIP:

It is easier to create a 3D sketch in an isometric orientation because the

X, Y, and Z directions are visible.

Click

3D Sketch

or click

Insert

3D Sketch

, to open a new sketch.

SolidWorks 2001 Getting Started 17-3

Special Topics

Click

Line

and sketch a 135mm line on the XY plane from the origin along the X axis. The pointer changes to while sketching along the X axis.

TIP:

Sketch the line to an approximate length, then dimension to the exact length later.

Begin sketch line at origin.

Click

Select

and click the beginning endpoint of the line. Make sure that the endpoint is exactly at the point of the origin (0, 0, 0 as shown in the

PropertyManager). Click

Add Relations

and add a

Fix

relation.

a) b) c) f) g) h)

Click

Line

and continue sketching the other lines from the endpoint of the previous line. Each time you begin a new line, the origin for the current coordinate system is displayed at the beginning of the new line to help orient you.

d) e)

Sketch down the Y axis for 15mm.

Sketch along the X axis for 15mm.

Press

Tab

to change the sketch plane to the

YZ plane .

Sketch along the Z axis for 240mm.

Press

Tab

twice to change the sketch plane back to the XY plane.

Sketch back along the X axis for 15mm.

Sketch up the Y axis for 15mm.

Sketch back along the X axis for 135mm.

Dimension each of the lines as shown.

Click

Fillet

on the Sketch Tools toolbar, or click

Tools

Sketch Tools

Fillet

and fillet each intersection with a 5mm fillet.

Close the sketch.

Save the part as

Rack.sldprt

17-4

Chapter 17 3D Sketching

To complete the base feature, one half of the outer frame, you sweep a 5mm diameter circle along the 3D sketch path.

Open a 2D sketch on the

Right

plane and sketch a 5mm diameter circle at the origin.

Close the sketch.

Click

Sweep

, or

Insert, Base, Sweep

The

Base-Sweep

PropertyManager appears.

Under

Profile and Path

, select the circle

(

Sketch1

) for the

Profile

, and select the 3D sketch (

3DSketch1

) for the

Path

Click

Extruding the Supports

Make a linear pattern of extrusions that extend from one side of the frame to the other.

Open a 2D sketch on the

Front

plane and sketch a circle on what appears to be the face of the frame. (The

Front

plane is actually in the center of the frame wire.)

Dimension the center of the circle 11mm from the origin.

Dimension the diameter of the circle to 4mm.

Click

Extruded Boss/Base

Insert,

Boss, Extrude

The

Boss-Extrude

PropertyManager appears.

Under

Direction 1

, set the

End condition

Blind

, and

Depth

to 240mm. Click

Reverse direction

and look at the preview to be sure the extrusion is moving in the correct direction to meet the other side of the frame.

Click

SolidWorks 2001 Getting Started 17-5

Special Topics

Now pattern the extrusion.

Click

View, Temporary Axes

to turn on the display of all temporary axes.

Select

Boss-Extrude1

and click

Linear Pattern

Pattern

The

Linear Pattern

PropertyManager appears.

Click the temporary axis on the face of the frame where you sketched the circle.

An arrow appears on the frame that points in the direction the pattern will take, and

Axis <1>

appears in the

Pattern

Direction

box.

Under

Direction 1

• Click

Reverse direction

if necessary. Check the preview for the direction of the pattern.

• Set

Spacing

to 22mm.

• Set

Number of Instances

to 6.

Click

The extrusion pattern is completed.

Use the

Mirror All

function to complete the wire rack.

Click

Insert, Pattern/Mirror, Mirror All

The

Mirror All

dialog box appears.

Rotate the half-rack that you created and click on the end face of the frame.

Face <1>

appears in the

Mirror Plane

box.

Click

The rack is completed.

Save the model.

17-6

Importing Files / Using FeatureWorks Software

This chapter guides you through the import of a gasket and a company logo, and demonstrates the following: q

Importing an IGES

file q

Using the FeatureWorks™ software to recognize features on the imported solid q

Importing a DXF file q

Copying a sketch from a drawing to use for a feature in a part q

Exporting a SolidWorks part document as an STL file

SolidWorks 2001 Getting Started 18-1

Special Topics

Importing an IGES File

You can import surfaces from IGES files and use them to create a base feature if the surfaces form a closed volume.

Click

File, Open

The

Open

dialog box appears.

In the

Files of type

list, click

IGES Files (*.igs, *.iges)

Click

Options

to set the import options.

Make sure

Knitting

and

Try forming solid(s)

are selected, then click

When these two options are selected, the SolidWorks software attempts to knit the surfaces from an imported file into a solid model.

Browse to the path

\installation_directory\

samples\tutorial

, select

Gasket.igs

, and click

Open

Once the SolidWorks software finishes knitting the surfaces into a base feature, the dialog box disappears and the imported body appears in the graphics area.

If a message appears asking if you want to proceed with feature recognition, click

Notice the new feature,

Imported1

, in the

FeatureManager design tree. You cannot edit the sketches, dimensions, or features of an imported solid model.

18-2

Chapter 18 Importing Files / Using FeatureWorks Software

Recognizing Features using the FeatureWorks Software

The FeatureWorks software recognizes features on an imported solid body in a part document. Recognized features are the same as features that you create using the

SolidWorks software. You can edit the definition of recognized features to change their parameters. For features that are based on sketches, you can edit the sketches of recognized features to change the geometry of the features.

NOTE:

If you do not have the FeatureWorks software installed on your computer, please turn to

Importing a DXF File

on page 18-4. You can

still complete the remainder of the exercise if you do not have the

FeatureWorks software.

FeatureWorks

does not appear on the SolidWorks main menu bar, click

Tools

Add-Ins

, select

FeatureWorks

, and click

Click

FeatureWorks Options

on the toolbar, or click

FeatureWorks

Options

Make sure

Overwrite existing part

and the

Basic features

check box are selected, then click

Selecting the

Basic features

check box enables the FeatureWorks software to recognize extrusions and revolves during Automatic Feature Recognition.

Click

Recognize Features

on the toolbar, or click

FeatureWorks

Recognize

Features

The

Recognize Features - Interactive

dialog box appears.

a) b) c)

Recognize a single feature.

Set the

Feature Type

Cut Extrude

Select the circular edge of the cut as shown.

Click

Recognize Feature

The selected edge is recognized as the sketch for a

Cut-Extrude

feature. The recognized feature disappears from the solid body. Any geometry not yet recognized still appears in the graphics area.

Click

Automatic

to perform Automatic Feature

Recognition.

The FeatureWorks software attempts to recognize as many features as possible from the remaining geometry.

Select this edge

Click

Map Features

to accept the default feature recognition.

The

Imported1

feature is replaced by a

Base-Extrude

and a

Cut-Extrude1

feature in the FeatureManager design tree. The

Base-Extrude

feature is the result of the

Automatic Feature Recognition. These new features are fully editable.

SolidWorks 2001 Getting Started 18-3

Special Topics

Editing the Sketch of a Feature

Now, you can change the size of one of the holes in the gasket.

Right-click

Cut-Extrude1

in the

FeatureManager design tree and select

Edit Sketch

Add a

Concentric

relation between the sketched circle and the circular edge as shown.

Add a 10mm dimension to the sketched circle, then exit the sketch.

The hole changes size.

Sketched circle

Save the part as

Gasket.sldprt

Circular edge

Importing a DXF File

You can import a DXF file to a drawing document. The DXF file that you import in this exercise contains the company logo for a fictitious company, Rainbow Corporation.

Click

File, Open

The

Open

dialog box appears.

In the

Files of type

list, click

Dxf Files (*.dxf)

Browse to the path \installation_directory\

samples\tutorial

, select

Rainbow.dxf

, and click

Open

The

DXF/DWG Import Wizard

starts.

The

DXF/DWG Import - Document Type

dialog box appears.

Click

Import to a new drawing

, then click

Next

The

DXF/DWG Import - Document Settings

dialog box appears.

a) b) c) d)

Do the following:

Select the

Show preview

check box.

Select

A-Landscape

as the

Paper size

Click

Position

, then set

and

to 0 (zero).

Under

Document template

, browse to the path

installation_directory

\lang\<

your_language

select

Draw.drwdot

, and click

Open

Click

Next

The

DXF/DWG Import - Drawing Layer Mapping

dialog box appears.

Click

Import all data to the sheet

, then click

Finish

18-4

Chapter 18 Importing Files / Using FeatureWorks Software

A new drawing document is created containing the entities in the DXF file. The imported company logo consists of lines, arcs, and dimensions.

Prepare the Imported Entities for Copying

Before you copy imported DXF entities from a drawing to a sketch in a part, you must prepare the entities. The imported sketch entities are unconstrained; there are no relations between the entities. Also, the dimensions in the imported DXF file are not attached to any sketch entities.

Click

Tools

Relations

Constrain All

, then click

in the message box.

The SolidWorks software adds all the apparent relations and reports the number of relations that are added.

Click

Display/Delete Relations

or ,

Relations

Display/Delete

Using the

Next

Previous

buttons, view each relation.

Notice that the SolidWorks software added many

Coincident

Collinear

, and

Horizontal

relations.

Click

Close

to close the

Display/Delete Relations

dialog box.

Click

Tools

Dimensions

Attach Dimensions

, then click

in the message box.

Each of the dimensions in the imported DXF file are attached to the appropriate arc.

Click

Rebuild

Copying and Pasting the Imported Entities

You can copy entities from a drawing to a sketch of a part. The software creates a new sketch in the part once you paste the entities.

Drag-select the entities on the drawing, including the dimensions.

Click

Copy

or press

Ctrl+C

Click

Window

Gasket

to switch to the part.

Select the front face of the gasket, then click

Paste

or press

Ctrl+V

A new sketch is automatically created in the part containing the company logo.

SolidWorks 2001 Getting Started 18-5

Special Topics

Right-click

Sketch3

and select

Edit Sketch

Notice that all of the dimensions and entities from the drawing are in the new sketch.

Add the 5mm and 20mm dimensions as shown to position the sketch entities.

Extrude the Company Logo

With the sketch still open from the previous section, click

Extruded Cut

Insert

Cut

Extrude

The

Cut-Extrude

PropertyManager appears.

Under

Direction 1

, do the following:

• Set

End Condition

Blind

•

Set

Depth

to 1mm

Click

Now, change the color of the new extrusion so it appears more easily.

Select

Cut-Extrude2

in the FeatureManager design tree.

Click

Edit Color

on the Standard toolbar.

The

Edit Color

dialog box appears.

Click the desired color on the palette, then click

18-6

Chapter 18 Importing Files / Using FeatureWorks Software

Exporting an STL File

You can save a SolidWorks part document as an STL file. STL format is intended for transfer to rapid prototyping machines.

Click

File

Save As

The

Save As

dialog box appears.

In the

Save as type

list, click

STL Files (*.stl)

, then click

Options

to set the export options.

The

STL Export Options

dialog box appears.

Make sure the

Quality

is set to

Fine

and the

Show STL info before file saving

check box is selected, then click

TIP:

You can experiment with the

Quality

settings to determine the best settings for your own rapid prototyping machines.

Click

Save

to save the file with the default name,

Gasket.stl

A message box appears displaying the number of

Triangles

File Size

, and

File

Format

Click

Yes

to complete the save operation.

SolidWorks 2001 Getting Started 18-7

Learning to use PhotoWorks

This chapter teaches you how to use the PhotoWorks

™ software to create photo-realistic images of SolidWorks models. This chapter covers the following topics: q

PhotoWorks fundamentals q

Using the PhotoWorksManager q

Rendering an image with the PhotoWorks Render Wizard q

Selecting and applying PhotoWorks materials q

Previewing and editing PhotoWorks materials q

Rendering a sub-image q

Saving and viewing image files q

Creating and managing PhotoWorks material archives q

Creating and applying decals with the PhotoWorks Decal Wizard q

Designing PhotoWorks scenery

SolidWorks 2001 Getting Started 19-1

Special Topics

Section 1: PhotoWorks Fundamentals

Before you begin, there are a few things you need to know about the PhotoWorks software.

PhotoWorks software creates realistic images directly from SolidWorks models.

The PhotoWorks software interacts with the 3D geometry that you create with

SolidWorks software. All changes to SolidWorks models are accurately represented in

PhotoWorks images.

PhotoWorks software is for use with 3D SolidWorks parts and assemblies. It cannot be used with SolidWorks drawings.

PhotoWorks software is fully integrated with SolidWorks. The PhotoWorks software is supplied as a SolidWorks dynamic link library (

.dll

) add-in. You access all the controls for the PhotoWorks rendering interface from the PhotoWorks item on the main SolidWorks menu bar, or from the PhotoWorks toolbar. This menu bar is displayed whenever a SolidWorks part or assembly document is open. q

PhotoWorks materials give you control over the appearance of SolidWorks

models. Materials are used in the PhotoWorks software to specify model surface properties such as color, texture, reflectance, and transparency. Material selection and composition are performed using the PhotoWorks material editor. The PhotoWorks software is supplied with a number of archives of pre-defined materials, (metals, plastics, woods, stones, and so on), which can be attached to, and stored with, individual SolidWorks parts and faces. Texture mapping is also supported, enabling you to attach 2D textures such as scanned images and logos, to the surfaces of your models. You can also create your own material archives in which to organize your own collections of materials.

PhotoWorks scenes add photo-realism to your designs. Each SolidWorks model is associated with a PhotoWorks scene, for which you can specify properties such as lighting, shadows, and backgrounds. Scene selection and composition are performed using the PhotoWorks scene editor. The PhotoWorks software is supplied with a number of archives of pre-defined scenes. You can also create your own scene archives. Once you are happy with the look of your scene, you can save it to an image file. You can then incorporate the image in design proposals, technical documentation, product presentations, and so on.

19-2

Chapter 19 Learning to use PhotoWorks

Section 2: The 40-Minute Running Start

This section guides you through your first rendering session with the PhotoWorks software.

PhotoWorks

does not appear on the SolidWorks main menu bar, click

Tools,

Add-Ins

, select

PhotoWorks

, and click

Click

Open

on the Standard toolbar, and open the file:

\installation directory

\samples\tutorial\photoworks\candlestick\cstick.sldprt

Notice that there is a

PhotoWorks Help

item available on the main

Help

menu, and that a PhotoWorks toolbar has been added to the SolidWorks window, beneath the

Standard toolbar. Context-sensitive, online help is also available for most PhotoWorks features by clicking the

Help

button in the dialog box or by pressing the

key.

Set view orientation to

*Trimetric

, then select the

Shaded

view mode from the

View

toolbar. Your screen should look like this:

SolidWorks 2001 Getting Started 19-3

Special Topics

Checking the Options Settings

Before you begin, make sure that your SolidWorks settings match the ones used in this example so that your results will be the same.

Click

Tools, Options

, and select the

Document Properties tab.

Under

Units

, in the

Linear units

section, make sure that

Millimeters

is selected and that

Decimal places

is set to 2.

Under

Image Quality

, make sure that

High Quality

is selected in the

Shaded

section.

Click

Now set PhotoWorks options.

Click

Options

on the PhotoWorks toolbar, or click

PhotoWorks

Options

On the

Render

tab, the PhotoWorks software provides options for trading image quality with rendering performance. Select these options if desired:

•

Anti-aliasing

eliminates jagged silhouette edges. Rendering is slower, but images are smoother. For final image rendering, select this option.

•

Overlay image

prevents the current image from being cleared before the next image is rendered. This option does not affect rendering speed.

On the

Materials

tab, the PhotoWorks software provides options for controlling the transfer of material properties between the SolidWorks and PhotoWorks software. By default, material properties such as color and reflectance are maintained separately in

SolidWorks and PhotoWorks software. The options are:

•

Overwrite SolidWorks properties on select/edit

updates SolidWorks material properties automatically when selecting or editing materials within PhotoWorks.

•

Apply SolidWorks properties for render causes the PhotoWorks software to use

SolidWorks material properties during rendering.

For the purpose of this example, leave both boxes clear.

Click

19-4

Chapter 19 Learning to use PhotoWorks

Using the PhotoWorksManager

The PhotoWorksManager is similar to the FeatureManager design tree in that it provides an outline view of the SolidWorks model.

The PhotoWorksManager indicates which items of geometry have which PhotoWorks materials and decals associated with them.

This makes it easy to: q

Understand the way in which material and decal inheritance works.

Select and edit materials and decals associated with the model.

Transfer materials and decals between components, features, and faces.

You can also customize the appearance of the PhotoWorksManager to suit your needs during a PhotoWorks session. For example, you can configure the PhotoWorksManager to show every feature and face in the model, or to show only those features or faces that have particular attributes associated with them, such as materials or decals.

Split the FeatureManager design tree.

Select

PhotoWorksManager

in the FeatureManager design tree to display the

PhotoWorksManager tab.

The top level of the tree shows two items:

• The part, indicated by the

Cstick

icon. From here, you can edit the material and decal properties associated with the part by right-clicking the

Cstick

icon and selecting from the

Material

Decals

shortcut menus.

• The current PhotoWorks scene, indicated by the

Scene

icon. From here, you can edit the scene by double-clicking the

Scene

icon (or right-clicking it and selecting

Edit

). You can also edit a particular scene property by clicking the

beside

Scene

icon, and then double-clicking the

Lighting

Foreground

Background

, or

Scenery

icons (or right-clicking an icon and selecting

Edit

When you apply a material or a decal to the part, or to a particular feature or face, the

PhotoWorksManager is updated automatically with new icons to reflect these changes.

You can access these properties again (for subsequent editing) by double-clicking on the appropriate material or decal icon within the PhotoWorksManager.

SolidWorks 2001 Getting Started 19-5

Special Topics

Rendering an Image

Rendering an image with the PhotoWorks software is straightforward.

Click

Render

on the PhotoWorks toolbar, or click

PhotoWorks

Render

19-6

The PhotoWorks software produces a solid, smooth-shaded rendering of the candlestick, against a default background scene consisting of a reflective tread-plate

‘floor’ and cork-patterned ‘walls’.

The

PhotoWorks - Default Material

dialog is displayed, indicating that the part has been rendered with the default material,

Polished Plastic

. The default material can be applied to the model automatically for you, if you do not wish to create and apply a material yourself. (You can also set your own default material.)

Click

Yes

to apply this material to the model.

The

PhotoWorks - Default Scene

dialog is displayed, indicating that the part has been rendered with the default scene,

Shiny Tread Plate and Cork

. The default scene can be applied to the model automatically for you, if you do not want to select or create a default scene yourself. (You can also set your own default scene.)

Click

Yes

to apply this scene to the model.

Change the view orientation.

The view returns to the normal, SolidWorks, shaded view.

Click

Render

again.

Each time you change the view, you need to render the image again.

To abort a rendering, click

Stop

in the

PhotoWorks - Render

dialog box.

Chapter 19 Learning to use PhotoWorks

Using the PhotoWorks Render Wizard

The PhotoWorks Render Wizard guides you through the basic steps involved in creating a photo-realistic image. Key steps include the selection of PhotoWorks material and scene properties.

A material defines how the surface of a part reacts to light. Each material consists of properties that determine various aspects of its appearance, such as surface color and texture, reflectance, and transparency.

A scene consists of properties additional to those directly associated with the SolidWorks model. These include lighting, shadows, foreground and background effects, and scenery.

Click

Render Wizard

on the PhotoWorks toolbar, or click

PhotoWorks

Render

Wizard.

After reading the

Welcome

note, click

Next

to learn about the PhotoWorks material

editor.

The

Manager

tab on the

PhotoWorks - Material Editor

dialog box has two display panels:

• A Material Archive tree, which lists all the material archives currently available

• A material selection area, in which to view and select materials

Click the

Show me

buttons to learn how to select a material.

In the

Stock Procedural

material archive, click the

Metals class to display the materials it contains.

Click the

Antique Brass

material to select it, then click

Apply

NOTE:

You can also select and apply a material in one operation by double-clicking the image in the material selection area.

Click

Next

to learn about the PhotoWorks scene editor.

The

Manager

tab on the

PhotoWorks - Scene Editor

dialog box has two display panels:

•

A Scene Archive tree, which lists all the scene archives currently available

•

A scene selection area, in which to view and select scene templates

Click the

Show me

buttons to learn how to select a scene.

Click

Next

to proceed to the final dialog box of the Render Wizard, then click

Finish

The PhotoWorks software renders the candlestick with an antique brass finish.

SolidWorks 2001 Getting Started 19-7

Special Topics

Selecting a Material

Now add more realism to the candlestick by selecting a different material for it.

Notice that the PhotoWorksManager has been updated by the addition of an

Antique

Brass

material icon to indicate the material currently associated with the candlestick.

Antique Brass

(or right-click and select

Edit

Alternatively, you can right-click the icon in the PhotoWorksManager and select

Material

Edit

, or you can click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials

Notice that the icon representing the material currently associated with the part is highlighted in the material selection area on the

Manager

tab whenever you open the material editor.

Select the

Polished Brass

material.

The

Preview

window, to the right of the

PhotoWorks - Material Editor

dialog box, is updated to show how the part will appear when it is rendered.

Click

Apply

, then click

Close

Notice that the PhotoWorksManager has been updated with a

Polished Brass

material icon, to indicate the change of material.

Click

Render

PhotoWorks, Render

19-8

The candlestick is rendered with a polished brass appearance. Notice how the base of the candlestick reflects its stem and the surrounding background.

Change the view orientation, then render again.

Notice how the reflections change on the curved surfaces of the candlestick.

Chapter 19 Learning to use PhotoWorks

Previewing a Material

You can use the

Preview

window on the

PhotoWorks - Material Editor

dialog box to preview materials and material edits rapidly, before committing to a full-size render.

Various controls are provided to manipulate the behavior of the

Preview

window.

1 Polished Brass

in the PhotoWorksManager (or right-click and select

Edit

Now examine the

Preview

window.

In the

Rendering

section, you have the following options for rendering the preview:

• In

Automatic

mode , each time you change a material property, the preview is rendered again.

• In

Manual

mode , you can change as many properties as you want, then render the preview once to incorporate all the changes. To render the preview in

Manual

mode, click

Automatic

mode . Click again to return to

Manual

mode .

• In

Full

mode , the PhotoWorks software uses photo-realistic rendering for the preview.

• In

Interactive

mode , the PhotoWorks software uses OpenGL rendering for the preview.

NOTE:

You can also use PhotoWorks OpenGL rendering in the active

SolidWorks document window. Click

Interactive Rendering

on the PhotoWorks toolbar, or click

PhotoWorks

Interactive

Rendering

•

In the Display components section, you can choose to display the

Model

, or you can choose a simpler geometric shape. Preview rendering is faster with a simpler shape that approximates that of the model, such as a

Cylinder

. For certain types of change, you may need to see the details on the model.

•

Click

Zoom to Fit

to display the part full size in the

Preview

window.

•

Click

Zoom to Area

to zoom in on a particular area of the

Preview

window by positioning the pointer over it, then clicking and dragging a bounding box to enclose the selected area.

•

Click

Rotate View

to rotate the part by clicking and dragging in the

Preview

window.

•

You can also choose to disable various material properties temporarily, such as reflectance and transparency, to further accelerate preview rendering.

NOTE:

The

PhotoWorks - Material Editor

dialog box is a modeless dialog.

You can keep it open while selecting other SolidWorks geometry and reference objects.

SolidWorks 2001 Getting Started 19-9

Special Topics

Editing a Material

Now try editing the reflectance properties of the polished brass material that you applied previously to the candlestick.

Click the

Reflectance

tab on the

PhotoWorks - Material Editor

dialog box.

The reflectance of a material defines its ‘finish’, and determines how it behaves in the presence of light. Notice that the

Style

is set to

Conductor

. The PhotoWorks software supports several reflectance styles.

Change the

Style

Metal

Notice that the preview retains the brass color but is now rendered with a specular metallic appearance.

Change the

Style

Glass

Click

Apply

, then click

Close

Click

Render

PhotoWorks

Render

19-10

The candlestick is rendered with a realistic approximation of glass reflectance, including transparency, reflection, and refraction.

Chapter 19 Learning to use PhotoWorks

Rendering a Sub-image

You can use sub-image rendering to constrain the PhotoWorks software to render a selected area or selected geometry within the active SolidWorks document window.

Change the view orientation.

Click

Render Area

on the PhotoWorks toolbar, or click

PhotoWorks

Render

Area

Drag a window over the area to render.

The PhotoWorks software renders only the area you selected.

Now edit the material again:

a) b) c)

Polished Brass

in the PhotoWorksManager (or right-click and select

Edit

On the

Reflectance

tab, set

Mirror

to 0.5, to make the surface of the material appear more reflective.

Click

Apply

, then click

Close

Click

Render Last

on the PhotoWorks toolbar, or click

PhotoWorks

Render

Last

The PhotoWorks software re-renders the sub-image that you selected previously. This is a useful facility for when you want to edit the properties of a single material but do not want to render the whole model. The last sub-image remains valid until you select a new sub-image.

Click

Boss-Sweep1

in the FeatureManager design tree.

Click

Render Selection

on the PhotoWorks toolbar, or click

PhotoWorks

Render Selection

The PhotoWorks software renders a sub-image of the selected geometry.

Change the view orientation again, then click

Render Last

PhotoWorks

Render Last

The PhotoWorks software re-renders the

Boss-Sweep1

feature. Again, this is a useful facility for when you want to ‘fine-tune’ the appearance of a particular feature, without having to render the whole model.

SolidWorks 2001 Getting Started 19-11

Special Topics

Saving an Image to File

You can save a PhotoWorks image to a file for use in design proposals, technical documentation, product presentations, and so on. The PhotoWorks software supports

Bitmap (

.bmp

), TIFF (

.tif

), Targa (

.tga

), and JPEG (

.jpg

) formats, as well as PostScript

(

.ps

) and the PhotoWorks image format (

.lwi

First, change the candlestick material once again:

a) b)

Polished Brass in the PhotoWorksManager (or right-click and select

Edit

Use the scroll bar in the material selection area to locate

Silver Plate

, then doubleclick it to select and apply the material.

Set view orientation to *Trimetric.

Click

Render Image to File

on the PhotoWorks toolbar, or click

PhotoWorks

Render Image to File

, to display a

Save As

dialog box.

The PhotoWorks software suggests an image file name based on the name of the part, along with the extension appropriate to the selected image format. By default, the image will be stored in the same directory as the part.

(Optional.) Select a different file name, file type, or storage location for the image.

(Optional.) Set the

Image Size

, by specifying the

Width

and

Height

By default, the PhotoWorks software sets the resolution of the image in

Pixels

, according to the width and height of the active SolidWorks document window. You can specify the

Width

and

Height

of the image in

Centimeters

Inches

if you find these units more convenient. If you want the image to retain its original proportions when you alter the

Width

Height

, select the

Fixed aspect ratio

check box.

(Optional.) Click

Options

to set options appropriate to the selected image format.

(Optional.) Select the

Prompt when render complete

check box if you want the

PhotoWorks software to notify you when the image has been rendered to file.

Click

Save

The PhotoWorks software renders the image to file.

19-12

Chapter 19 Learning to use PhotoWorks

Viewing an Image File

You can view previously saved images using the PhotoWorks image viewer. All the image formats available in the PhotoWorks software (except PostScript) are supported by this utility.

Click

View Image File

on the PhotoWorks toolbar

, or click

PhotoWorks

View

Image File

Locate the image file that you saved from

Saving an Image to File

on page 19-12.

NOTE:

Select the

Preview

check box on the file browser if you want to preview the image file before opening. This is useful if you have several image files.

Click

Open

The PhotoWorks software loads the image file and displays it in a separate window.

SolidWorks is disabled temporarily while viewing an image file

Close the

PhotoWorks - Image Viewer

window.

Save and close the part.

SolidWorks 2001 Getting Started 19-13

Special Topics

Section 3: Working with PhotoWorks Materials

The PhotoWorks software provides an intuitive and flexible interface to material selection and editing, enabling you quickly and easily to specify surface properties such as color, texture, reflectance, and transparency for your SolidWorks models. This section teaches you more about applying PhotoWorks materials to SolidWorks parts, features, and faces.

The PhotoWorks software is supplied with a number of archives of pre-defined materials.

This section also demonstrates how to create and manage your own material archives, to help you to organize your own collections of materials.

Finally, this section shows how to link materials to an archive via instancing. This facility enables you to edit material properties across multiple items of geometry simultaneously.

Click

Open

and open the file:

\installation directory

\samples\tutorial\universal_joint\ujoint.sldasm

Split the FeatureManager design tree.

Select the

PhotoWorksManager

tab.

Set view orientation to

*Isometric

, and set view mode to

Shaded

. Your screen should look like this:

19-14

Chapter 19 Learning to use PhotoWorks

Adding a Material to a Part Within an Assembly

Start by creating a knurled plastic finish for the knob on the crank handle.

Click

crank-knob

in the FeatureManager design tree.

Click

Edit Part

on the Assembly toolbar.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

Double-click the

Stock Procedural 3

archive (or click the

beside its name) to expand it and display the material classes it contains.

Click the

Plastic: Resin

class to display the materials it contains.

Select the

Shiny Resin Cyan

material.

Switch to the

Displacement

tab.

The displacement property of a material defines how rough or ‘bumpy’ it is. Notice that the

Style

is set to

Rough

. The PhotoWorks software supports several displacement styles.

Change the

Style

Knurled

Set

Scale

to 0.25, to make the knurls slightly smaller.

Click

Apply

, then click

Close

Notice that the

crank-knob

part in the

PhotoWorksManager has been updated by the addition of

(p) Shiny Resin Cyan

material icon. The

(p)

indicates that the material is associated with a base part.

Click

Edit Part

again.

Click

Render

on the PhotoWorks toolbar, or click

PhotoWorks

Render

The PhotoWorks software renders the assembly, the crank-knob now having a knurled plastic appearance.

SolidWorks 2001 Getting Started 19-15

Special Topics

Using Interactive Rendering to Preview Material Edits

You can use PhotoWorks interactive rendering to preview the effects of editing a material.

In this mode, the PhotoWorks software uses OpenGL rendering in the active SolidWorks document window. Although interactive rendering does not support all the advanced effects available within the PhotoWorks software, it does provide for rapid previewing of material edits.

Click

Interactive Rendering

on the PhotoWorks toolbar, or click

PhotoWorks

Interactive Rendering

Click

bracket

in the FeatureManager design tree.

Click

Edit Part

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

Move the

PhotoWorks - Material Editor

dialog box so that it does not obscure the

SolidWorks window.

Expand the

Stock Procedural

material archive, click the

Metals

class, then click the

Steel

material to select it.

The

Preview

window is updated to show how the part will appear when it is rendered.

Click

Apply

The PhotoWorks software updates the main window to show the application of the material.

In the material selection area, click

Stainless Steel

, then click

Apply

The PhotoWorks software updates the main window to show the change of material.

Expand the

Metal Textures

archive, click

Brushed

, then double-click

Galvanized

to select and apply it.

Notice that the

bracket

feature in the

PhotoWorksManager has been updated by the addition of a

(p) Galvanized

material icon.

Click

Render

PhotoWorks

Render

19-16

Chapter 19 Learning to use PhotoWorks

Adding Materials to Individual Features and Faces

You can use the PhotoWorks material editor to apply different materials to individual features and faces. You can also use the PhotoWorksManager to cut, copy, and paste materials between selected features and faces.

Hold down

Ctrl

and select

Boss-Extrude1

and

Fillet1

of the bracket in the

FeatureManager design tree.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

NOTE:

When you edit the material on selected features or faces, the

Preview

window displays the selected geometry only, rather than the whole part or assembly.

Expand the

Stock Procedural

archive, click

Metals

, then locate and double-click

Machined Aluminum

to select and apply it.

Notice that the

Boss-Extrude1

and

Fillet1

features in the PhotoWorksManager have been updated by the addition of

Machined Aluminum

material icons.

b) c) d)

Now edit the material associated with

Boss-Extrude1

, then copy and paste the change to

Fillet1

, via the PhotoWorksManager:

Double-click the

Machined Aluminum

icon beneath

Boss-Extrude1

in the

PhotoWorksManager.

Locate and double-click

Chrome Plate

to select and apply it.

Chrome Plate

in the PhotoWorksManager and select

Copy

Right-click the

Machined Aluminum

icon beneath

Fillet1

in the

PhotoWorksManager and select

Paste

a) b) c)

Now edit the material on a single face:

Select the flat face on the top of the bracket.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

Expand the

Metal Textures

archive, click

Brushed

, then double-click

Brushed 1

to select and apply it.

Notice that the

Shell1

feature in the PhotoWorksManager has been updated by the addition of a

<Face>

icon, with an associated

Brushed 1

material icon.

a) b) c)

Now copy the

Brushed 1

material and paste it onto another face:

Right-click the

Brushed 1

icon and select

Copy

Select another face of the bracket.

Click

Paste Material

on the PhotoWorks toolbar, or click

PhotoWorks

Paste

Material

Click

Edit Part

again.

Click

Render

PhotoWorks

Render

Save the assembly.

SolidWorks 2001 Getting Started 19-17

Special Topics

Creating a Material Archive

With the PhotoWorks Material Manager you can create your own material archives.

You can archive both procedurally defined (solid) and texture-mapped (wrapped) materials, and you are free to organize the contents of each archive to suit your needs. For example, you may want to create material classes that classify materials according to their inherent properties (metal, plastic, stone, fabric, and so on). Alternatively, you may want to store all the materials that relate to a particular project or model in a class of their own.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials

Click

Create Archive

to display the

Create Archive

dialog box.

Type

My Materials

in the

File name

box, choose the location of the

.pma

file in which to store the archive, then click

Save

NOTE:

By default, the PhotoWorks software uses the root directory on your drive to store your material archives. You may want to create a new directory in which to store material archives.

The PhotoWorks software appends a new material archive,

My Materials

, containing an empty

Untitled

material class to the Material Archive tree.

Click-pause-click

Untitled

, and rename it to

Universal Joint

The PhotoWorks software updates the symbol denoting the archive to indicate that the class has been renamed.

Click the

My Materials

archive to select it, then click

Save Archive

Click

Close

19-18

Chapter 19 Learning to use PhotoWorks

Archiving a Procedurally Defined Material

Although it is not possible to edit the pre-defined material archives supplied with the

PhotoWorks software, it is possible to add a copy of any pre-defined material to a material archive of your own. You can then edit the properties of your copy of the material to suit the needs of a particular project or model.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials

Expand the

My Materials

archive.

Now expand the

Stock Procedural

archive, then click

Metals

Drag the

Polished Brass

material and drop it on the

Universal Joint

class when the class is highlighted.

The PhotoWorks software appends a copy of the

Polished Brass

material to the

Universal Joint

class.

Click-pause-click

Polished Brass

, and rename it to

Yoke

Click the

My Materials

archive to select it, then click

Save Archive

Click

Close

The PhotoWorks software notifies you that the current material selection has changed, and asks whether you want to apply this material.

Click

. (You will apply this material, and edit its definition, later in this tutorial.)

SolidWorks 2001 Getting Started 19-19

Special Topics

Archiving a Texture-Mapped Material

You can archive your own texture-mapped materials. For example, these may include scanned bitmaps of paint swatches, metal finishes, decals, labels, and company logos.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials

Expand the

My Materials

archive, and click the

Universal Joint

class.

Click

Create Material (from Image File) in Archive

to display the

PhotoWorks –

Add Texture Materials

dialog box.

Locate the file:

\installation directory

\samples\tutorial\photoworks\textures\tex_tile.bmp

Click

Add

, then click

Close

The PhotoWorks software appends a new texture-mapped material to the class, based on the image file. The material is given the image filename, minus the three-letter filename extension.

Click the

My Materials

archive to select it, then click

Save Archive

Click

Close

The PhotoWorks software notifies you that the current material selection has changed, and asks whether you want to apply this material.

Click

Close the assembly.

19-20

Chapter 19 Learning to use PhotoWorks

Linking Materials to an Archive via Instancing

You can use instancing to apply identical copies of any PhotoWorks material to multiple items of SolidWorks geometry. All instances of a given material share the same material definition, which is recorded in the material archive to which they are linked.

In this exercise, you apply the

Yoke

material that you created previously to two separate parts within the Universal Joint assembly.

Open the file:

\installation directory

\samples\tutorial\universal_joint\yoke_male.sldprt

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

Expand the

My Materials

material archive, click the

Universal Joint

class, then click the

Yoke

material to select it.

(Optional.) Press

The PhotoWorks software re-renders the thumbnail image in the archive to match the image displayed in the

Preview

window.

Select the

Link to Archive

check box.

The PhotoWorks software notifies you that instancing the material will apply the properties from the shared material definition in the linked material archive.

Click

Yes

to proceed with the instanced material.

Click

Apply

, then click

Close

Save the part, then close it.

Open the file:

\installation directory

\samples\tutorial\universal_joint\yoke_female.sldprt

Repeat steps

through

, above.

Both the

yoke_male

and

yoke_female

parts now share identical instances of the

Yoke

material.

SolidWorks 2001 Getting Started 19-21

Special Topics

Editing a Shared Material Instance Definition

Any edits that you make to a shared material instance definition are applied automatically to all instances of the material. This feature enables you to alter material properties across multiple items of geometry simultaneously.

Try editing the definition of the

Yoke

material that you applied in the previous exercise.

Open the file:

\installation directory

\samples\tutorial\universal_joint\ujoint.sldasm

Click

Render

PhotoWorks

Render

Notice that the

yoke_male

and

yoke_female

parts are rendered with the polished brass

Yoke

material that you created previously.

Click

yoke_male

in the FeatureManager design tree.

Click

Edit Part

on the Assembly toolbar.

Click

Materials

on the PhotoWorks toolbar, or click

PhotoWorks, Materials.

In the

Apply to

list, select

Archive

Click the

Color

tab.

Under

Colors

, click

Edit

, select a color from the palette, then click

Click

Apply

Click

Yes

to update the existing shared material definition.

Click

Close

Click

Edit Part

again.

Click

Render

PhotoWorks

Render

Notice that the appearance of the

Yoke

material has changed on both the

yoke_male

and

yoke_female

parts.

Save and close the assembly.

19-22

Chapter 19 Learning to use PhotoWorks

Section 4: Working with PhotoWorks Decals

This section shows you how to use the PhotoWorks software to attach custom labels or artwork (such as company logos or part numbers) to SolidWorks models.

The PhotoWorks Decal Wizard guides you through the steps involved in creating and adding a decal to a SolidWorks model.

Once you have added a decal, you can control its size and position, and overlay multiple decals, in any order, over any material type, including texture-mapped materials, using the

PhotoWorks decal editor.

Open the file:

\installation directory

\samples\tutorial\photoworks\housing\housing.sldprt

Split the FeatureManager design tree.

Select the

PhotoWorksManager

tab. Your screen should look like this:

SolidWorks 2001 Getting Started 19-23

Special Topics

Adding a Decal to a Face

Now attach a decal representing a part number.

Select the large curved face on the

Base

Click

Decals

or click

PhotoWorks, Decals

The

PhotoWorks - Decal Editor

dialog box is displayed. It includes:

• A Decal Manager tree, which lists all decals attached to the current part, feature, or face.

•

A display area, in which to view the components of individual decals.

Select this face

Notice that

Create new decal with wizard

is selected.

Click

Create New Decal

The

PhotoWorks - Decal Wizard

is displayed.

After reading the

Welcome

note, click

Next

to select a decal image.

Click

Browse

, then locate and open the file:

\installation directory\

samples\tutorial\photoworks\decals\pw_image.bmp

The image file contains the decal artwork – in this case, a simple part number.

Click

Next

to create a decal mask.

Select

From file

, then click

Next

Browse to the file:

\installation directory\

samples\tutorial\photoworks\decals\pw_mask.bmp

Click

Next

to view the complete decal, consisting of the image combined with the mask.

Click

Next

through to the

Finished!

dialog box of the wizard, then click

Finish

The PhotoWorks software adds the new decal to the Decal Manager tree, giving it the name

Decal1

. The PhotoWorks software displays the components of the decal in the display area on the decal Manager tab. Also,

Image

Mask

, and

Mapping

tabs are added to the

PhotoWorks - Decal Editor

dialog box.

19-24

Chapter 19 Learning to use PhotoWorks

Adjusting a Decal on a Face

Now use the PhotoWorks decal editor to fine-tune the scale and orientation of the decal on the face.

With

Decal1

still selected in the Decal Manager tree, click the

Mapping

tab.

Notice that the PhotoWorks software has created a

Cylindrical

mapping for the decal, with reference to the

Selected face

. However, the scale and orientation of the decal require some adjustment to position it correctly.

Under

Scaling

, drag the

Around axis

slider to a position halfway between

Small

and

Large

Set

Along axis

to 14.00mm.

Under

Orientation

, set

Rotation about axis

to 85°.

The

Preview

window shows the decal correctly sized and centered on the face.

Click

Close.

The PhotoWorks software notifies you that the decal has changed, and asks whether you want to apply the change.

Click

Yes

Notice that the PhotoWorksManager has been updated by the addition of a

Decal1

decal icon, associated with the selected face.

Click

Render

on the PhotoWorks toolbar, or click

PhotoWorks

Render

The PhotoWorks software scales the decal and offsets it to the specified position on the face.

SolidWorks 2001 Getting Started 19-25

Special Topics

Section 5: Working with PhotoWorks Scenes

Composing a scene can improve visual realism by giving your model a more solid, 3D appearance. Rather than leaving the model floating in space, you can use shadows to anchor it against a simple geometric backdrop. You can apply PhotoWorks materials to the backdrop for added realism.

Set view orientation to

*Top

, and rotate the part to approximately the orientation shown.

Click

Scene

on the PhotoWorks toolbar, or click

PhotoWorks, Scene

The

PhotoWorks - Scene Editor

dialog box is displayed. It includes a scene

Manager

tab, from which to access scene archives, plus separate tabs for specific scene properties, and a

Preview

window with which to preview edits to these properties before rendering.

The scene

Manager

tab has two display panels:

•

A Scene Archive tree, which lists all the scene archives currently available

•

A scene selection area, in which to view and select scene templates

Notice that the icon representing the scene currently associated with the part – in this example, the

Default

scene in the

Basic

class of the

Stock Combinations

archive – is highlighted in the scene selection area on the

Manager

tab whenever you open the scene editor.

Click the

Lighting

tab.

Select the

Display shadows

check box.

The PhotoWorks software generates shadows for all SolidWorks directional lights, point lights, and spotlights in the scene.

NOTE:

You can also specify shadow properties for individual SolidWorks lights, using the

PhotoWorks properties

on the appropriate

SolidWorks

Light properties

dialog boxes.

In the

Display components

section of the

Preview

window, select the

Shadows

check box.

Notice how the

Preview

window shows the raised boss casting a shadow onto the base of the housing. Internal self-shadowing of the part is also visible.

19-26

Chapter 19 Learning to use PhotoWorks

Adding an Image Background

Areas of the image not covered by parts of the SolidWorks model are known as image

background. You can fill these areas with various patterns or images, thereby adding further visual interest and appeal to your PhotoWorks images.

Click the

Background

tab on the

PhotoWorks - Scene Editor

dialog box.

Notice that the

Style

is set to

Graduated

. The PhotoWorks software supports several background styles.

Under

Parameters

, make sure that

Top Color

is selected, then click

Edit

Select a color from the palette, then click

The

Preview

window is updated to show the change.

Modify the

Bottom Color

, if desired, observing the effect in the

Preview

window.

Now change the

Style

Clouds

Under

Parameters

, make sure that

Scale

is selected, then set

Number

to 2.

Modify the

Sky Color

Cloud Color

, and

Detail

parameters, if desired, observing the effect in the

Preview

window.

Other background options include scaled or tiled images, or plain colors.

The

PhotoWorks - Scene Editor

dialog box also includes a

Foreground

tab, from which you can select various styles of attenuation, to simulate atmospheric phenomena, such as fog and depth-cueing.

Click

Render

on the PhotoWorks toolbar, or click

PhotoWorks

Render

SolidWorks 2001 Getting Started 19-27

Special Topics

Creating Background Scenery

The visual effectiveness of your presentation can be improved still further by setting the part against a geometric backdrop, rather than simply leaving it suspended in space.

With the PhotoWorks software, you can create simple background scenery consisting of a horizontal base plane and vertical sides surrounding the part. You can control the size and position of the scenery relative to the part, and select materials for the base and sides.

The scenery dimensions are calculated from the bounding box of the SolidWorks model.

The scenery will never obscure the part. Only those planes visible behind the part will be displayed. Any reflective materials attached to the part will pick up and reflect color and texture from the background scenery.

Click

Scene

PhotoWorks

Scene

, then click the

Scenery

tab.

Under

Base

, do the following :

Select the

Display

check box.

b) c) d) e) f)

Notice that the default material,

Polished Plastic

, has been selected for the base.

Click

Edit

The

PhotoWorks - Material Editor

dialog box appears.

Expand the

Stone Textures

material archive, click the

Stone

class, then click the

Pink Marble

material to select it.

Click the

Under

Click

Scaling

Mapping

tab.

set both

Width

Under

Sides

, do the following:

Select the

Display

check box.

and

Height

to 65.00mm.

d) e) f) b) c)

Notice that the default material,

Polished Plastic

, has been selected for the sides.

Click

Edit

The

PhotoWorks - Material Editor

dialog box appears.

Expand the

Wood Textures

material archive, click the

Wood

class, then click the

Mahogany

material to select it.

Click the

Mapping

tab.

Under

Scaling

, set both

Width

and

Height

to 50.00mm.

Click

Under

Base size

, set both

Base width

and

Base height

to 125.00mm, to reduce the size of the base relative to the model.

Set

Base offset

to -25.00mm, to move the base closer to the model.

Set

Sides height

to 75.00mm.

Click

Render

PhotoWorks

Render

19-28

SolidWorks Animator

In this chapter, you create animations and animation files of the claw model using

SolidWorks Animator tools. This chapter discusses the following topics: q

Viewing the SolidWorks AnimationManager tab q

Animating a rotation with the Animation Wizard q

Animating an exploded view q

Scheduling motion q

Animating a collapsed view q

Creating a motion path q

Recording an animation q

Creating an animation file from screen captures

SolidWorks 2001 Getting Started 20-1

Special Topics

Getting Started with SolidWorks Animator

SolidWorks Animator is an add-in product, and it has its own AnimationManager tab.

Click

Open

and open

Claw-Mechanism.sldasm

, found in the directory

\installation directory

\samples\tutorial\animator

Animator

does not appear on the SolidWorks main menu bar, click

Tools, Add-Ins

The

Add-ins

dialog box appears.

Select

SolidWorks Animator

and click

The following Animator tools are now available:

•

The Animator menu appears in the menu bar.

• A

SolidWorks Animator Help Topics

item appears in the Help menu.

•

The Animator Controller toolbar appears above the graphics area.

Animation Wizard

Create Path

Traverse Path

Edit Path

First

Previous Frame

Stop

Play

Next Frame

Last

Loop

Record Animation

Turn off screen capture

Turn on screen capture

Click the AnimationManager tab at the bottom of the left pane.

The AnimationManager tab is displayed when SolidWorks Animator is available. The

AnimationManager display includes two sections. Each section lists the assembly components in a different manner.

•

Viewpoint - in the chronological order of the assembly creation

• Schedule - in the chronological order of the animation

Items (motion paths) are added to Schedule as you generate animations.

20-2

Chapter 20 SolidWorks Animator

Animating a Rotation with the Animation Wizard

The Animation Wizard helps you animate a rotation of the model through 360 degrees.

To create a rotation animation:

Click

Animation Wizard

on the Animation Controller toolbar or

Animator,

Animation Wizard

On the

Select an Animation Type

screen, select

Rotate model

, then click

Next

On the

Select an Axis of Rotation

screen, select the following.

•

Axis of rotation

- Y axis

•

Number of rotations

- 1

•

Direction

- Clockwise

NOTE:

The axes of rotation are as follows:

- around the horizontal screen axis

- around the vertical screen axis

- around the screen axis pointing out of the screen

Click

Next

On the

Animation Control Options

screen, select the following.

•

Duration (seconds)

- 10

•

Start Time (seconds)

•

At the close of the AnimationWizard

- Play animation

NOTE:

The setting for

Duration

is the time of replay from an

.avi

file, which may vary from the play time in SolidWorks.

Click

Finish

The model rotates 360 degrees.

SolidWorks 2001 Getting Started 20-3

Special Topics

Animating an Exploded View

The assembly already contains an exploded configuration. You can animate this exploded view using the Animation Wizard. You add the

Explode

animation at the end of the

Rotate

animation.

To animate an exploded view:

Click

Animation Wizard

on the Animation Controller toolbar or

Animator,

On the

Select an Animation Type

screen, select

Explode

, then click

Next

On the

Animation Control Options

screen, select the following.

•

Duration (seconds)

- 10

•

Start Time (seconds)

•

At the close of the AnimationWizard

- Play animation

NOTE:

Since the

Rotate

path begins at 0 and ends at 10 seconds, you set the

Explode

animation to begin (

Start Time

) at 10 seconds, after the rotation is completed.

In the AnimationManager Schedule section, note that only one motion path is created for

Rotate

. For

Explode

, each component has a separate path, and each path has the same start time, as set in

Start

Time

Click

Finish

The model rotates 360 degrees, then explodes the view.

20-4

Chapter 20 SolidWorks Animator

Scheduling Motion

You can edit the Schedule motion paths manually and set the scheduled times so that the components explode one at a time.

To schedule motion manually:

If necessary, click the AnimationManager tab , and click the beside

Schedule

to expand the motion path schedules.

At the end of each Schedule line, the starting and ending time of the motion appears in parentheses. Notice that all the

Explode

paths start and end at the same time. You want to schedule the parts individually so that they move one at a time to simulate a disassembly process: first the pins, then the claw, the rod, and the collar.

Select

- or -

Pin-2 Explode

, then click

Edit Path

on the Animation toolbar.

Right-click

Pin-2 Explode

and select

Edit Path

The

Edit Path

dialog box appears.

In the

Change Timing

section, change

Start time (sec)

to 20, then click

Pin-2 Explode

appears at the bottom of the list with the timing (20.00, 30.00) showing that Pin-2 starts moving at 20 seconds and stops at 30 seconds.

Repeat steps 3 and 4 for the other parts except

Pin-1 Explode

. Leave

Duration

at 10 for all the parts. Set the following start times:

Pin-3 Explode

Claw-1 Explode

Con-Rod-1 Explode 50

Collar-1 Explode 60

The Explode components appear in the Schedule list in chronological order.

Click

Play

or .

The model rotates 360 degrees, then explodes one part at a time.

SolidWorks 2001 Getting Started 20-5

Special Topics

Playing the Animation

You can move through the animation using the Animator tools as follows:

Action

Click

Play

Animator, Animation, Play

Click

First

Animator, Animation, First

Click

Last

Animator, Animation, Last

Click

Previous Frame

Animator, Animation, Previous Frame

Click

Next Frame

Animator, Animation, Next Frame

Result

Plays the animation from beginning to end

Moves to the beginning of the animation

Moves to the end of the animation

Single steps backwards from the end of the animation

Single steps forward from the beginning of the animation

Animating a Collapsed View

Animating a collapsed view is similar to animating an exploded view.

To animate a collapsed view:

Click

Animation Wizard

or .

On the

Select an Animation Type

screen, select

Collapse

, then click

Next

On the

Animation Control Options

screen, select the following.

•

Duration (seconds)

- 10

•

Start time (seconds)

- 70

•

At the close of the AnimationWizard

- Play Animation

Click

Finish

The model rotates 360 degrees, explodes one part at a time, then collapses.

20-6

Chapter 20 SolidWorks Animator

Creating a Motion Path

You use the

Move Component

tool on the Assembly toolbar to specify a motion path for animation.

To create a motion path:

Select

Collar-1

in either AnimationManager, FeatureManager, or the graphics area.

Click

Create Path

or .

The

Create Path

dialog box appears.

Click

Add Path Point

to set the current position as the initial position of the collar.

Leave the dialog box open. On the Assembly toolbar, click

Move Component .

In the graphics area, drag the collar up to a new position.

In the dialog box, click

Add Path Point

to set the current position on the motion path.

Select the

Repeat initial path point as final path point

check box so the collar returns to the starting position at the end of the motion path.

Set the

Start time (sec)

to 70 to place the motion path at the end of the previous animation, then click

Done

A warning message appears indicating that two or more paths are overlapping. By setting the starting time to 70, the new motion path overlaps the

Collar-1 Collapse

motion path.

Click

and click

Move Component

to display AnimationManager.

Note the red exclamation points beside all instances of

Collar-1

AnimationManager.

To fix the overlapping paths:

Select

Collar-1-3

, then click

Edit Path

on the Animation toolbar.

- or -

Right-click

Collar-1-3

and select

Edit Path

The

Edit Path

dialog box appears.

In the

Change Timing

section, change

Start time (sec)

to 80, then click

The warning exclamation points disappear.

To play the animation:

Click

Play

or . The model rotates, explodes, collapses, and finally the collar moves up and back down.

SolidWorks 2001 Getting Started 20-7

Special Topics

Recording an Animation

You can record an existing animation to a file of type

.avi

that you can play later.

To record an existing animation:

Click

Record Animation

or .

The

Save Animation to File

dialog box appears.

Set

Frames per second

, and click

Save

In the

Video Compression

dialog box, click

The animation plays as the recording occurs, which takes a few minutes.

To replay the animation from the .avi file:

In Microsoft Explorer, find

Claw-Mechanism.avi

in the same directory as the model.

Double-click the file name to play the animation in a separate window.

Creating an Animation File from Screen Captures

Use the part file

Claw.sldprt

to create an animation (

.avi

) file from screen captures.

To create an animation file from screen captures:

Open file

Claw.sldprt

, which is in the same directory as the claw assembly.

Drag the rollback bar to before the first feature,

Base-Extrude

, so that nothing appears in the graphics window.

Click

Turn on screen capture

capture

In the

Save Animation to File

dialog box, set

Frames per second

to 1, and click

Save

In the

Video Compression

dialog box, click

In the FeatureManager design tree, rebuild the part by dragging the rollback bar down the tree one feature at a time.

Click

Turn off screen capture

Animator, Screen Capture, Turn off screen capture

To replay the animation from file:

In Microsoft Explorer, find

Claw.avi

same directory as the model.

in the

Double-click the file name to play the animation in a separate window.

20-8

More about SolidWorks Functionality

SolidWorks 2001 offers a seamless integration with the Windows

environment, allowing you to benefit from its capabilities. It also allows you to include many add-in functions to enhance your productivity and efficiently manipulate the design environment. This section addresses some of these capabilities and functions.

For more information, see the SolidWorks 2001 Online User’s Guide.

Importing and Exporting Files

You can import and export files using tools other than IGES, DXF, and STL shown in

Chapter 18, “Importing Files / Using FeatureWorks Software.” Also included with the

SolidWorks software are the following translation tools: q

Solid, Surface, or Wireframe Standards. STEP, ACIS

, VDAFS, and DWG q

Graphics Standards. VRML, TIFF, Metastream

, CATIA

Graphics, Highly

Compressed Graphics, and ZGL q

Direct Translators. Parasolid

™

, Unigraphics

, Pro/ENGINEER

, Autodesk

Inventor

™

, Solid Edge

™

, and Mechanical Desktop

2D Sketching and Command Emulator

If you are familiar with 2D drafting with AutoCAD

using a command line interface, you can continue sketching in the same way by using the SolidWorks 2D Command Emulator.

This is available as a standard add-in. To activate the 2D Command Emulator, click

Tools,

Add-Ins

and select

SolidWorks 2D Emulator

By default the command insertion window is docked at the bottom of the screen, but you can move it to another position. To turn the visibility of the command line window on or off, click

2D Command Emulator

on the

View

menu. For more information about using the 2D Command Emulator, refer to the 2D Command Emulator Help online help.

More about SolidWorks Functionality

Object Linking and Embedding

You can use Object Linking and

Embedding (OLE) to take advantage of features of other applications while in a SolidWorks document. You can also link or embed a SolidWorks part, assembly, or drawing document to another OLE-compliant application.

For example, OLE allows you to bring data generated by another application, such as a word processing application, into the

SolidWorks application. Or, you may want to include a SolidWorks part in an another document, such as a product data sheet.

When using OLE, you can link or embed documents. Linking documents allows you to change the contents of a document in all places where it appears without having to edit each individual occurrence. Embedding a document allows you to keep any edits specific to the place in which you embedded it.

Rendering Models with the PhotoWorks Application

The PhotoWorks TM application is a photorealistic rendering application that lets you create realistic images directly from

SolidWorks models. The PhotoWorks application is a separately purchased addin to the SolidWorks 2001 application.

Like other add-ins, it is accessible by clicking

Tools, Add-Ins

Using the PhotoWorks application, you can specify model surface properties such as color, texture, reflectance, and transparency. PhotoWorks is supplied with a library of surface textures (metals, plastics, and so on) and, in addition, you can scan in and use your own bit-mapped surface textures, materials, scenery, and

logos. For more information, see Chapter

19, “Learning to use PhotoWorks.”

Engine subassembly: UAMZ

Identifying Features with the FeatureWorks Application

FeatureWorks TM is an application that recognizes a limited set of features on an imported solid in a SolidWorks part document. Once these features have been recognized, they are added to the FeatureManager design tree to be modified like any other SolidWorks features. The FeatureWorks application is primarily intended for machined parts and sheet metal parts.

The FeatureWorks application is a separately purchased and licensed application that can be ordered from the dealer from whom you purchased the SolidWorks software. The

FeatureWorks application is supplied as a SolidWorks dynamic link library (.DLL) add-in to the SolidWorks 2001 application, and is accessible by clicking

Tools, Add-Ins

For more information, see Chapter 18, “Importing Files / Using FeatureWorks Software.”

Animating Assemblies with the SolidWorks Animator Application

Like the FeatureWorks application, the SolidWorks Animator application is a separately purchased and licensed application. With the SolidWorks Animator add-in, you can animate and capture motion of SolidWorks assemblies.

The SolidWorks Animator application can generate Windows-based animations (.avi files) that you can play on any Windows-based computer. In conjunction with the PhotoWorks software, the SolidWorks Animator application can output photo-realistic animations.

The SolidWorks Animator application allows you to use: q

AnimationWizard - to quickly create a fly-around animation, an exploded view animation, or a collapsed view animation q

Motion paths - to explicitly create motion paths for various components in your

SolidWorks assembly

Building Piping Systems

Piping is available as a separately purchased add-in. The SolidWorks Piping software supports routing functionality for fabricated pipes. You model the path of the pipe by creating a 3D sketch of the pipe centerline.

The software uses the centerline definition to generate the pipe and elbow components for the route.

SolidWorks 2001 Getting Started

More about SolidWorks Functionality

The software makes extensive use of design tables to create and modify the configurations of routing components. The configurations are distinguished by different dimensions and properties.

You can add various types of fittings to the route, such as flanges, tees, crosses, and reducers. The fitting components must have configurations that match the pipe sizes.

Examining eDrawings

eDrawings eliminates the communication barriers that designers and engineers deal with daily. Compact and self-viewing, eDrawings are significantly easier to understand than standard 2D drawings.

The following innovative features give you the capabilities that you need to overcome common barriers to effective 2D drawing communication: q

Virtual Folding - Open individual views in a drawing and arrange them in any way you desire, regardless of how the views were arranged in the original drawing. Virtual

Folding enables the eDrawings recipient to print and export any subset of a drawing.

Hyperlinking - Navigate through views automatically, ending searches for views or details. Simply click on the view annotation. That section view or detail is immediately added to your layout. q

3D Pointer - Identify and match geometry in multiple views. It is much easier to interpret what you are looking at when comparing that same location in all other views.

Ultra Compact Files - Send eDrawings using email. Substantially smaller in size than the original files, eDrawings make it practical to send 2D drawings via email, even over slow connections. q

Built-in Viewer - View eDrawings immediately. Anyone with a Windows-based computer can view eDrawings. No additional CAD software or special viewers required. The eDrawing Viewer comes bundled with the eDrawing as a single email attachment. q

Animation - Demonstrate automatically how drawing views relate to each other.

Creating Websites

SolidWorks 3D Instant Website allows you to create a web page from your SolidWorks application. The web page is based on a template and style that you can customize. The default templates that come with SolidWorks 3D Instant Website include: q

An embedded Metastream viewer for parts and assemblies and an eDrawings viewer for drawings q

A comment section where multiple reviewers can offer opinions q

Your company’s contact information with a link to its home page

Additionally, you can create your web page on a password-protected secure site hosted by

SolidWorks. With this feature, you do not need your own web server to share your designs with others outside your company. You can also create your web page on a local or network drive.

SolidWorks Application Programming Interface

The SolidWorks Application Programming Interface (API) is an OLE programming interface to SolidWorks. The API contains hundreds of functions that can be called from

Visual Basic, VBA (Excel, Access, and so forth), C, C++, or SolidWorks macro files.

These functions provide the programmer with direct access to SolidWorks functionality.

For a detailed description of the API and a list of all the new functionality added to the

API since the last release of the SolidWorks software, refer to the API online help file.

Click

Help

SolidWorks API Help Topics

to access the API help.

There is also a detailed description of the API functions on the SolidWorks Web page

(http://www.solidworks.com/html/products/api).

SolidWorks 2001 Getting Started

More about SolidWorks Functionality

Collaborating with Others

SolidWorks offers many tools that allow you to work in a multi-user environment or to share your design with others. These tools include: q

SolidWorks 3D Meeting. SolidWorks 3D Meeting is a SolidWorks application that interfaces with Microsoft Windows NetMeeting

. It enables you to share SolidWorks

(or other applications on your system) with other users over the Internet.

SolidWorks 3D Instant Website. SolidWorks 3D Instant Website allows you to create a web page from your SolidWorks application. The web page can include an embedded viewer and a comment section where multiple reviewers can offer opinions.

Additionally, you can create your web page on a password-protected secure site hosted by SolidWorks. See Creating Websites for more information.

eDrawings. eDrawings is the first email enabled communications tool designed to dramatically ease the sharing and interpretation of 2D mechanical drawings. You can share eDrawings with anyone who has a Windows-based computer as the eDrawings

Viewer comes bundled with the eDrawing as a single email attachment. See

Examining eDrawings for more information.

SolidWorks Explorer. SolidWorks Explorer is a file management tool design to help you easily perform such tasks as renaming, replacing, and copying SolidWorks documents. See Managing SolidWorks Documents for more information.

FeaturePalette window. The FeaturePalette window help you organize and use library features, sheet metal forming tools, piping components, and other commonly used parts. You can store palette items anywhere you want on a network so you can share them with your colleagues.

Open from Internet server. You can open files residing on an Internet server. You can also modify then save the files back to an Internet server.

Copy Options Wizard. After you customize your SolidWorks software, you can use the Copy Options Wizard to copy the options information set by one user and specify the same options on the machines of other users.

Hyperlinks in notes. You can add an embedded hyperlink in a note, or you can add a floating hyperlink in any SolidWorks document. The hyperlink can be to a document on the Internet, on your local network, or on your own hard drive.

Reload/Replace. You can refresh shared documents to reload the latest version including any changes made by one of your colleagues. You can replace a referenced document with another document from anywhere you want on a network.

Search paths. When you open a parent document, the other documents that are referenced in the parent document are loaded into memory also. You can set the location where the SolidWorks software searches for referenced components to include shared folders for frequently used components.

Managing SolidWorks Documents

SolidWorks Explorer is a file management tool designed to help you easily perform such tasks as renaming, replacing, and copying SolidWorks documents.

SolidWorks Explorer is accessible from within the SolidWorks 2001 application. You can also open SolidWorks Explorer independently (by creating a shortcut on your desktop), and then open any SolidWorks documents from within SolidWorks Explorer.

To open SolidWorks Explorer from within the SolidWorks 2001 application, click

Tools,

SolidWorks Explorer

. SolidWorks Explorer allows you to: q

View document dependencies for drawings, parts, and assemblies, using a tree structure.

Copy, rename, or replace referenced documents. You have the option to find and update references to documents.

View data and previews, or input data, according to the function you have active.

Use the following tools in SolidWorks Explorer to perform these tasks:

View any SolidWorks document on your system using the

Preview

tool. It is similar to using the shortcut menu in Windows Explorer for a

Quick View

View and edit specific, custom, or configuration-specific properties using the

Properties

tool. It also displays system data such as when the document was created and when it was last saved.

List all external references for SolidWorks documents using the

Edit References

tool.

Locate assemblies, drawings, or parts that reference a designated SolidWorks document using the

Where Used

tool.

Search for SolidWorks documents that meet a specified criterion, such as a custom property value, using the

Properties Search

tool.

List, rename, or delete configurations in an assembly or a part document using the

Edit Configurations

tool.

List, edit, and open any existing hyperlinks in a SolidWorks document using the

Edit Hyperlinks

tool.

SolidWorks 2001 Getting Started

Index

3 point arc

7-2

3D sketch

17-2 change planes

17-2 coordinate system

dimensions

virtual sharps

adding boss

components to an assembly

4-4

dimensions to a drawing

5-5

dimensions to a sketch

drawing sheet

4-6 align. See mating

alignment condition in assembly

analyzing a design

anchor

animation collapse

explode

motion path

record to file

SolidWorks 2001 Getting Started

screen captures to file

SolidWorks Animator

toolbar

wizard

AnimationManager tab

annotations

datum feature symbol

geometric tolerance

note

surface finish symbol

arcs

tangent

analysis of dependencies

bottom-up design

creating

creating component in context

12-13

designing in context

12-3

dragging parts from another window

11-4

dragging parts from Windows Explorer

11-5

exploding

11-17

Index - 1

inserting components from files

11-11

lightweight components

origin inferencing

overview

referenced configuration

attach dimensions

automatic geometric relations

7-6

axis animation rotation

temporary

balloon inserting

options

base feature creating

loft

revolve

specifying depth

specifying end type

anchoring

editing

inserting

properties

saving

BOM. See bill of materials

boss adding

loft

sweep

cavity

scaling type

centerpoint arc

chain dimensions

changing

Index - 2

color of a part

circular pattern creating

equal-spacing

total instances

collapsing animation

assembly

FeatureManager design tree

11-5

components adding to an assembly dragging parts from another window

4-4,

11-4

dragging parts from Windows Explorer

inserting from file

derived

lightweight

properties

resolved

ConfigurationManager

configurations created by suppressing features

12-11

generated by design table 6-9

in parts

12-3

referenced in assembly

12-12

constrain all

18-5

constraint. See relation

context

12-13

convert entities 4-3, 8-6

copy component instance

copy and paste

countersunk hole

creating assembly

base feature

cavity

constant radius fillets

drawing

face blend fillets

fillets

loft

part

3-2 planes

revolve

sketch

3-2

sweep

7-5

thin feature

9-4

variable radius fillets

crosshatch

cut

datum feature symbol

defining relations

deleting design table

6-10

derive component part

design ideas

design table closing

configurations

editing

embedding in document

6-8

inserting new

6-7 using to control parameters

6-7

dialog box help

2-7

dimension-driven system

2-2

dimensioning standard

5-3

dimensions adding to a drawing

attach

chain

displaying names

linear

modifying in a drawing

5-6

SolidWorks 2001 Getting Started

modifying on a part

reference

renaming

witness lines

display dimension names

dimensions

feature dimensions

section view

toolbars

display/delete relations

dome

draft feature

drawing adding a sheet

adding dimensions

creating

moving views

printing

specifying a template

5-2

standard 3 view

5-4

views

5-4

drawing sheet format. See sheet format

DXF files

18-4

edges selecting hidden

9-5 edit animation path

assembly

bill of materials

color

in separate window

exploded view

part in assembly

sheet format

sketch plane

ellipse

equation used in a pattern

9-10

used with sketch dimensions

12-6, 12-8

Excel

Index - 3

creating a bill of materials

14-1

editing a bill of materials

14-5

editing design table

6-10

inserting new design table

6-7

saving a bill of materials

14-6

exploded view animation

assembly

extend sketch entity

external references

extruding base feature

boss

cut

midplane

offset from surface 10-8

with draft

16-2

faces selecting hidden 9-5 feature changing the name

defined

displaying dimensions

dome

hiding dimensions

hole wizard

linear pattern

loft

mirror

mirror all

naming

order

properties

suppress

sweep

unsuppress

feature handles

FeatureManager design tree

2-4

FeatureWorks

18-3

Index - 4

fillet adding

constant radius

face blend

sketch tool

variable radius

font, dimensions

foreshortened radius

format. See sheet format

getting help

help animation

design portfolio

in dialog boxes

online

online tutorial

tip of the day

tooltips

hidden in gray

hide feature dimensions

toolbars

IGES files

import

DXF files

18-4

IGES files

18-2

in-context

12-13

inferencing assembly origin

11-4

lines

7-2

inplace mating relation

12-13

inserting balloon

14-6

bill of materials in drawing 14-3

component

dome

loft

model items in drawing

new component

plane

revolve

installation allow changes from drawing

individual

procedures

server and client

system requirements

jog ordinate dimensions

label letter

layout sketch

leader

lightweight components, assembly

line

linear pattern

linking dimension values

6-3, 16-4

list external references

loft

8-5 ordering the sketches

mate components

mategroup

material properties, transparency

mating

coincident

concentric

distance

SolidWorks 2001 Getting Started

tangent

testing relationships

midplane extrusion

mirror

features

modifying

dimensions in a drawing

5-6

dimensions on a part

3-5, 3-15

mold creating a mold base part

16-5

cutting

16-9

inserting the design part

16-6

moving bill of materials

14-4

drawing views

5-4

named view adding to a drawing

naming features

new assembly

part

3-2

offset entities

online help

online tutorial

opening new part document

3-2 sketch

3-2 options

automatically load parts lightweight

balloons

bill of materials

5-3 dimensioning standard

5-3

display dimension names

6-3

drawings

13-4

edit design tables in separate window

6-7

font, dimensions

5-3

Index - 5

name feature on creation

show dimension names

ordinate dimensions

origin assembly

output to image file, PhotoWorks

19-12

over defined sketch

3-4

part

configurations 12-11

creating

3-2 opening new document

3-2 saving

3-7

path, sweep

7-5

pattern circular, defined

linear, defined

mirror all

PhotoWorks background scenery

19-27, 19-28 creating a backdrop

decals

19-12 saving image file 19-12

view image file

planes

copying

creating

offsetting

plotting drawings. See printing drawings

preview dimension

section view

printing drawings

profile detail view

loft

properties

bill of materials

dimension

Index - 6

dimensions

note

sheet format note

PropertyManager

recording an animation

20-8

rectangle

3-3

reference plane 8-2

referenced configuration

12-12

references, external

16-8

regenerate. See rebuild

relation adding

coincident

collinear

concentric

constrain all

coradial

defining

display/delete

equal

external information

geometric

midpoint

relationship coincident mating

concentric mating

distance mating

inplace mating

parallel mating

tangent mating

renaming dimensions

features

resolved components, assembly 11-3

revolve

rollback

rotate view

saving

drawing

drawing template

part

scale detail view

sheet

schedule, animation

section

view

selecting hidden edges

9-5 hidden faces

9-5 other

9-5

shared values

sheet adding to drawing

show dimension names

feature dimensions

sketch

defined

opening a new sketch

3-2

status

sketching

3 point arc

centerpoint arc

ellipse

extend

tangent arc

trim

SolidWorks 2001 Getting Started

slice. See section view

SmartMates

flip alignment

SolidWorks 2001

SolidWorks Animator

standard 3 view drawing

status bar

suppress feature

surface finish symbol

sweep

path

section

system requirements

tab

AnimationManager

ConfigurationManager

tangent arc

template, drawing

temporary axis

thin feature

tip of the day

toolbars

display or hide

tooltips

transparency

trim

tutorial

unsuppress feature

update view

verify relations

exploded

label

Index - 7

view image file, PhotoWorks

viewpoint, animation

virtual sharps

zoom

Index - 8

Hello! I've reviewed the SolidWorks 2001 Getting Started manual and I'm ready to answer your questions about SolidWorks 2001. I can provide information on creating parts, building assemblies, detailing drawings and more. Ask away!

Show related prompts

Assistant typing

Assistant is out of keyboard. Please, try again later.

Key features

3D part creation
2D drawing generation
Assembly creation
Dimension-driven system
Feature-based modeling
Sketch-based feature creation

Frequently asked questions

SolidWorks 2001 is mechanical design automation software used for sketching ideas, experimenting with features, and producing models and detailed drawings.

SolidWorks 2001 models consist of parts, assemblies, and drawings. These are created using features and sketches.

The SolidWorks 2001 Setup Wizard located on the CD-ROM will guide you through the installation process. You will need a serial number and a registration code.