I
N
T
R
O
D
U
C
T
I
O
N
This manual is the User's Guide for the NC-CAM 6 Drill and
Router Programming System for personal computers running
Microsoft Windows NT, Windows 95, Windows-98 Windows
2000 and Windows XP Proffesional. NC-CAM 6 provides a
mission-specific workstation approach to printed circuit board drill
and router program engineering. By concentrating exclusively on
the drill and rout processes, this system is able to offer a much
more highly evolved set of problem-solving tools than are
available on general-purpose CAM systems. It does this while
maintaining the ease of use typical of Windows programs.
While NC-CAM is an integrated drill and router programming
system, it is also made available with only the drill or only the
rout functions enabled. This User's Guide covers all NC-CAM
functions for both drill and rout programming, however it is
organized to allow you to easily distinguish which chapters apply
to the options you have installed.
What’s in this manual
This book is divided into three parts:
Part 1: NC-CAM Basics
„ Chapter 1, “NC-CAM: An overview,” describes the basic
functions NC-CAM performs.
„ Chapter 2, “System walkthrough,” gives a quick tour through
the features of NC-CAM 6 CAD, RoutEdit, and DrillEdit.
„ Chapter 3, “Using the CAD and RoutEdit modules,” gives a
step-by-step tutorial of rout programming.
„ Chapter 4, “Using the DrillEdit module,” gives a step-by-step
tutorial of drill programming.
Introduction
1
Part 2: Command
references
„ Chapter 5, “CAD command reference,” documents each of
the commands in the CAD module.
„ Chapter 6, “RoutEdit command reference,” documents each
of the commands in the RoutEdit module.
„ Chapter 7, “DrillEdit command reference,” documents each
Part 3: Appendices
of the commands in the DrillEdit module.
„ Appendix A, “In case of difficulty,” addresses potential
installation and configuration problems.
„ Appendix B, “Frequently-asked questions,” is a collection of
the questions and answers which occur most often with new
NC-CAM users.
2
NC-CAM 6 User's Guide
Typefaces and icons in this book
The different typefaces in this manual are used as follows:
Monospace
This typeface represents text as it appears on the
screen, and anything you must type.
Italics
Italics are used for emphasis and to introduce
new terms.
KEYCAP
This typeface indicates a key on your keyboard.
It usually indicates a specific key you should
press; for example, “Press ESC to cancel a
menu.”
Menu commands reached by a sequence of selections, for
example closing a file, will be shown in italic type, separated by
forward slashes. Hence, the main menu command for closing a
file will be shown as File | Close. Note that the “hot keys” used
to select the choices from the keyboard (i.e. ALT+F and ALT+C) are
shown in boldface.
The lightbulb icon is used to point out special tips and ideas for
using NC-CAM more efficiently.
The mouse icon is used to indicate functions which require the
use of the mouse.
The lightning icon is used to point out tips for more efficient
drilling and routing.
The “attention” arrow is used to draw your attention to especially
important points.
Introduction
3
Supported equipment
Here's what you need to run NC-CAM:
Computer. NC-CAM is designed to run on PC-compatible
computers, running the Microsoft Windows-NT (WinNT),
Windows-95 (Win95), Windows-98 (Win98) or Windows 2000
operating system.
Memory. To run NC-CAM, you'll need at least 32 megabytes of
RAM. This figure should be considered to be minimum values
only:
Disk space. Installing NC-CAM requires that your computer
have at least eleven megabytes of free disk space available. The
performance of Windows will suffer any time less than 40
megabytes are free after installing NC-CAM.
Printer port. NC-CAM is a secured application, and its
authorization lock must be installed on an IBM-compatible printer
port. (The port remains usable for driving a printer).
A three-buttoned mouse
make running CAD
much, much faster.
4
Mouse. Your computer must have a two or three-button mouse.
A three-button mouse is highly recommended for users who will
regularly be creating new CAD drawings for routing.
NC-CAM 6 User's Guide
How to contact FASTechnologies
FASTechnologies offers several types of technical support, both
directly from FASTechnologies in the USA, and from its dealers
overseas. In order to receive technical support, you must register
your copy of NC-CAM with FASTechnologies. Be sure to
contact FASTechnologies for you temporary authorization codes
as soon as you install NC-CAM.
Resources in your
package
This package contains several resources to help you:
This manual provides information on every aspect of NC-CAM.
Use it as your main information source.
NC-CAM features context-sensitive help. You may press the F1
function key at any time. If NC-CAM can determine the exact
function you're trying to use, it will pop up help on that topic.
Otherwise, pressing F1 will give you the help index.
Many common questions are answered in Appendix A, “In case
of difficulty,” Appendix B, “Frequently Asked Questions,” and
the README.TXT file located in the program directory.
FASTechnologies
resources
FASTechnologies has offers real-time technical support via
telephone, email & fax. New users are automatically entitled to
free technical support for a period of ninety days following
installation. Technical support may be reached in the USA at
763-763-0611, and the lines are staffed from 08:00 to 16:00 hours
US central time (usually the same as Greenwich Mean Time
minus 6 hours). If you're calling from outside the US, please
leave a FAX number for your reply.
Technical support is also available via FAX, at USA 949-2036483, and EMAIL, “support@fastec.com”. Please include your
product serial number and revision (as shown on your File | About
menu) on all faxed and emailed technical support inquiries.
Introduction
5
6
NC-CAM 6 User's Guide
P
A
R
T
1
NC-CAM basics
Chapter 1, NC-CAM: An overview
7
8
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
1
NC-CAM: An overview
This chapter introduces you to some of the basic procedures
involved in using NC-CAM, and what its capabilities are.
There's a special section for those who have used earlier
versions of NC-CAM. The chapter also describes:
„ how to start NC-CAM
„ how to enter security codes
„ the parts of the NC-CAM 6 desktop
„ how layers and modules are related
„ how to get onscreen help
„ how to exit NC-CAM
After reading this chapter, you should be able to run NC-CAM,
navigate through its menus and modules, obtain help on its
functions, and exit NC-CAM. You should also have a basic
understanding of the functioning of NC-CAM's layers and
modules.
Chapter 1, NC-CAM: An overview
9
NC-CAM's capabilities
NC-CAM was designed specifically to work with CNC drill
data, CAD drawings for rout programming, and CNC rout
programs, in either metric or inch measurement units. It allows
you to import data from a variety of sources, graphically edit in
CAD, drilling, and routing modes, and output production-ready
CNC programs. Unlike general-purpose artwork CAM systems,
the needs of the drill and rout processes are given top priority at
every stage of the operation of NC-CAM. The jobs you'll make
with NC-CAM are the highest-quality CNC programs available.
The system's CNC focus, and the resulting high quality output,
begin with the way NC-CAM stores your coordinates.
In NC-CAM, all coordinate data is stored in integer form at a
resolution of one nanometer (0.000001 millimeter, or about
0.00000004 inch). If this resolution sounds incredibly small, it
is: One nanometer is roughly the width of five hydrogen atoms
lined up side-by-side. Why such extreme resolution? Because
in printed circuit board manufacturing, there is often the need to
switch between metric and inch measurement units. In the
floating-point databases often used in other CAM systems,
switching units is just one of many ways that data can be
corrupted by math round-offs.
nanometer resolution
means no round-offs
Because NC-CAM always stores your coordinates in
nanometers, it is not possible to cause NC-CAM to destructively
round off coordinates. When you switch between inch and
metric units, your coordinates are not actually changed at all,
they're just displayed (and output) in the units of your choice.
Thus, you may freely switch between inch and metric with no
accuracy penalty of any kind.
When you start up NC-CAM, you'll notice that the work area
shown on-screen is square. This is because NC-CAM's
nanometer database has a maximum range of 2.4 meters (about
+/-42 inches). Limiting the work area this way allows NCCAM to use very fast database and display math, and it is
adequate for almost all known PWB fabrication needs.
10
NC-CAM 6 User's Guide
Starting NC-CAM
When you're ready to begin working with NC-CAM, find and
select the NC-CAM icon. The first time NC-CAM is executed,
you may see the “Lock Menu,” as shown below. (If you don't
see the Lock Menu, but instead see NC-CAM's splash screen,
just skip the next few paragraphs).
the NC-CAM icon
The first time you run
NC-CAM in a new
installation, or if you're in
an evaluation period
which has expired,
you'll see this
Authorization dialog.
Check your serial
number
no serial number means
the lock isn't working
If you do get the “Lock Menu” when you run NC-CAM, the
first thing to look for is the serial number. If you don't see a
serial number, you may see a message saying “Unauthorized
version.” The “Unauthorized version” message means that NCCAM cannot communicate with its printer port software lock. If
this happens on your machine, you should double-check your
NC-CAM installation instructions, and perhaps consult
Appendix A, “In case of difficulty.” Of course, you may also
contact FASTechnologies Tech Support (see page 5). In any
event, you will not be able to proceed until you get NC-CAM to
display your lock's serial number.
Chapter 1, NC-CAM: An overview
11
Authorization
codes
When you see the authorization menu, you will need to enter the
authorization codes which your NC-CAM software needs in
order to run. If you received your NC-CAM 6 package directly
from FASTechnologies, or if it came from a dealer, just contact
FASTechnologies, and we will FAX or EMail codes to you.
first check your
date and time
12
Before you enter any authorization codes into NC-CAM, it's very
important that you check your PC's time and date, to make sure
they are correct. The NC-CAM lock has a built-in clock, which
must agree with the PC's clock within reasonable limits. So make
sure your PC is set to the correct date and time (including the a.m.
or p.m. setting) before entering your authorization codes.
NC-CAM 6 User's Guide
check the serial
numbers, then enter
your authorization codes
When you receive authorization codes from FASTechnologies,
they will refer to a specific NC-CAM serial number. Just in case
your company owns more than one FASTechnologies product, you
should check to see that the serial number supplied with the
authorization codes matches the lock serial number displayed on
your authorization menu. If there's a mismatch, contact
FASTechnologies with the serial number shown on the menu, so
we can correctly register which software you're using
with which software lock. We may also need to supply you
with new authorization codes for the appropriate lock serial
number.
NC-CAM software security codes come in two types; temporary
and permanent. Temporary codes consist of both a number of
days and a ten-digit code number. The temporary codes are
issued when you first install a new copy of NC-CAM. Later,
after any evaluation period is completed, FASTechnologies will
supply you with permanent authorization codes.
Note that there are three different authorization codes used in
NC-CAM, one for each of the three modules; drill, rout, and
CAD. To enter the codes for a module, use the TAB key or your
mouse to select the menu boxes adjacent to the name of the
module. If you're entering a temporary code, first enter the
number of days in the “days” column. If you're entering a
permanent code, just leave the “days” column blank.
Enter the ten-digit authorization code in the “code” column.
You may enter codes for all three modules at once. When
you're done entering your codes and you've verified them, press
the OK button.
Chapter 1, NC-CAM: An overview
13
Insure your lock!
New users of NC-CAM often ask one or two questions about
the software lock. As this is an important topic, we'll address
the questions here in the introductory section of the manual.
Question #1, “Why is this software locked?” The answer to
this question is simple: If FASTechnologies did not lock its
software, many companies would run more copies of the
program than they've paid for, and some companies would copy
it but wouldn't pay for it at all. The market for this specialized
software is small (about 1,200 copies worldwide), and the cost
of creating it is high (over $800,000 so far). If
FASTechnologies didn't get paid for each copy of NC-CAM, we
would quickly go bankrupt. We prefer to continue to develop
new generations of NC-CAM for you to use.
Your lock is your
NC-CAM system!
add the software lock
to your business
insurance!
14
Question #2, “What happens if I lose my software lock?” This
answer is also simple: A replacement NC-CAM lock will cost
you over ten times its weight in gold! If you lose your lock,
first file an insurance claim, then call FASTechnologies. We'll
exchange your lock for free if it should fail, but if it turns up
missing, you'll have to buy a new copy of the product. Your
lock is your NC-CAM system. We strongly recommend that
you take reasonable precautions against the loss or theft of your
software lock. You should also have the software lock
explicitly listed at full value in your business insurance policies.
NC-CAM 6 User's Guide
The NC-CAM
screen
edit drill, rout, or CAD
by just clicking
the layer buttons
Once your software is authorized, you'll see the NC-CAM
screen shown above. The display will look familiar to those
who have experience with NC-CAM 5, because the NC-CAM 6
display resembles the CAD display in NC-CAM 5.
editing commands are
accessed by icons,
pulldown menus,
or two-letter shortcuts
In NC-CAM 6, most of the editing functions for CAD, rout, and
drill are available in three different ways: By selecting an icon
on the toolbar (to the right), by pulling down a choice from the
main menu (at the top), or by typing a two-letter shortcut into
the command window (at the bottom). This choice of three ways
to enter commands was extremely popular in the NC-CAM 5
CAD editor, which is why the CAD interface model has been
extended to both rout and drill editing in NC-CAM 6.
Chapter 1, NC-CAM: An overview
15
NC-CAM's desktop
The figure below describes NC-CAM's desktop. Each part of
the desktop is described in more detail in the following pages.
Main menu: gives you access to all commands. The choices
change to match the type of layer you select; CAD, rout, or drill.
Layer
buttons:
The pressed
button
indicates the
selected layer
and module:
0-29 for CAD,
D0-9 for drill,
R0-4 for rout.
Status line: shows the time
of day, shortcut commands
for the toolbar icons,
and the cursor's X:Y.
16
Toolbar:
editing
icons for
the type
of layer
you've
selected:
CAD, rout,
or drill.
Workspace: shows the layers
of the selected module in
color, others in grey. Colors
may be changed by choosing
Layers on the main menu.
Command window: shows the
current editing command, lets
you enter and edit command
parameters.
NC-CAM 6 User's Guide
The layer buttons
These are the most important buttons in NC-CAM. When you
left-click a layer button, you select two things. First, the pressed
layer button determines the selected module (drill, rout, or
CAD). The selected module determines the type of data you can
edit. Secondly, the layer button determines the selected layer.
The selected layer is the layer you're allowed to edit.
The layer buttons (on the left side of the screen) control both the
display in the workspace and the editing mode. When you leftclick on a layer button, you have made that layer the selected
layer. When a layer is the selected layer, you may create, alter,
and delete individual drawing items on that layer.
The first thirty layers, numbered zero through twenty-nine, are
CAD drawing layers. When you select one of the CAD layers,
the CAD tools will appear on the toolbar, and the CAD choices
will appear on the main menu.
The layers numbered “D0” through “D9” are drill layers. When
a drill layer is the selected layer, the drill tools and choices will
appear on the toolbar and the main menu.
The layers numbered “R0” through “R4” are rout layers. When
a rout layer is selected, the rout tools will appear in the toolbar,
and the rout choices will appear in the main menu.
The toolbar
The toolbar lets you select individual editing functions by
clicking icons. The icons will change when you select CAD,
rout, or drill layers on the layer buttons. If you want to know
the name of an icon's function, place your mouse over the icon
and hold it there. The button's description will appear in the
status line.
Toolbar functions may also be selected by choosing a menu item
from the main menu, or by typing the function's two-letter
shortcut into the command window.
Some of the buttons on the toolbar are modal. This means that
when you press a button, it stays down, and the function is
repeated until another button is selected. The modal buttons
generally create or change drawing items.
Chapter 1, NC-CAM: An overview
17
Many buttons on the
toolbar stay down until
you press another.
If you're ever in doubt about which function is currently in
effect, check the command window at the bottom of the screen.
The currently-selected command will always be shown there,
next to the “>” prompt
The command
window
The command window shows the current editing command.
There's also a command prompt “>” where you can type in
keyboard commands and coordinates.
Any time NC-CAM is expecting a coordinate, you may enter an
X:Y coordinate pair on your keyboard. For instance, if you
want to draw a line from X=1,Y=1 to X=2,Y=2, first you would
select the command Create Line. Then you would type 1,1 and
press ENTER. Then you would type 2,2 and again press ENTER.
Hand-entering coordinates allows you to duplicate the
coordinates exactly as they exist on a blueprint.
Note that when a command is already selected, you may type in
a different a new two-letter command. This will cancel the
current command and activate the new one.
The parameters for the
advanced functions are
shown in blue. Just click
on them to edit them.
Some functions, such as the [MC] Matrix Copy command have
several parameters. In the case of Matrix Copy, there are
horizontal and vertical steps, and horizontal and vertical
quantities. Parameters like these are also displayed in the
command window, with their names in black, and their values in
blue. Any number shown in blue in the command window may
be clicked with the mouse and then changed with the keyboard.
The status line
The status line contains several pieces of information. First,
there is the system clock, which shows the system time. Then
there’s the hint area, which shows the function and two-letter
shortcut for the toolbar buttons when you move the mouse over
them. Finally, the coordinate display on the right side of the
status line shows the X and Y location of the mouse cursor as
you move it through the workspace area.
18
NC-CAM 6 User's Guide
The main menu
This drop-down style menu gives you access to all the functions
of the selected module. The selected module is determined by
which layer button is currently depressed. Many of the
functions on the main menu are not available from the toolbar or
with two-letter command window shortcuts.
In order to get context-sensitive help on a main menu choice,
you must first highlight it. (This is most easily done by using
the keyboard arrow keys.) When a main menu choice is
highlighted, you get help by pressing function key F1.
Note that the system-wide file management functions are always
accessable on the File pulldown, regardless of which module
(DrillEdit, RoutEdit, or CAD) is selected.
The workspace
The workspace area is where all the features contained in NCCAM’s database are displayed. The workspace area is 84
inches square, with 42 inches to travel in the positive direction,
and 42 inches in the negative direction. Note that the
orientations of the X and Y axes in the workspace are usersettable, with the View | Version function. This is especially
useful in cases where the CNC machines are set up in one of the
seven nonstandard axis versions.
drag the
workspace display
by holding the ALT key
The scrollbars at the side and bottom of the area determine
which part of the workspace you are currently viewing. You
may pan the screen by using the scrollbars, or by using the
“magnifying glass” icons on the toolbar. You may also simply
drag the workspace view with your mouse by first holding the
ALT key, and then dragging in the workspace while holding
down your left mouse button.
Chapter 1, NC-CAM: An overview
19
DrillEdit , RoutEdit, and CAD layers
NC-CAM 6 consists of three different modules, DrillEdit,
RoutEdit, and CAD, which may be purchased separately or in
any combination. In NC-CAM, each module uses its own
layers. There are thirty CAD layers, nine DrillEdit layers, and
five RoutEdit layers.
When you select a layer by clicking on its button, you're also
automatically selecting the editing module for that layer. Click a
CAD layer, and the CAD module is automatically selected.
When a drill layer is selected, the DrillEdit module is selected,
and when a rout layer is selected, the RoutEdit module is
selected. You can always tell which module is selected by
looking at NC-CAM's title bar: It'll say “DrillEdit,” “RoutEdit,”
or “CAD.”
The workspace displays the data on all layers, but the data in the
unselected modules is shown in grey. The data in the selected
module is shown in different colors, one for each layer in that
module.
20
new things go to the
layer that's selected on
the layer buttons
When you create new things, whether they're CAD lines, drill
holes, or rout cuts, they go to the selected layer. When you
choose edit functions which change things, they generally
change things only on the selected layer. So, where making and
changing individual things are concerned, the selected layer acts
like it's the only layer.
if you can see
something, you
can snap to it
The snap functions allow you to use existing points, lines, arcs,
and circles to define positions when you're creating or changing
things. You can snap to anything you have displayed in the
workspace. For example, you can snap a drill hole to the end of
a CAD line, etcetera.
window operations can
affect all layers in the
selected module
By default, window operations like delete, move, copy, and so
on, affect all of the layers in the selected module. This way, you
can make window changes to all of the layers in CAD, drill, or
rout at the same time. (It's not possible to change data of all
three types at once, however).
NC-CAM 6 User's Guide
Shutting layers
off
For special occasions, it is possible to “shut off” individual
layers in the selected module, so that window operations like
delete, move, and copy will not affect those layers. If you want
to shut off just one layer, do this by right-clicking its layer
button, to get the following dialog.
When you right-click a layer button, you'll see the dialog shown
above. To shut off the layer, click off the checkbox labeled
“ACT.,” and then press OK. That layer is now inactive, and it
won't be affected by window edits.
You may hide a layer by clicking the checkbox labeled “DIS.,”
which makes the layer invisible. Doing this automatically shuts
off the checkbox labeled “ACT.,” so you won't accidently
window-change data you can't see.
When you want to check on all of the layers in NC-CAM at
once, you may select Layers | Layer Control button on the main
menu. This brings up a large dialog containing “ACT.” and
“DIS.” buttons for all of the layers at once.
The button labeled “C” pops up the layer's color dialog. The
foreground color of each layer can be set independently in this
dialog. There's only one system-wide setting for the workspace
background color, however. The background color setting is
found by selecting File | Options.
Chapter 1, NC-CAM: An overview
21
Layer modes
Layers have four different modes; disabled, displayed, active,
and selected.
The first mode, disabled, means not displayed and not active.
When a layer is disabled, it is hidden, and it can't be changed.
The items on disabled layers remain exactly the same, unless
you select File | New, which erases all layers.
The second mode, displayed, means displayed but not active.
The layer is shown on the screen, in color if the layer belongs to
the selected module, or in grey if it's not in the selected module.
When a layer is only displayed but not active, you can snap to
the items on the layer, but the layer cannot be changed.
The third mode is active. When a layer is active, it's always also
displayed. Items on an active layer can be used in snaps, and
they can also be changed with any of the window editing
commands. Window editing commands include delete, move,
scale, copy, and so on.
The fourth mode is selected, indicated by the layer button. Only
one layer button can be selected, and the selected layer is always
both displayed and active. Newly-created entities are created on
the selected layer. In CAD, when you do a Create Line, or any
other operation that adds an entity to the database, will be placed
on the selected layer. On drill or rout layers, anything that
creates database entities (such as AutoRout or Drill Hole) will
create those entities on the selected layer. In addition to this, the
selected layer also determines the selected module, DrillEdit,
RoutEdit, or CAD.
Layer colors
You can change the color in which each layer is shown by
clicking on the button simply labeled “C” in either the individual
layer's control dialog, or on the main menu Layers | Layer
Control dialog. To get an individual layer's control dialog, you
must right-click on its layer button.
22
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
2
System walkthrough
Introduction
This system walkthrough assumes that the shipping defaults for
NC-CAM 6 are still in effect. For example, the input data is
formatted assuming that the program is running in Inch mode and
not in Metric mode.
Note that this system walkthrough will highlight features of all
three modules of NC-CAM. Therefore, if your system is not
authorized to run one of the modules, you will want to skip over
the sections applying to the module(s) you don't have.
Starting NC-CAM
Find and select the NC-CAM icon.
After a few seconds, the program will display a dialog. If your
copy of NC-CAM has already been authorized to run, this dialog
will be a splash screen, which displays how many trial days are
remaining.
Chapter 2, System Walkthrough
23
Otherwise, a lock dialog will be displayed, where you will need to
enter security codes that you have received from
FASTechnologies. For more help on entering security codes, see
Chapter 1. When the software is authorized, you can click on OK
to continue. The NC-CAM 6 desktop will be displayed, with the
words “NC-CAM 6” and a module name “CAD”, “DrillEdit”, or
“RoutEdit” displayed at the top.
NC-CAM remembers which layer you had selected the last time
you ran it, and starts up with the same layer selected.
24
NC-CAM 6 User's Guide
Loading CAD
data
This walkthrough takes you through many stages of what would
have to be accomplished to take a CAD drawing for a rout
program from a customer and produce a production-ready CNC
program for routing. The first step in this process is to load the
CAD drawing into the CAD module, which can be accomplished
by chosing the File | Import menu item from the main menu. The
familiar “open” dialog will be displayed, with the title “Select file
to import.”
Select the file “6SAMPLE.DXF” for importing by clicking on the
name of the file, and then clicking on the Open (or OK) button. A
“File Format” dialog appears, to verify the format of the file that
you have selected.
NC-CAM has identified that this is a DXF file, so you can click
on OK to proceed with importing the file.
Chapter 2, System Walkthrough
25
The “DXF File Units” dialog appears next. (This is needed since
the unit flags in DXF files are often misleading). The sample file
uses inch units, so you can again click on OK.
As shown below, a CAD drawing should now appear in the work
area.
As you can see, the sample DXF file contains a board outline on
only one CAD layer. When you import DXF files having multiple
layers, you'll see the data on the different layers displayed in
different colors.
The NC-CAM desktop is resizable, to allow you to take
advantage of as much of your computer's screen as possible. If
you need to view another application while running NC-CAM,
simply resize NC-CAM down to its smallest size by dragging one
of the corners of the window towards the opposite corner. The
program will shrink down to a fixed minimum size.
26
NC-CAM 6 User's Guide
In order to examine the data in fine detail, it makes sense to use
as much of your computer's screen as possible. To do this, click
on the “Maximize” button at the upper right corner of the desktop.
Once the desktop is as large as you desire, select View | Zoom All
from the main menu.
The View | Zoom All function is available in every NC-CAM
module. Choosing it will cause NC-CAM to display the work
area in the highest resolution possible. In other words, it will
make the drawing as large as possible, so that you can see the
entire drawing in fine detail. Investing in a high-end monitor and
video card can make a huge difference in the amount of detail that
can be seen in your drawings. A display that can reach a
resolution of 1024 by 768 pixels provides much more detail than
one that can display only 640 by 480 pixels. It should be noted
that NC-CAM 6.0 uses only the Windows standard 16 colors, so
setting your computer to video modes with more colors will not
enhance the NC-CAM display.
Chapter 2, System Walkthrough
27
The 6SAMPLE.DXF drawing has a problem very common to
customer-supplied rout-path drawings. Select View | Const Points
from the main menu to see “X” symbols at the ends of every
entitiy, and at the centers of arcs and circles.
The arcs in this drawing are not true arcs, but are instead drawn
with hundreds of small lines. These are known as “chorded
arcs,” meaning that straight-line chord segments are used in place
of true arcs.
28
NC-CAM 6 User's Guide
To see how bad the drawing data is, select File | Get Info from
the main menu. A dialog labeled “Drawing Statistics” will
appear.
Note that NC-CAM reports that the drawing is made of 1,103
lines, and no arcs. Click on OK to continue.
In order to prepare this drawing for rout processing, you will need
to create true arcs in the place of the chorded arcs. In most
cases, NC-CAM can accomplish this task with terrific ease.
Select Modify | Automatic Cleanup from the main menu, and the
“Clean Up Drawing” dialog will appear.
Enable each of the cleanup tasks with the checkbox next to each
name. Three of the tasks each require a parameter, which is a
measure of how much the task is allowed to change the drawing.
The parameters should all be set to 0.0020 inches, for now. Click
on OK to continue with Automatic Cleanup.
Chapter 2, System Walkthrough
29
Once the Automatic Cleanup tasks have completed, a “Drawing
Statistics” dialog will be displayed.
Note that 1090 entities have been deleted! Although the drawing
looks the same, there are now only 21 lines and 7 arcs. Working
with 28 entities is significantly easier than working with 1,103.
Also, the arcs are now true mathematical arcs, and could be
edited as such. Click on OK to exit this dialog. Select View |
Const Points to turn off the construction point display.
30
NC-CAM 6 User's Guide
NC-CAM saves all changes that you make, so that you can easily
“un-do” any mistakes. The advantages of being able to revert
your work back to a stage before you made any mistakes are
obvious. The disadvantage is that if you modify many entities,
such as by doing a Matrix Copy of your entire drawing, and then
undo your work, many “deleted” entities have been stored in
memory, and will remain there as long as you edit the drawing.
Select File | Pack Database from the main menu to eliminate all
of these deleted entities from the database. Remember, though:
After you pack the database, you will not be able to undo any
previous changes!
Chapter 2, System Walkthrough
31
Routing from
CAD data
Select the first rout layer, “R0” by clicking on the R0 layer button.
The title bar now says “RoutEdit,” and the buttons in the toolbar
have changed to allow rout editing. In this section, we’re going to
rout the board outline first, and then we'll create the internal routs.
When this is done, we’ll edit the sequence to make the internal
cuts first, to show you how to re-sequence rout cuts in NC-CAM.
32
NC-CAM 6 User's Guide
Usually, it makes sense to rout the outside of the board with a
large cutter. To select the cutter, select Modify | Cutter Config
from the main menu.
There is one set of tools for each RoutEdit layer. Since R0 is the
layer we're working on, leave the R0 tab (at the top of the dialog)
selected.
As you can see, default values are already in effect. Tool 1
should have a diameter of 0.032 inches. Tool 2 should be 0.062,
Tool 3 should be 0.093, and Tool 4 should be 0.125 inches. An
0.062 cutter will work fairly well, so Select Tool 2 in the left-hand
side of the dialog. Note that the compensation jumps to Tool 2, as
well. Click on OK to exit this dialog.
Chapter 2, System Walkthrough
33
Almost all routing is done with right compensation, so select
Modify | Compensation | Right from the main menu. For the
outside of the panel, you can use the Auto Rout Outside function
to generate a good rout path. Select Edit | Auto Rout Outside
from the main menu. You will almost always want to change the
parameters for Auto Rout, so select Modify | Auto Rout Config
from the main menu, and a dialog labeled “Auto Rout Settings”
will appear.
Click on the top drawing, which has the text “CORNER” in it. It
should stay down, to indicate that it is selected. For this rout,
only the A and B parameters are used, as can be seen in the
selected diagram. Set Plunge Offset (A) to a value of 0.031
inches. Set Overcut (B) to 0.031 inches. Since the C value is not
used, you can leave the Edge Offset (C) value as it is. Click on
OK to continue with routing.
34
NC-CAM 6 User's Guide
Most NC-CAM commands that take coordinates as input can take
either a mouse click (or mouse drag), or they can take typed
values in the command window. In this example, you will select
the bottom right edge to begin the Auto Rout. If you were to click
on it with the mouse, you would want to click at the top end of
that line. To make it easy to communicate exactly where clicks
should be made, this text will refer to coordinates by the value
that you can type to specify them. Enter the coordinate
8.1,0.26 by typing the keys EIGHT PERIOD ONE COMMA ZERO
PERIOD TWO SIX ENTER.
NC-CAM Rout traces the outside edge of the board, creating
compensated cuts that exactly follow the outside edge of the
board, as can be seen in the drawing above. It Auto Routs the
Outside Edge, creating both line cuts and arc cuts, until it reaches
the starting point. It uses the options specified in the Auto Rout
Config dialog box to generate the appropriate Plunge Offset and
Overcut.
Click in the workspace with the mouse or hit ENTER to complete
the rout program. Auto Rout Outside remains active to allow you
to rout additional features. The command will remain active until
you select another command.
Chapter 2, System Walkthrough
35
Routing internal
cuts
The internal cuts should be routed with a smaller cutter. The
pocket could potentially be routed with the current cutter, but
some shops prefer to do all of their internal routing with one cutter
radius, if possible. In fact, pocketing should be done with the
largest cutter that will fit through all of the pathways in the
polygon, to save time. For this example, you will make all of the
internal cuts with one cutter. Select Modify | Cutter Config from
the main menu. The “Define Cutters” dialog will appear again,
with R0 still selected. The 0.032 cutter should be selected, so
click next to Tool 1 in the right-hand side. Click on OK to
continue.
Select Edit | Follow Profile from the main menu. Enter the
coordinates 1.9,0.9 in the command window, and then hit ENTER.
36
NC-CAM 6 User's Guide
At this point, the right-hand line in the slot will be displayed with
a dashed line, to indicate that it has been selected. The command
window will display instructions telling you to “Select Direction
With Both Buttons.” In this case, you will use the mouse to select
which direction the cutter should follow. With right compensation
selected, the cutter should follow the inside of the slot by moving
in a clock-wise direction. In order to inform NC-CAM of the
direction you wish the cutter to follow, click on the bottom arc of
the slot with both buttons (left and right buttons on a three-button
mouse.) Check the slot to make sure that it has been routed
correctly, with the rout path completely inside the original CAD
drawing of the slot.
Select Edit | Pocket Rout from the main menu. Enter the
coordinates 4.5,1.5 in the command window, and then hit ENTER.
The large arc on the left of the pocket will be selected for a
moment, and then the entire pocket will be filled with a rout path.
The rout path crosses left-to-right and right-to-left, moving up or
down when the cutter encounters another line in the polygon.
Then, the path goes once around the outside of the pocket, to
ensure a smooth edge.
Chapter 2, System Walkthrough
37
Changing rout
sequence order
In order to rout the board in the proper order, you will have to reorder the cuts so that the internal cuts are made first. To see the
order displayed, select View | Sequence Number from the main
menu.
Next to each cut, a number is displayed, indicating the order that
the cuts will be made. Select Modify | Do Last from the main
menu. Click on the outside cut next to the “1”, making it the last
cut.
38
NC-CAM 6 User's Guide
Notice that the sequence number next to the internal cuts are
lower numbers than the outside cut. Turn off the sequence
number display by selecting View | Sequence Number again.
Chapter 2, System Walkthrough
39
Step & repeats
in rout programs
To get the maximum usage out of a panel, a board is often
stepped and repeated many times. In order to easily generate a
step and repeat, select Modify | Auto Step & Repeat from the
main menu. In order to Select All of the entities for stepping and
repeating, type SA at the command window. Hit ENTER to confirm
the selection of all of the entities. A dialog labeled “Auto Step &
Repeat” will appear.
In the “X Direction” section, enter a value of 2 for Number of
Steps, and a Step Distance of 9.0. In the “Y Direction” section,
enter 3 for Number of Steps, and 3.5 for Step Distance. Make
sure that “Nested Steps” is selected, and then click on OK. By
default, stepped parts are displayed with dashed lines. In order to
turn this off, select View | Dash Stepped Parts from the main
menu. To view the entire panel area, select View | Zoom All
from the main menu.
40
NC-CAM 6 User's Guide
One of the most powerful features of NC-CAM’s RoutEdit is the
ability to modify a board after it has been stepped and repeated.
In the following section, you will add break-away tabs to the
board, and NC-CAM will automatically modify all of the boards
in the step and repeat pattern.
Chapter 2, System Walkthrough
41
Creating tabs
From the main menu, select Edit | Auto Tab. Select Modify |
Auto Tab Config from the main menu to modify the settings for
the tabs. A dialog labeled “Auto Tab Settings” will appear.
Select the topmost drawing by clicking on it. Select a Width (A)
of 0.25 inches. Enter a Cut-In Width (B) of 0.2 inches, and a CutIn Offset (C) of 0.02 inches. Make sure that both the Cutter
Radius Offset and the Drilled Holes Enabled features are enabled.
Enter a Hole Offset (D) of 0.01 inches, 2 for the Number Of
Holes, a Hole Spacing of 0.09 inches, and 2 for the Tool Number.
Click on OK to continue with these values.
To specify the location of a break-away tab, you must first select
the cut that a break-away tab will be inserted into. That is, you
will select the cut which will be interrupted by the tab. Then, you
specify the location along that cut where the break-away tab will
be inserted.
To select the bottom line, enter 1.7,-0.25 in the command window.
To specify the location, enter 1.7,-0.25 again.
Select the right half of the bottom line by typing 6.4,-0.25 and then
specify the location by entering 6.4,-0.25 again.
Select the top line with 1.7,2.6 and then the location with 1.7,2.6
again.
42
NC-CAM 6 User's Guide
Select the right half of the top line with 6.4,2.6 and then specify
the location by typing 6.4,2.6 again.
Output rout
In order to save the rout data that you have created, select File |
Make Rout Tape from the main menu. A dialog labeled “Save
Rout file as:” will appear.
Enter the file name “6SAMPLE.RT” and then click on OK. An
“Output Format” dialog will appear.
Chapter 2, System Walkthrough
43
All of the default values for this dialog will be fine, so click on
OK to finish saving the file.
Loading drill data
Select the first drill layer, “D0” by clicking on the D0 Layer
Button.
The title bar now says “DrillEdit,” and the buttons in the toolbar
have changed to allow drill editing.
44
NC-CAM 6 User's Guide
Load the sample drill file into NC-CAM by selecting File |
Import from the main menu, which causes the “Select file to
import” dialog to appear.
Click on the name “6SAMPLE.DRL” and then click on OK to
select the file. The “File Format” dialog appears, with the type
“Excellon Drill/Rout” selected, so click on OK to continue. A
dialog appears with the title “Excellon-to-Drill,” with several
parameters available.
Chapter 2, System Walkthrough
45
The sample file fits these parameters, so simply click on OK.
The Import Results window pops up to show information on the
file you just read in. This is just for your information, so click
OK. NC-CAM will ask if this is the main part. Click on Yes to
continue. NC-CAM will then ask what layer to place the data on
with a dialog labeled “Select Layer For Data” with Layer D0
already selected, so click on OK.
As you can see above, NC-CAM will display the drill data in the
work area.
Step and
repeats in drill
programs
The step & repeat information for your drill data will typically
mirror the step & repeat information for your rout data, since the
boards will physically be layed out in the same configuration.
Therefore, select Step & Repeat | Auto Step & Repeat from the
main menu. To Select All of the drill data, type SA in the
command window, and then hit ENTER. The “Auto Step &
Repeat” dialog will appear, with the same values that you entered
while editing the rout data. Click on OK to step & repeat the drill
data in the same way.
46
NC-CAM 6 User's Guide
Output drill
In order to save the drill data, select File | Make Drill Tape from
the main menu. A dialog labeled “Make Drill Tape as:” will
appear, in which you should enter the name “6PANEL.DRL” and
then click on OK.
Another dialog, labled “Make Drill Tape” will appear.
Chapter 2, System Walkthrough
47
You’ll want to pay close attention to the values that you set in this
dialog. For now, change the Optimizer value to “OptiScan!” and
turn off the checkboxes labeled “Mark First Tooling Hits” and
“Mark Last Tooling Hits”, and then click on OK.
A dialog will appear, labled “Save Tools and Layers” with all of
the tools selected, which is fine, so click on OK to finish making
a drill tape.
48
NC-CAM 6 User's Guide
A window will pop up asking if you want to print out a tool table
of the drill data in this file. Click Yes or No. You now have a
completed Excellon drill program in your \NCCAM6\DRILL
directory.
Printing
Be aware that NC-CAM will print to the active printer, in the
same manner as all of your Windows applications. To change the
active printer, select File | Printer Setup from the main menu.
Select File | Quick Print from the main menu, and a “Quick
Print” dialog will appear.
Select a scale of 1/2:1 for the printing, and specify that the data be
Rotated. Click on OK, and the dialog will close, and you will be
prompted to specify the lower left-hand corner of where the page
will be placed, relative to the work area.
Chapter 2, System Walkthrough
49
Click on the lower left-hand most edge of the displayed data, and
Quick Print will print to your active printer.
The Plot Configuration window will pop up, allowing you to add 2
lines of text to your drawing. Type in the text (i.e. your name, a
part number, etc.) and click the Plot format block option. Click
OK to send the screen image to the printer. If you do not want to
add text, simply click OK.
50
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
3
Using the CAD and RoutEdit modules
This chapter provides a step-by-step introduction to NC-CAM's
rout programming system, the CAD and RoutEdit modules.
Through the course of the tutorial, you will learn how to:
„ build routable CAD drawings from paper drawings
„ build and output rout programs from your CAD drawings
After reading this chapter, you should be able to access the CAD
and RoutEdit modules, and use their basic features to create rout
programs.
Chapter 3, Using the CAD and RoutEdit modules
51
Your first CAD drawing
Generally speaking, there are two ways you'll begin when it's
time to make a CNC router program. You'll be supplied with
either a paper drawing of the customer's board profile or panel,
or a data file (photoplotter, HPGL, or even an old rout program)
containing the board profile. NC-CAM is very well equipped to
handle each of these possibilities. This chapter will cover both
situations.
Finding your way
around
To begin your CAD session, select CAD layer zero on your
layer buttons. The CAD layers are numbered 0 through 29.
When a CAD layer is selected, you'll see the word “CAD” in the
program's title bar, and you'll see the CAD toolbar at the right
side of your screen.
In CAD, the majority of the work you'll be doing involves
editing drawing entities. To do this, you need ready access to a
large number of special editing functions. Most of these editing
functions are made available to you in the icons on the right side
of the screen.
52
NC-CAM 6 User's Guide
To help you learn what these icons indicate, there is an
automatic fly-by help built in to the CAD editor's menu system.
To get a look at the fly-by help, position your cursor over one of
the icons without pressing any mouse buttons.
Fly-by help for each icon
As you can see, the icon beneath the cursor is the button for the
ZW Zoom In function. The two letters “ZW” in front of the
function's name indicate the shortcut keyboard command for this
function. Experienced users of older NC-CAM revisions will
recognize ZW as the same command used by Generic CADD
and NC-CAM 5 for the Zoom Window function. This
consistency allows all experienced users of any revision of NCCAM's CAD module with very little adjustment.
You should take the time to place the mouse over each of the
buttons, and read the fly-by help for each of them. If you're an
experienced 2D CAD user, you'll find that all of the major
functions you're going to need for building printed circuit board
profiles are available on these icons.
If you select an operation and press the F1 Key, the NC-CAM
Online Help will be opened to the entry for this function. This
allows you to see a detailed description of each command. You
can also access a complete directory of Help Topics for the
features and operations of NC-CAM.
Chapter 3, Using the CAD and RoutEdit modules
53
Drawing in CAD
Drawing the basic entities in the CAD module involves first
selecting what you want to draw, then entering the points needed
to draw it. There are four types of entities used in the CAD
module.
CAD Entities
Points: Points are shown on-screen as small plus “+” signs.
They are defined by a single XY coordinate. The point shortcut
command is PO.
Lines: On-screen, lines just look like thin, straight line
segments. They are defined at their two endpoints by two XY
coordinates. In CAD editing for board profiles, the lines (and
arcs and circles) have no width attribute: They are regarded as
being infinitely thin. The shortcut command for Create Line is
LI.
Arcs: On-screen, arcs are shown as semicircles. They are
defined by three XY coordinates; one at each endpoint, and one
at the center. The shortcut commands for making arcs are A2
and A3.
Circles: A circle is defined by its radius and an XY center
coordinate. The circle shortcut command is C2.
Every drawing you'll ever create or import into CAD will be
represented by combinations of these four types of entities. The
small number of data types allows the CAD editor to provide
you a very predictable, uncomplicated way of working with the
drawings to make rout profiles, regardless of where or how the
drawings were made.
54
NC-CAM 6 User's Guide
Coordinates and
dimensions
In using CAD to make profile drawings of printed circuit
boards, you're called upon to produce very exacting drawings,
with precise coordinates and dimensions. Because of this, you
cannot avoid using the keyboard quite a lot, since entering
accurate values is the only way to produce accurate drawings.
The most important part of learning to use a CAD editor for
PCB work is learning when to use the keyboard, and when to
use the mouse. In general, using the mouse is much faster than
using the keyboard, so the technique you'll learn is to construct
your drawings by snapping and trimming lines to other lines
you've already created, thus avoiding as much keyboard entry as
possible.
To enter a coordinate with the keyboard, you type the X value, a
comma, then the Y value, and press ENTER. So, to enter the
coordinate X 12.34 Y-4.56 you'd type in 12.34,-4.56 and
press ENTER. The values are entered with decimal points and
minus signs as needed.
Modal functions
The button that stays
depressed determines
which function
is selected.
When you select a drawing function in the CAD module, the
toolbar button corresponding to the function will remain
depressed. That's because the drawing and editing function
buttons are modal. When a toolbar button is “modal,” it remains
selected until you select a different toolbar button. Note that in
NC-CAM, the main drawing and editing functions are generally
modal, while the modifier butttons (like snaps) are not modal.
Sometimes you may forget which function you've got selected,
and by clicking the mouse you'll start to draw a feature you
really don't want. Any time you want to abort a drawing
function in NC-CAM, press your ESC key. Pressing the ESC key
will free you from whatever function you may be “stuck in”.
Chapter 3, Using the CAD and RoutEdit modules
55
Making points
Let's start our CAD drawing by creating some points. To create
a point, select the point icon (at the top of the menu), or type
PO. You'll see that the prompt at the bottom of the screen now
indicates you're about to create a point.
CAD allows you to combine its functions in a variety of ways.
If you ever lose track of what function or combination of
functions you've selected, look to the text prompts at the bottom
of the screen.
Begin this drawing by creating a point at X 1.0" Y 1.0". Do this
by typing 1,1 and pressing ENTER. You'll see a plus “+” sign
appear near the intersection of the two dashed zero-zero
indicator lines. Make another point by typing 5,1 and again
pressing ENTER. (The PO point function is modal, so you don't
need to reselect it to make a second point). Make a third point
by typing 5,4 followed by ENTER.
56
NC-CAM 6 User's Guide
Zoom All
To get a better look at the three points you've made, select Zoom
All either by pressing the button, or by typing the two-letter
shortcut ZA.
As you can see, the ZA Zoom All function re-sizes the screen to
zoom in as far as possible, while still showing all of the entities
in your drawing. The other zoom commands are:
ZB Zoom Back: Zooms out by a factor of two (makes things
smaller)
ZW Zoom Window: Zooms the screen in on a user-defined
window.
Chapter 3, Using the CAD and RoutEdit modules
57
Making lines
The command to make a line is LI. You may select the line
function by typing LI or pressing the line button. Start your first
line by typing its endpoint, 1,4 then press ENTER. When you
move your mouse around, you'll see a rubber-banded line is
attached to your cursor.
One of the ways you can avoid entering coordinates on the
keyboard is to snap to existing points in your drawing. Now
move your cursor close to the lower-left point, as shown in the
figure above.
58
NC-CAM 6 User's Guide
Snaps
With the cursor positioned as shown on the preceding page, type
NP on your keyboard. NP stands for “nearest point,” and it
causes your cursor to snap to the nearest point, and it simulates a
center mouse button click there. As you can see, your line has
snapped to precisely the same coordinate as the first point you
created.
If you're using a three-buttoned mouse, you can access the NP
command by pressing your center mouse button. It's a real
time-saver!
CAD offers several more snap commands. They are:
SC Snap Closest: Acts exactly like the near point snap, except
that it waits for you to click your left mouse button, allowing
you to move the mouse close to the endpoint you wish to snap
to.
SI Snap Intersection: Asks you to select two entities, then snaps
to their intersection point. (If the entities intersect in more than
one place, snaps to the intersection closest to the mouse when
you pick the second entity).
SM Snap Midpoint: Snaps to the midpoint of the line or arc you
select.
SN Snap Center: Snaps to the center of the circle or arc you
select next.
ST Snap Tangent: Snaps to the edge of the arc or circle you
select next. Doesn't establish the line end immediately: It keeps
moving the snapped end to keep the line tangent to the arc or
circle as you move your mouse.
SP Snap Perpendicular: Snaps to the entity you select next.
Like the snap tangent function, this does not establish the line
end: It keeps moving the line end to keep the line from your
mouse perpendicular to the entity you selected. (Works on arcs
and circles, too!)
Chapter 3, Using the CAD and RoutEdit modules
59
The snap commands save a tremendous amount of time, make it
possible to avoid entering redundant coordinates, as well as
performing complex trigonometric functions.
To complete this part of the drawing, move your mouse close to
the top end of the line you've made. Type NP on your keyboard.
This will snap the cursor to the top of the line, and begin
drawing a new line (since you did not select any other modal
command).
60
NC-CAM 6 User's Guide
Now, let's see what happens when you make a mistake while
drawing in CAD. Assuming that our drawing is supposed to
end up as a plain rectangle, it would be a mistake to connect a
line from the upper-left corner to the lower-right. Go ahead and
move your mouse to the lower-right corner, and click your left
mouse button.
Undo...Redo
The line you've just made doesn't belong in this drawing. If
you've taken the time to look at the buttons in the CAD menu,
you've probably seen the “pencil eraser” icon. Yes, you could
use the eraser to just erase the errant line you just made, but
there's a more powerful tool you could use. For almost any
error you make in your CAD drawing, you can undo the mistake
by selecting OO, the Undo command.
Place your mouse over the “reverse arrow” icon, and you'll
notice that the help prompt at the bottom-right corner of the
screen says, “Undo make line.” If you press the button, the bad
line you've made will disappear.
Chapter 3, Using the CAD and RoutEdit modules
61
Redo
If you press the “Undo” button again, you'll erase the line at the
left side of the drawing. Now you've undone something you
actually wanted to keep! Never fear, just move your mouse to
the UU Redo button (just to the right of the Undo button), and
read the help prompt.
As you can see, the Redo function lets you put back changes
you've reversed with the Undo function. You can think of the
Undo as acting somewhat like a “rewind,” and Redo as acting
like a “replay” function.
More snaps
To continue your drawing, select the SC Snap Closest function.
This behaves much like the NP Near Point function you've
already used, except that it waits for you to reposition your
mouse and click your left mouse button before it snaps to the
closest point.
62
NC-CAM 6 User's Guide
After selecting SC Snap Closest, place your mouse near the top
of the line at the left side of your screen, and click your left
mouse button. You'll see the starting end of your line snap to
the top of the other line. Now select Snap Closest again,
position your mouse near the point at the upper-right corner of
your screen, and again click your left mouse button. You'll see
that the line end has snapped to the point at coordinate X5Y4.
Use LI Create Line and SC Snap Closest to add two more lines,
completing a rectangle as shown above. If you make any
mistakes, “undo” them by using the OO Undo command.
Chapter 3, Using the CAD and RoutEdit modules
63
Chamfer
Often times, you'll need to chamfer square corners in a drawing.
To chamfer a corner, type CH or select the Chamfer icon on the
menu.
After you select CH Chamfer, you must identify the intersection
where you want to make the chamfer. To identify the upper-left
intersection, click first near the center of the top line. You'll see
the line become highlighted. Then, click near the center of the
line at the left side of the screen. You'll see the lines highlight as
you select them, then you'll see the chamfer made automatically.
64
NC-CAM 6 User's Guide
Here you can see the 0.1" chamfer made at the upper-left corner
of the rectangle. There's an important lesson to be learned in the
way you indicated the intersection at the upper-left corner to the
CAD program: You selected the entities that intersected, not the
intersection itself. Many of the edits and snaps you'll want to
perform in CAD require that you select intersections, so we'll
examine this further.
Chapter 3, Using the CAD and RoutEdit modules
65
Selecting
intersections
Some of the most powerful editing functions you can perform in
CAD require that you select an intersection. The CH Chamfer
function shown in the preceding pages gives one example of a
function that “happens” at an intersection. Before we examine
other functions which act on intersections, we'll focus on this
idea of selecting an intersection in CAD. First, there's the
definition of an intersection:
INTERSECTION: The point where two entities either
meet, or would meet if they were extended. (CAD makes
no distinction between actual and would-be intersections).
Any time you need to select an intersection in CAD, select the
two entities which intersect, not the intersection point itself.
66
NC-CAM 6 User's Guide
In this example, assume you want to select the intersection in the
upper-left corner of the drawing. To do this, you would first
select the top line, then the left line. You would not click near
the intersection, because CAD needs to find the entities before it
can compute their intersection. The next pages will introduce
you to several functions that deal with intersections. In each
case, when CAD needs to know which intersection you want,
you must identify it by clicking separately on each of the two
intersecting entities.
More about
Chamfer
When you select CH Chamfer, you'll see something new at the
bottom of your screen. The extra text below the command line
describes the current distance settings for the chamfer function.
Assume that you need to make an asymmetric chamfer which is
0.25" on one side, and 0.5" on the other. Begin by selecting the
CH Chamfer function. The text at the bottom of your screen will
show:
To change the chamfer settings, select Chamfer Distance 1,
which is now set to “0.1.” You may select the Chamfer
Distance 1 field by clicking on it with your mouse. After you've
selected the field, type 0.25 then press ENTER.
Select the Chamfer Distance 2 field, and set it to one half inch
by typing 0.5 and pressing ENTER.
Now, chamfer the upper-right corner of the rectangle, by
clicking on the right-hand line, then the top line. You'll see that
the short side of the chamfer is on the line you clicked first; the
right-hand line. This is Chamfer Distance 1. The long side of
the chamfer, Chamfer Distance 2, is on the line you clicked last;
the top line.
Chapter 3, Using the CAD and RoutEdit modules
67
Points vs. Entities
In CAD, sometimes you need to enter points, and at other times
you need to select entities. How do you know what CAD is
expecting at any given time? The answer is usually found in the
progress prompt at the bottom of the screen.
When you're creating something new in CAD, you need to
define a point, or possibly several points. You may define
points by clicking your left mouse button, typing in coordinates,
or snapping to entities. When you're editing or snapping, you
need to select entities that are already present in your drawing.
The progress prompt usually indicates what CAD is expecting
you to do next.
when in doubt, check
the command line
and the progress prompt
As shown in the illustration, the top two lines of the text box are
called the Command Line, and the Progress Prompt. When you
type coordinates and commands in CAD, these will appear on
the Command Line. If you've selected one or more functions
(like LI, then SC), these commands will appear to the left of the
“>” prompt on the Command Line, as a reminder to tell you
what you've entered.
to abort any function:
right mouse button
or the Escape key
68
When you select a command that requires several steps to
complete, the step that's needed next will usually be indicated in
the Progress Prompt. In the case of CH Chamfer, CAD needs to
“know” which two lines you want to chamfer. So, after you've
selected CH Chamfer, the Progress Prompt says “First Line.”
This means that, in order to proceed with the chamfer, CAD
needs for you to select a line.
NC-CAM 6 User's Guide
Fillet
Radiused corners are another common feature of routed PCB
profiles. In CAD, a radiused corner is called a fillet. CAD will
automatically make a fillet between any two lines (or arcs) with
the FL Fillet command.
When you select the FL Fillet command, you'll see the fillet
parameters appear at the bottom of your screen. Fillet works
exactly like the Chamfer function, inasmuch as it requires you to
select the two entities you wish to join with a radiused corner.
In this case, select the bottom and left-hand lines to fillet the
bottom-left corner of the rectangle.
Chapter 3, Using the CAD and RoutEdit modules
69
Measuring
If you've followed the steps on the preceding pages closely, your
drawing should match the above illustration.
There are two inspection functions in CAD; ME Measure, and
OI Object Inspect. Select the ME Measure function, and click
your mouse in the lower-right corner, as shown. The cursor will
snap to the corner, and attach a rubber-banded line to it. The
end of the rubber-banded line attached to the corner indicates
the point you're measuring from.
70
NC-CAM 6 User's Guide
Now, position your cursor as shown above, and click the left
mouse button. The right-hand line will change color, and
measurement values will appear at the bottom of the screen.
Chapter 3, Using the CAD and RoutEdit modules
71
The measurement values given are:
Measure from-to: Gives the start and end points of your
measurement.
DX: The from-to distance in the X direction.
DY: The from-to distance in the Y direction.
Len: The from-to length
Ang: The from-to angle, measured from the positive
horizontal axis.
You'll notice that there's still a rubber-banded line attached to
your cursor, and there is also a large “X” under the center of the
cursor. This is the other part of the measure function; the ability
to measure angles.
Position your cursor as shown, and click the left mouse button.
You'll see the “X” snap to the left end of the bottom line, and
the measurement report at the bottom of the screen will update
to show you the statistics for the bottom line.
72
NC-CAM 6 User's Guide
The arc between the two measurement lines indicates the angle
that's being reported by the text “Ang=180.0000.”
To take the ME Measure function a step further, click your
mouse on the “X” at the left end of the bottom line. The “X”
will re-attach itself to your cursor, allowing you to snap it to
another point in your drawing for another measurement. Go
ahead and test measuring to various endpoints in the drawing.
When you want to exit the measure function, press your righthand mouse button, or the ESC key.
Inspect
In addition to the measurement capability described in the
preceding pages, CAD offers a powerful OI Object Inspect
function. Object Inspect allows you to select an object, view all
of its parameters, and change them as desired. Try selecting OI
Object Inspect, and then click on the right-hand line.
As you can see, the line's endpoint coordinates are now
available in editable fields at the bottom of the screen. You can
use this function to verify the values an entity has, or change
them by clicking on any of them with the mouse. Try clicking
on the upper-left X value, and typing 0 then ENTER.
Chapter 3, Using the CAD and RoutEdit modules
73
Here's the line with one of its X ordinates set to zero. If you
wanted to keep the changed line, you would press ENTER (don't
do it). To abandon the change, press ESC. The line will be
restored to its original location.
74
NC-CAM 6 User's Guide
Saving your work
If you've followed all of the steps in this chapter, your drawing
should match the illustration below.
To save your drawing, select File/Save As... from the main
menu. You'll see a dialog box appear, with the cursor blinking
in the file name field.
Type a name for your file, for example FIRSTJOB.FAS and
press ENTER. Your file will be saved to the default job directory,
\NCCAM6\DATABASE. Note that when you save a job in
NC-CAM 6, you're saving all layers of the CAD, Rout, and
Drill data, to an NC-CAM 6 database file. If you want to save
your CAD drawings to another format (such as DXF), select
File/Export.
Chapter 3, Using the CAD and RoutEdit modules
75
Arcs
There are two functions for creating arcs in CAD; the two-point
arc, and the three-point arc. We'll look at the more commonly
used function, A2 Create 2-Point Arc, so type A2 or click the 2point arc button.
Just to get a look at how a two-point arc is created, use the
mouse to click the arc center, arc start, and arc end as shown.
As you can see, when you're making a two-point arc the first
point establishes the arc's center. The second point sets the arc
start and defines the arc's radius. The third point determines the
arc's endpoint indirectly, by combining the arc's radius and the
angle of the third point you enter.
Use OO Undo to erase the arc you just made. Next, we'll
combine the A2 Create 2-Point Arc command with other
commands, to create an arc cut-out on the right-hand line.
76
NC-CAM 6 User's Guide
Snaps with other
functions
Snap functions can create accurate points quickly, when you'd
otherwise have to compute them and type them in. You may
use a snap function any time CAD is waiting for you to enter a
point. To see this, begin by selecting the A2 Create 2-Point Arc
function.
To use a snap with the A2 function, select SM Snap Midpoint.
Next, click your mouse near the center of the right-hand line (as
shown). The Snap Midpoint function will compute the exact
coordinate of the line's midpoint, and snap the center of your arc
to that location. Now you're ready to create the arc's start point.
In this case, we'd like the arc to have a radius of one-half inch.
How can you create the start point and know that it's set to a
half-inch radius, when you don't know the coordinate of the
center point? By using CAD's relative mode.
Chapter 3, Using the CAD and RoutEdit modules
77
Relative mode
CAD drawings tend to be dimensioned arbitrarily. There's
usually enough information in the dimensions for you to
duplicate the drawing, but they're often given as distances from
other features. The coordinates you've entered into CAD thus
far have been absolute distances from your drawing's zero point.
For the half-inch arc you're making, it is convenient to enter the
start point as a distance away from the arc's center point. To do
this, you may toggle CAD's coordinate entry mode from
absolute (the default) to relative mode. Type MR, or press the
Relative Mode button on the menu.
When you turn on Relative Mode, notice that the button stays
depressed. This is because Relative Mode is a modal function:
It stays turned on until you shut it off. While the Relative Mode
button is depressed, each coordinate you type will be taken as an
offset from the previous coordinate. This is true whether you
snapped to the previous coordinate, or you typed it in.
When you want to type in
a coordinate as an offset,
use relative mode.
To set the “last point,”
you can do an NP (nearpoint snap) to the point,
then press Esc. The next
coorinated you type will
be relative to the point
you snapped.
With the MR button toggled on, type 0,0.5 and press ENTER.
This will set your arc's start point one-half inch above the center
point. Now shut off Relative Mode by typing MO (for ManualOrigin), or press the Relative Mode button. The button will pop
up to indicate that Relative Mode is now off.
78
NC-CAM 6 User's Guide
Trims
Trims are fast; much
faster than typing in
coordinates.
Complete your arc by using the mouse to drag the arc down, and
then past the right of the vertical line as shown. Click your left
mouse button to complete drawing the arc.
With the arc drawn as shown, you'll need to trim the arc's end
point to stop at the vertical line. This idea of trimming lines to
other lines is used often in CAD, because it helps you make
absolutely accurate features without having to calculate
coordinates. Once you've created an accurate feature in CAD,
the Trim functions allow you to use the feature like a knife, to
cut new lines to precisely where they intersect the existing
feature. The trim functions cut (or extend) lines and arcs. You
can use lines, arcs, or circles as the “knives” for cutting lines
and arcs.
As with intersections, the trim functions work whether the two
entities actually intersect or not. If two lines (or arcs) could
intersect if they were extended, the trim functions work.
There's one major idea to keep in mind when you use the trim
functions: Click the side you want to keep. If you're trimming a
line that crosses something else, you've got to click the side of
the line you want to keep, not the side you want to throw away.
Chapter 3, Using the CAD and RoutEdit modules
79
Click the part of the arc
you want to keep.
To trim the bottom of the arc to the vertical line, select RM Trim
Line, position your mouse as shown, and click the left mouse
button. This selects what you want to trim, and which side of it
you want to keep. Next, click on the line as shown below.
The line you select
will act like a knife,
trimming the arc.
80
NC-CAM 6 User's Guide
If you click at exactly the two points indicated, the trim function
will neatly trim your arc to the point where it intersects the
vertical line. If anything went wrong, use the OO Undo function
to reverse the mistake, and try again, paying close attention to
your mouse positions.
Chapter 3, Using the CAD and RoutEdit modules
81
Breaking lines
To complete the sample board outline, you'll need to break the
right-hand line at the top and bottom of the arc.
Break lets you break one
object into two.
Select the OB Object Break function, and click with your mouse
on the right-hand line. Remember, when you're selecting an
entity, put the cursor on the entity, away from any other entity.
To break things precisely,
use a snap function
When you've selected the vertical line for the Object Break
operation, the line will highlight, and you'll have a rubberbanded indicator line attached to your cursor. This line indicates
the point where you'll break the right-hand line if you click your
left mouse button. In this case, you want to break the line
exactly where it meets the arc, so you'll use the SC Snap Closest
function. Select Snap Closest, position your mouse as shown in
the illustration, and click your left mouse button. If you now
move your mouse up and down, you'll see that the right-hand
line will be broken exactly where it meets the bottom of the arc.
To complete the break operation, again select SC Snap Closest,
place the cursor near the top of the arc, and click your left
mouse button. You'll see the line is neatly broken into two lines
which end exactly at the top and bottom of the arc.
82
NC-CAM 6 User's Guide
Preparing to rout
Select the ZB Zoom Back function to get a good overall look at
your drawing. If you've followed all of the instructions in this
chapter, your drawing should match the above illustration. If
not, you'll want to review your steps now.
This would be a good time to save the job to disk again, using
the File/Save main menu function.
Regardless of how you've built your drawing, it's a good idea to
check the outlines before you try to use them to build a rout
program. It's not possible to create a good rout program unless
the lines you're planning to rout are correctly trimmed (or
snapped) to each other. The main-menu function to check the
profile is Check/Path.
Chapter 3, Using the CAD and RoutEdit modules
83
Check your profiles with
Test Path before routing.
The profile-follower goes
towards the line end
you're closest to when
you click both buttons.
When you select Check/Path, you'll see this display. The
procedure used here is the same one you'll use when you're
creating a rout program.
The general idea is that you first select the line where you want
the test to begin. Then, you move your mouse to the end of the
line you want the test to go towards. When you've got the
mouse close to the proper line end, you simultaneously press,
hold, and then release both the left and right mouse buttons.
The profile-follower will chase the part edge, checking each
intersection along the way. The profile-follower will stop when
the path is completed, where there is a gap, or where there is
more than one path to follow.
84
NC-CAM 6 User's Guide
When Test Path can
follow the profile, it's
ready for routing.
When you press, hold, and release both buttons, the profilefollower should completely follow the outline you've made, and
this message should appear. If it does, congratulations are in
order: You've successfully made your first board profile! Click
OK to exit the Test Path function.
On the other hand, many first-time users do not succeed at
building a perfect profile on the first try. The two most common
problems are duplicated lines and gaps.
Fix multi-paths with Erase.
Fix gaps with Join.
Duplicated lines may be difficult to detect, because if one line is
directly on top of another, there's no way to see the problem on
the screen. When you get the error message “Stopped due to
multiple paths” but you cannot see more than two lines meeting
at the trouble spot, you've probably got overlapping lines there.
The easiest way to eliminate overlapping lines is to use WE
Window Erase to erase one of the lines, then RD View Refresh
to see what might have been underneath the line you've erased.
The erased line may be easily replaced by using the NP Near
Point snap function.
Gaps are most easily cured with the JO Join Lines function.
The Join Lines function prompts you to select two intersecting
entities, and it then trims the two so that they meet perfectly.
Once you've corrected any problems in your profile, test it again
with the Check/Path function. Do not proceed to the next
section until your drawing passes the test.
Chapter 3, Using the CAD and RoutEdit modules
85
Your first rout program
To build a rout program,
first you select
a routing layer.
With your board profile complete, it's time to call up the Rout
module. Select the first rout layer, “R0” by clicking the R0
layer button. This automatically selects the rout module, and the
routing tools will be displayed on the toolbar.
In the rout module, you'll be able to create, view, and modify
rout paths using the specialized routing toolbar. For this
exercise, we're going to quickly create a simple external rout of
this board.
86
NC-CAM 6 User's Guide
Cutter selection
To define cutter diameters and select cutters, select
Modify|Cutter Config from the main menu.
Because NC-CAM 6 allows you to work on as many as five rout
programs at once, there are also five tool tables. When you
select Modify|Cutter Config, you must then select which of the
five tables you wish to use. In this case, choose the tab for layer
R0.
For this rout, you'll want to select tool number three, which
defaults to an 0.093 cutter size. Note that when you press the
radio button for tool three, the compensation automatically
switches to index number three. Click OK to proceed with this
cutter.
Chapter 3, Using the CAD and RoutEdit modules
87
Auto Rout
To rout the outline you've created, select Edit|Auto Rout
Outside. The Auto Rout function offers several different cut-in/
cut-out styles, which you may choose by selecting Modify|Auto
Rout Config, or by clicking on the words “configure autorout”
in the Command Window.
Auto Rout offers three
cut-in/cut-out styles;
Corner, Inline, and Pinless
Choose the Inline cut-in/cut-out style by pressing the large
button at the lower-left corner of the dialog. Then press OK to
proceed.
88
NC-CAM 6 User's Guide
Choosing
compensation
For most routing, you'll
want to select the righthand compensation.
When you're creating external routs, you'll ordinarily want to
use the standard “comp right, counter-clockwise” technique. To
use this approach, you'll need to select HR Comp Right before
you create the rout. (It is also possible to make NC-CAM
perform external routs using left-hand compensation and a
counter-clockwise approach. This is useful in certain cases
where internal pinning is supplied, and two counter-clockwise
passes can be used for high accuracy.)
For now, select the right-hand compensation as shown.
Chapter 3, Using the CAD and RoutEdit modules
89
AutoRout Outside
automatically picks the
direction, based on your
choice of right-hand or
left-hand compensation.
Once you've selected the Auto Rout Outside function and the
right-hand compensation button is depressed, routing the profile
is as simple as clicking your mouse near the line where you
want the plunge and lift to occur, and then pressing enter to
confirm the selected line. When you have multiple items to
rout, you must select them in the sequence in which you want
them routed on the machine.
90
NC-CAM 6 User's Guide
When you click on the line, NC-CAM's Rout module analyzes
the board outline and creates the routing information
automatically. The cutter path is shown graphically atop the
CAD outline, exactly simulating a CNC rout controller.
Select File|Save to save the job as an NC-CAM 6 database,
including both the CAD and Rout layers.
Chapter 3, Using the CAD and RoutEdit modules
91
Rout program
output
When you've finished creating a rout in NC-CAM, you will
undoubtedly want to output it in a CNC format so you can run it
on a routing machine. To do this, select File|Make Rout Tape.
After you've chosen the directory and filename for your rout
program, press ENTER or click Save. The format dialog appears.
This is to let you select the format for your router program.
Choose the format you'd like, and press OK.
When you press OK, the rout layer will be saved as a CNC
router program. Congratulations! You have now completed
your first rout program, using the CAD and Rout modules.
Your output rout program is a regular ASCII DOS file, ready to
send to a CNC routing machine.
92
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
4
Using the DrillEdit module
This chapter provides a step-by-step introduction to NC-CAM's
“DrillEdit” drill programming capabilities. Through the course
of the tutorial, you will learn how to:
„ import customer data files
„ take measurements in the drill pattern
„ sort tool tables
„ edit holes individually and in windows
„ check for and correct spacing violations
„ step-and-repeat a board into a panel
„ optimize and output a finished drill program
After reading this chapter, you should be able to use NC-CAM's
DrillEdit module to process drill programs. You should also
have an understanding of how DrillEdit handles tool tables, inch
and metric units, and step-and-repeats.
Chapter 4, Using the DrillEdit module
93
Your first drill program
To select the DrillEdit module, press the “D0” button on the
layer menu (on the left side of the screen). This will make layer
D0 the selected layer, and the DrillEdit module's toolbar and
main menu will be displayed. Why would a drill editor have
“layers?” Because you will sometimes have to work with more
than one drill job at a time. Consider the case of a first-drill
(pre-plating) and second-drill (post-plating) process. With NCCAM, you can bring in the data for both of these drill processes
at once, by using layer D0 for the first-drill data and layer D1
for the second-drill data. You can use additional layers for blind
and buried vias, etcetera.
The advantage here is that you can make sure the several drill
programs match perfectly, long before you ever drill them in
production. You can check to see that the two programs don't
conflict. You can use the same step-and-repeat data for both
files. In short, you can use NC-CAM to be absolutely certain
that the programs are correct: And being absolutely certain is
what NC-CAM is all about.
Using the DrillEdit module is not at all like hand-editing a drill
program in a text editor. Apart from the obvious difference that
DrillEdit shows you the drill program as graphics instead of text,
DrillEdit is a genuine CAD program, with a CAD database.
Begin your exploration by selecting File/Import. This will give
you a look at the file import dialog box.
This is the menu you'll be using to read all of your drill files into
DrillEdit. We'll get into the details of how to use the file import
dialog in later chapters. For now, just select the file
SAMPLE.60, either by typing the name in, or by doubleclicking on the name with your left mouse button.
94
NC-CAM 6 User's Guide
Any time you select File/Import in any of NC-CAM's three
modules, NC-CAM will try to automatically figure out what
type of file you've selected. NC-CAM is a very flexible
program. It allows you to read in data from a variety of sources,
not just CNC drill files. When you select File/Import, NCCAM's import routines each take a quick look at the file to see if
they can tell what it is. They “bid” for the opportunity to decode
the file. Whichever routine best “understands” the file is given
the job of reading the file in. What this means is that you don't
have to tell NC-CAM what kind of file you're trying to read.
You just click on the file name, and NC-CAM figures out how
to read the file.
The File Format dialog tells you which data format NC-CAM
thinks the file is. If you want to look at the file in text mode to
verify the format, press the VIEW FILE button. In this case, the
SAMPLE.60 file is in the Excellon format, so just press OK.
Chapter 4, Using the DrillEdit module
95
Excellon-to-Drill
dialog
After you press OK on the File Format dialog, the DrillEdit
module will bring up the Excellon-to-Drill dialog, as shown
below.
The settings here are just like the settings on a drilling machine,
and they have the same effect. Before you choose the settings
for this file, you might want to take a look at it. To do this, you
would select View File, either by typing V on your keyboard, or
by pressing the button with your mouse.
Note that no matter what settings you choose in the Excellon-toDrill dialog, if the drill program you're reading contains format
control commands in an M48 header, the commands in the drill
program will override your menu settings. (This is also exactly
the way an actual drilling machine would behave). Press ENTER
or Click OK to read the drill file.
Import Results
Dialog
This window shows information
on the file, including the number
of drill hits and size of the part.
Click OK to proceed.
96
NC-CAM 6 User's Guide
Is this the main
part?
The next dialog you'll see asks the question, “Is this the main
part?” Why would the DrillEdit module want to know if the file
you're about to read in contains the “main part?” For several
reasons. First, understand that DrillEdit allows you to read
several files into the same job. These may include a part, some
coupons, panel tooling holes, and so on. So, DrillEdit needs to
know which file contains the “main part” so that it knows which
file to pay the most attention to.
When you're importing the main part, DrillEdit automatically
positions it in the workspace with no offset, so that the
coordinates you'll see on-screen are the same as the coordinates
in the original file (you can always change these later). DrillEdit
also automatically accepts any G93 offset (if there are any)
which the “main part” file contains. Any time you're working
with a simple job having only one file, you'll answer “Yes” to
this question. For now, press Y on your keyboard, or press the
Yes button with your mouse.
Select Layer for
Data Dialog
This window allows you to place the drill data on any one of 10
different drill layers. The selection defaults to Layer D0. This
will work for our purposes, so simply click on OK.
Chapter 4, Using the DrillEdit module
97
before using
View|Zoom All
After you click OK on the Select Layer window, you'll see the
drill data appear on the screen. The location of the data relative
to the zero-zero lines is determined by the X:Y values of the
coordinates in the drill file.
At this point, the screen is “zoomed out” so that the visible area
is about 46 inches (1.2 meters) wide. The drill data will look
very small. To get a better look at this job, first select View/
Zoom All.
98
NC-CAM 6 User's Guide
after using
View|Zoom All
The Zoom All function will automatically resize the screen to
center your view, and magnify it as well. (Zoom All is a
function you'll use frequently.)
Chapter 4, Using the DrillEdit module
99
Not a drill
program
Now you're actually looking at the drill data taken from the
SAMPLE.60 file. Note that we don't say, “you're looking at the
data in the file,” because you are not. When you read a drill
program into the DrillEdit module of NC-CAM, it isn't a drill
program any more. It is a 2D CAD database of drill holes with
a tool table. You can inspect any hole by just clicking your left
mouse button on it. You can make needed changes by clicking
on holes or windows of holes. You can control the sequence in
which holes are drilled by placing windows around them. You
can create nibbled slots, add holes, change hole sizes, check for
double hits, make coupons... in short you can do almost
anything you'd ever want to do with drill data, and you can do it
quickly, all because your drill data is no longer a text file of XY
coordinates, it's in a special-purpose 2D CAD database.
100
NC-CAM 6 User's Guide
Zoom and Pan
In the next couple of pages, you're going to need to get a closer
look at part of this drill pattern. To zoom in, you may type ZW,
click the left “magnifying glass” icon, or select View|Zoom In
from the main menu.
to zoom in , first type ZW,
then click+drag the area
you want to have
fill the workspace
With Zoom Window, the area you select will be magnified to fill
the workspace. Note that when you're “zoomed in,” you can
drag (pan) the screen around by holding down the ALT key while
you click+drag the workspace with the mouse.
Chapter 4, Using the DrillEdit module
101
Inspecting holes
The [OI] Object Inspect
function lets you
inspect and edit
To inspect a hole, place the point of the arrow cursor close to the
hole, and click your left mouse button. You'll see an “X” shape
snap to the hole. This indicates which exact hole you're
currently locked on to. You'll also notice that the command
window shows the X and Y ordinates of the hole, its tool
number and diameter, and which Layer the hole is located on
(D0). The X and Y ordinates, the tool number, and drill layer
are displayed in blue, because they are editable.
To alter a hole's location or tool number, you just use your TAB
key to select the the appropriate blue number in the command
window, type in the new value, and then press ENTER twice.
102
NC-CAM 6 User's Guide
To change a hole's tool,
use OI object inspect,
click on the hole, and
type the new tool
number into the
command window.
In this case, press the TAB key three times, to highlight the tool
number. Type in 7 for the new tool number, and press ENTER
only once. At this point, you'll see the hole change to the
diameter of the tool number seven, 0.126", and the hole will
change to red in color. If you want the hole to be permanently
changed to the new tool number, you may press ENTER a second
time. If you want to return the hole to its original tool number,
you may press ESC. In this case, press Enter to change this hole
to tool number seven.
Changing units
If you read the introductory text on page 10, you know that NCCAM can be easily switched between inch and metric units.
How easily? Try selecting View/Units/Millimeters, then click
on another hole to inspect it. You'll see that the units for the
drill diameter and the hole location are all now in millimeters.
This chapter is written assuming you're using the “inches”
display mode, so it would be best if you reselect View/Units/
Inches, for now.
Chapter 4, Using the DrillEdit module
103
Measuring
In preparing a drill job for production, many times you'll need to
measure the distance between two holes. First, though, select
ZA (zoom all) to show all of the drill data in this job.
To measure, first select the [ME] Measure icon on the toolbar.
Next, click on the hole you wish to measure from. You'll see a
rubber-banded line attached to your cursor. Next, select the hole
you wish to measure to. In the command window, you'll see the
X:Y coordinates of both of the holes, as well as three distances:
The “Manhattan” X and Y distances, as well as the straight-line
distance between the two holes.
The ME measure function
measures distance,
X:Y difference,
and angles
You may now measure from the first hole to any other hole by
just clicking on the other holes. All measurements will be made
from the first hole you selected. To get out of this measurement
mode, you may either press your right mouse button or the ESC
key.
104
NC-CAM 6 User's Guide
Tool tables
As we said earlier, this 2D drill database contains holes and a
tool table. So what does the tool table contain? To find out,
select Tools/Show Tool Table, and you'll see this display:
As you can see, the tool table lists the tools by number, with the
diameters and feed and speed parameters, if any, from the input
file's M48 header. The hit counts for regular holes and nibbled
circle/slot/drilled text holes are listed separately. The last
column is headed with the abbreviation “FLH-COUP,” which
stands for first-hit/last-hit coupon. Click OK to close the dialog.
As is often the case with the drill files you'll receive from your
customers, the tool sizes are not in any particular order. You
may sort the tool table by selecting Tools|Sort Small Tool First
from the main menu. When you do, the screen will repaint, and
you may notice that the hole colors have changed to reflect the
new tool assignments. Select Tools|Show Tool Table a second
time, and you'll see that the tools are now in a smallest-to-largest
sequence.
Chapter 4, Using the DrillEdit module
105
Spacing check
With the pervasive use of CAD printed circuit board design
software (especially by inexperienced operators), much of the
drill data you'll receive will have multiple hits at the same
location. It is also common to have double hits at almost the
same position. These “near double hits” result in a great deal of
tool breakage on the drilling machines, and a lot of scrapped
panels. DrillEdit's spacing check function allows you to
absolutely prevent these problems before they cause scrap.
Once the problems are identified, you can use Point Edit to
correct them. (Remember that we changed a hole from tool
number five to tool number seven a few pages ago. That's going
to cause a spacing violation in this job).
To use the spacing check function, select File/Spacing Check
from the main menu.
You'll notice some options in the Spacing Check dialog. First,
there's a checkbox for Delete Exact Duplicates. This choice
does what it says: If any hits in the job are duplicated exactly
(same tool, same exact coordinate). they will be deleted
automatically.
The Delete Pilot Holes choice deletes small hole(s) when they
are found at exactly the same coordinate as larger holes.
Finally, the Clearance choice actually compares every hole to
every other hole, to verify that there no two hole edges are
closer than the distance you've specified. In this case, set the
clearance value to 0.007 inch, make sure the Clearance
checkbox is checked, and then press OK.
106
NC-CAM 6 User's Guide
Spacing check will very quickly perform the tests you requested.
When the tests are done, you'll see the results in a dialog.
In this case, the Spacing Check function has detected three holes
which violated the specified minimum hole wall thickness of
0.007 inch. Holes violating spacing check are not automatically
changed in any way (because NC-CAM can't just guess how to fix
the violation). Instead, they are just moved to layer D9, so that
you can correct the problem after consulting with your customer
or his documentation.
Chapter 4, Using the DrillEdit module
107
The cursor is pointing to the three holes which are closer than
0.007 inch, as shown by Spacing Check. To correct this
violation, repeat the steps on the previous pages, using Object
Inspect to find the one large hole, and change it to tool number
five.
108
NC-CAM 6 User's Guide
Window editing
To change the three holes back to layer one, select [LO] Layer
Operation from the toolbar. The Layer Operation choice may be
used to move holes from one layer to another.
As you'll see in the command window, you may select any drill
layer as the “target” of the layer operation. In this case, you
want to move the three holes to layer D0, so just leave the
default setting alone. Next, drag a window around the three
holes, and they'll be moved back to layer D0. Note that it
doesn't matter if you also include other holes in the window:
They're already on layer D0, so nothing will happen to them if
they're also in the window when you do this layer operation.
Chapter 4, Using the DrillEdit module
109
Making an output drill program
To create an output drill program, begin by selecting File/Make
Drill Tape. You'll first be asked to select a name for your new
output drill program.
For the moment, you may name the job FIRSTJOB.DRL. Type
the file name in and either press Enter or click Save. Next you'll
see the imposing-looking Make Drill Tape menu.
'
'The Make Drill Tape menu offers control over most aspects of
the CNC drill program you'll output. There are many choices
available (these are discussed in Chapter 7, “DrillEdit
Command Reference”), but for the moment, the default values
will work fine. Just press OK.
110
NC-CAM 6 User's Guide
After you press OK, the Active Control Menu pops up
automatically. This is to remind you that only the active tools,
layers, and types will be output to your drill program. This is
where you may control the output of multiple files for special
purposes. Make sure all of the checkboxes are turned on, and
press OK.
At this point, there's a lot to watch. You'll see NC-CAM go
through the steps of optimizing and outputting your file.
When the output is completed, you'll be prompted with a menu
asking if you want to print out the “new” tool list. What would
be “new” about the tool list? Possibly quite a bit. As you'll
learn in Chapter 7, it is possible for DrillEdit to automatically
enforce maximum hit counts, and automatically average the
number of hits each tool is actually used for. It's also possible to
output the nibbled slots and circles as individual hits, instead of
G84 and G85 commands. There can be some tremendous
quality advantages in this approach. In any case, it's quite
possible that the output file will have a different tool list than
you had in the editor, and that's why you're given the option of
printing out the new list.
Chapter 4, Using the DrillEdit module
111
112
NC-CAM 6 User's Guide
P
A
R
T
2
Command references
Chapter 5, CAD command reference
113
114
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
5
CAD command reference
This chapter provides a command-by-command reference to the
NC-CAM 6 CAD functions.
Chapter 5, CAD command reference
115
The functions, in the order presented on the CAD button menu are:
PO Create Point
LI Create Line
RE Create Rectangle
A2 Create 2-Point Arc
A3 Create 3-Point Arc
C2 Create Circle
SC Snap Closest Endpoint
SI Snap Intersection
SM Snap Midpoint
SN Snap Arc-Circle Center
ST Snap Tangent
SP Snap Perpendicular
SL Snap Parallel
LO Layer Operation
OR Turn on Ortho Snap
OA Ortho Angle
MR Relative Mode
RM Trim Line
JO Join Lines
OB Object Break
CH Chamfer Lines
FL Fillet Lines
DO Drawing Origin
WM Window Move
WS Window Stretch
SW Window Scale
WC Window Copy
WI Window Mirror
WF Window Flip
MC Matrix Copy
RC Radial Copy
RO Rotate
WE Window Erase
OO Undo
UU Redo
OI Object Inspect
ME Measure
SA Select All
ZW Zoom In
ZA Zoom All
ZB Zoom Out
116
NC-CAM 6 User's Guide
[PO] Create
Point
The Make Point function allows you to make a reference point,
which is displayed in your drawing as a small plus “+” sign. The
points you make with PO are primarily useful for tagging
locations you will need later, in the course of constructing your
drawing.
One good example of a case where you might use a point would
be to tag the zero location of your drawing when you want to use
RO Rotate to rotate the entire drawing to work on an off-axis
section. This happens often in the flex circuit business, where the
drawings will often have entire sections which are dimensioned
off-axis. In this case, having a point at the zero location gives you
an easy reference to rotate the drawing around.
One case where you might encounter a lot of points is when you
import a Gerber photoplot file. Because CAD’s import filter has
no provision for entering an aperture list for the Gerber data, any
“D03” flash commands in the Gerber file will be converted to
points in the CAD database.
[LI] Create Line
The Line function is undoubtedly the one you’ll use most often in
CAD. In CAD, lines are actually line segments, with no
thickness, defined by their two endpoints. When you create a line,
you’ll be prompted to enter the first endpoint. After you do, you’ll
notice a “rubber-banded” line connecting the first endpoint you
made to the cursor. When you define the second endpoint, the
rubber-banded line will change to a line entity in the CAD
database.
There’s one key modifier you’ll often use when making lines; the
orthogonal mode. The button for the orthogonal mode is a drafting
“T-square” symbol, for good reason. The orthogonal mode forces
your line to be square to the axes, or to the angle you’ve entered
with the OA Ortho Angle function. The ortho mode is available
instantly without toggling on the OA button, though: Any time
you want the ortho mode turned on for just one mouse click, it’s
easier to just press and hold the CTRL key on your keyboard. This
works both ways, i.e., if the ortho mode button is turned on,
pressing CTRL will temporarily release the ortho mode.
Chapter 5, CAD command reference
117
[RE] Create
Rectangle
The RE Rectangle function allows you to create an axis-aligned
rectangle by placing its two diagonally-opposite corners. Once
you've created a rectangle, it isn't a rectangle any longer, though.
The RE Rectangle function actually creates four independent
line entities in the shape of a rectangle. The only respect in
which a rectangle is still treated as a rectangle after it's made is
by the OO Undo and UU Redo functions.
As with the LI Line function, after you enter the first coordinate
of a rectangle, you'll see a rubber-banded rectangle attached to
your cursor.
[A2] Create 2Point Arc
The A2 Two-Point Arc function creates an arc, by defining the
arc's center point, then a startpoint, and finally its endpoint. The
centerpoint is like the place you'd anchor a compass if you were
drawing an arc on a drafting table. Once the centerpoint is
defined, you'll get a rubber-banded straight line attached to your
cursor, until you define the start point.
A two-point arc's start point defines both the angle from the
center to the start, as well as fixing the arc's radius. After the
start point is defined, the rubber-banded arc you'll see attached
to your cursor has a radius that's fixed at the distance from the
center point. When you're defining the end point, all you're
actually setting is the ending angle of the arc, even if you use a
snap function to enter it.
[A3] Create 3Point Arc
The A3 Three-Point Arc function allows you to create an arc by
defining one endpoint, then a point along the arc, and finally the
other endpoint. This means that the radius is not actually set
until the third and final point has been entered. The resulting
rubber-band effect is quite unusual, as the arc's center and radius
change fluidly as you move the mouse while defining the second
end point.
118
NC-CAM 6 User's Guide
[C2] Create
Circle
The C2 Create Circle command will add a circle to the CAD
database, by defining the circles’ center point, and secondly, a
point on the edge of the circle. Once you define a center point,
you’ll get a rubber-banded circle that is attached to your cursor,
until you define a point on the circle.
[SC] Snap Closest
Endpoint
The SC Snap Closest function is used when you’re entering a
coordinate and you want it to be exactly the same as an existing
coordinate in the drawing. To use snap closest, you simply
select the function, then move the cursor close to the point you
wish to snap to, and press your left mouse button.
There’s a similar function that’s actually used more often than
SC by experienced CAD users, and that is the NP Near Point
function. Unlike the SC function, NP does not require that you
click your left mouse button. Instead, it snaps immediately
when you enter NP on the keyboard. This immediate snap, and
the fact that you don’t have to move your mouse over to the
menu and then back to the desired point, save a considerable
amount of time. Obviously, there’s no point in having a menu
button for NP, because you’d have to have your mouse on the
menu and not near the snap point in order to press the button! An
alternate way to select NP is to click the middle mouse button, if
you have a three-button mouse.
There’s one aspect of SC and NP that’s not obvious to first-time
users: There are more snappable points than you can ordinarily
see on the screen. This is because both arcs and circles have
construction points at their centers. These points become visible
only when you turn on the View|Const Points function, but they
may always be used for snapping.
If you have a 3-button mouse on your computer, the middle button
works as an NP snap. Simply move the cursor near a point and
press the middle mouse button once to snap to the point.
Chapter 5, CAD command reference
119
[SI] Snap
Intersection
The SI Snap Intersection function is used when you’re entering a
coordinate, and you want it to be at precisely the point where two
existing entities intersect. The process of using snap intersection,
as described in the progress prompt, is to select the two
intersecting entities, one at a time. CAD then computes the
location of the intersection of the two entities, and enters the
needed coordinate at that location.
An interesting nuance of the Snap Intersection function occurs
when there are actually two places where the entities you’ve
chosen intersect. This is possible any time one or both of the
intersecting entities are circular. In this instance, the intersection
you’ll snap to is the one closest to your mouse when you select
the second entity.
In the example shown above, to snap to intersection “A,” you
must select the line to the left-hand side, which is closer to the
“A” intersection than it is to the “B” intersection.
Note that the snap intersection function does not require that the
two entities actually intersect; only that they could intersect if they
were long enough to touch each other.
120
NC-CAM 6 User's Guide
[SM] Snap
Midpoint
The SM Snap Midpoint function snaps to the midpoint of the line
or arc you select next. The line midpoint chosen is exactly
halfway between its two endpoints.
If you select an arc with the Snap Midpoint function, the
coordinate you’ll snap to is the arc’s midpoint, not its center.
The midpoint of an arc is a point along the arc, such that the point
bisects the arc as shown above.
Chapter 5, CAD command reference
121
[SN] Snap ArcCircle Center
The SN Snap Arc Center command snaps the coordinate to the
center of the arc or circle you choose.
In the illustration above, one line end has been snapped to the
center of the arc.
Note that it is not possible to snap to an arc center which falls
outside of the 84 inch (2.14 meter) working area of the CAD
database.
122
NC-CAM 6 User's Guide
[ST] Snap
Tangent
The ST Snap Tangent function performs a fairly complex
function. First off, ST works only when you’re creating a line,
not an arc or a circle. Secondly, the snap is tricky because the
point you’re creating with the snap isn’t actually defined until you
create the second line end. When you select snap tangent and
click on an arc or circle, the rubber-banded line you’ll see
constantly moves to remain tangent to the arc or circle, until you
select the second line end.
There is another important issue when you’re using snap tangent:
There are actually two lines that would be tangent to an arc or
circle from any given point outside the arc or circle. In other
words, your rubber-banded tangent line may be coming off of the
selected circular entity either clockwise or counterclockwise.
If you want to reverse the direction of the snap tangent function,
you must pass your cursor through the center of the circular
object, and out the other side.
Chapter 5, CAD command reference
123
[SP] Snap
Perpendicular
The SP Snap Perpendicular function acts to alter the behavior of
the rubber-banded line you’re creating. Snap perpendicular also
works only when you’re creating lines, not arcs or circles.
One surprising behavior of the snap perpendicular function is that
you may snap perpendicular to a line, point, circle, or arc. When
you’re snapping perpendicular to an arc or circle, the line you
make will end at the circular object, aligned with its center.
Note that like the snap intersection function, it is not necessary
that the point you’re trying to create with the snapped end actually
touch the entity it’s perpendicular to.
124
NC-CAM 6 User's Guide
[SL] Snap Parallel
The SL Snap Parallel function, like the SP Snap Perpendicular
function, works only when creating lines, not arcs or circles. The
function can be used in two different ways. Both methods require
that a line is already present to apply the snap to. Both methods
also require that you are currently using LI Create Line.
The first method for using SL Snap Parallel, is to pick the SL
Snap Parallel button first. In the user panel, you will see the
parallel offset. This is the distance from the selected entity where
the line will be placed. Next, pick the line to which you wish to
snap. Then you must pick the first point of the line you are
creating. The point you pick will determine the first point in the
following way: The point forms a perpendicular line to the
selected entity. The point on this line at the specified offset is the
first point of the line created.
You must now select the second point. The second point is picked
in a similar fashion to the first point.
The second method for using SL Snap Parallel, is to select the
first point before using Snap Parallel. Using this method, the
parallel offset is determined by the first point, not a value
specified in the user panel.
After selecting the first point, press the SL Snap Parallel button.
You must then select a line entity to which to apply the snap.
After selecting the entity, you must select the second point of the
line in the same fashion as in the first method.
Chapter 5, CAD command reference
125
[LO] Layer
Operation
The LO Layer Operation function allows you to move entities
from one layer to another. This function may be used in the
following two ways:
1) When this button is pressed by itself, the function acts like
WE Window Erase, with one difference. The selected entities
are not erased, they are merely moved to the layer specified in the
user panel. The selection of entities, however, is exactly the
same as WE Window Erase. You can use Layer Operation to
move either single entities or windowed groups of entities. This
window function does not, however, allow you to select multiple
entities using the shift-click approach described in the WM
Window Move function: When you select an entity by clicking on
it, or a group of entities with a click-drag window, they are moved
immediately.
2) The Layer Operation function may be applied to any window
edit function as well. To do so, first pick the operation you wish
to perform. Then select Layer Operation. The result of the
operation, instead of landing on the construction layer, will be
placed on the layer selected in the user panel instead. Notice that
doing a Window Move still requires you to select the offset when
using this function.
126
NC-CAM 6 User's Guide
[OR] Turn on
Ortho Snap
OR Ortho Mode applies a constraint to the cursor motion once a
point has been entered. The constraint acts to force the line
you’re creating to be square to the axes, or to the angle you’ve
entered with the OA Ortho Angle function described on the
following page.
When it’s turned on, the Ortho Mode will force newly-created
lines square to the ortho angle, even if you snap the second end of
a line you’re creating to some other object.
In one respect, ortho mode acts a bit like the ST Snap Tangent
function described earlier: Once it’s locked on to an axis, say the
“X” axis for example, it stays locked on to that axis no matter
how far you move your mouse along the other axis.
To get the line to swap from being locked on one axis to being
locked on the other, you must move your cursor very close to the
start point of the line.
One final note about Ortho Mode: You may instantly reverse
Ortho Mode’s on/off state by holding down the CTRL key. This is
much quicker than actually pushing the button on the menu.
Chapter 5, CAD command reference
127
[OA] Ortho Angle
The OA Ortho Angle function allows you to set the angle of the
axes used by the OR Ortho Mode to any angle you wish. This is
incredibly handy for creating lines which have a known angle, and
one endpoint you can create with a snap or a keyboarded
coordinate.
The angles you specify with the ortho angle function are measured
in degrees, and the positive angles run counterclockwise with
respect to the right-hand horizontal axis (usually the X+ axis).
Using the ortho angle function automatically turns on ortho mode,
as you’ll see when the ortho mode button automatically flips to the
“on” state when you enter a new ortho angle.
The only catch with using ortho angle is that it’s persistent: Once
you set it to an odd angle, that angle remains the effecive ortho
angle until you select OA a second time, and set the angle back
to zero.
128
NC-CAM 6 User's Guide
[MR] Relative
Mode
The MR Relative Mode toggle affects the way coordinates you
enter are interpreted. Ordinarily, all of the coordinates you enter
are relative to the zero point of your drawing. Sometimes,
however, it’s advantageous for you to be able to enter a coordinate
as a distance from the previous coordinate. That’s what the MR
Relative Mode toggle allows you to do.
Assume for a moment that you have a dimension on a drawing
that’s given as being one-half inch to the right of the upper-right
corner of a rectangle. You could either inspect the rectangle’s
upper right corner, write down its coordinate, add half an inch in
the X axis, and type in the resulting coordinate, or you could use
the MR mode to enter the point.
As shown above, if the point you most recently created is not the
point you’ve got to enter a coordinate relative to, just use NP or
SC to snap the start of a new line to your desired reference point,
then press ESC. Turn on MR, and the numbers you enter will be
relative to that reference point.
Chapter 5, CAD command reference
129
There’s one added point worthy of special mention here: It’s best
to make sure you turn off the MR Relative Mode as soon as
you’re done using it. Forgetting that you’re in relative mode can
lead to some frustration when you later enter coordinates, and
discover that they’re not ending up where you intended them to be.
[RM] Trim Line
The RM Trim function allows you to extend or trim a line or arc
to the point where it does (or would) intersect another linear
entity. This function saves a huge amount of time when you’re
creating CAD drawings, because it allows you to avoid entering
coordinates repeatedly.
When you select RM Trim, you must first choose the entity you
want to change. Second, you select the entity you want to use as
a knife, to cut the first entity at the point where the two intersect.
One aspect of the RM function that confuses some first-time
users is that when you’re using it to trim off the end of an entity, it
keeps the side of the entity you click on first.
130
NC-CAM 6 User's Guide
In this case, the left side of the line will be kept, and the right side
will be trimmed off. As with the SI Snap Intersection function, if
two intersections are possible, the one used is the one closest to
your cursor when you select the second entity.
Chapter 5, CAD command reference
131
[JO] Join Lines
The JO Join function acts just like RM Trim, except that it trims
both of the entities you select, keeping the side of each entity that
you clicked on.
The JO Join function is very useful for cleaning up badly made
intersections in customer-supplied drawings.
132
NC-CAM 6 User's Guide
[OB] Object
Break
OB Object Break allows you to break lines, arcs, and circles.
When you break a line or an arc, the result is two lines or arcs.
When you break a circle, it becomes an arc.
When you’re using the object break function, rubber-banded
indicator lines connecting to your cursor will show where the
object will be broken when you enter the next coordinate. You
may break objects at precise locations by using snap functions to
determine the break points.
One special note about using break on arcs and circles: If you
need to break a circular entity at precise locations, it’s generally
faster to just break the object casually and then trim its ends than
it would be to use the snap intersection function during the break
command itself.
Chapter 5, CAD command reference
133
[CH] Chamfer
Lines
The CH Chamfer command creates a perfect chamfer (or bevel,
if you prefer) at the intersection of the two lines you select. As
with the JO Join command, the parts of the lines to be kept will
be the parts you click.
The chamfer function has two settings; CA Chamfer Distance 1,
and CB Chamfer Distance 2. These control how far back the two
lines are trimmed before the joining chamfer is created.
In this example, chamfer distance 1 was one-half inch, and
chamfer distance 2 was one inch.
134
NC-CAM 6 User's Guide
[FL] Fillet Lines
The FL Fillet function acts like the JO Join function, but it
creates a radius between the two entities. The radius is set with
the FR Fillet Radius function. As with the join and chamfer
functions, when the line or arc entities will be trimmed by the
function, the side kept is the side you clicked on.
Two special cases for the FL function arise when you use choose
lines which are parallel and end square to each other. In this
case, the setting of the fillet radius is ignored, and a perfect 180
degree fillet is created between the two parallel lines.
In this illustration, FL has been used twice: Once with the clicks
at 1 & 2, and again with the clicks at A & B. As shown above,
filleting the open end of a rectangle puts a half circle across the
end. Filleting the closed end of a rectangle also makes a half
circle, but it deletes the joining line and backs up the arc to the
point where it would have been tangent to the joining line.
Chapter 5, CAD command reference
135
[DO] Drawing
Origin
The DO Drawing Origin command moves all of the data in your
drawing relative to the drawing origin. This is useful for
temporarily setting the drawing’s origin during editing, as well as
finally establishing the zero point for routing.
[WM] Window
Move
The WM Window Move command allows you to click on an
entity, or click-drag a window around a group of entities, and then
move them.
The process of establishing the from/to positions for the entities to
move is exactly the same as creating a line. This means you can
use the same tricks you’d use in making a line to determine the
exact positions the window moves from and to.
As with many CAD functions, there’s a hidden feature in the
window move, as well as all of the other window functions which
follow: When you select a window full of objects, they become
highlighted on the screen. If you want to add selected entities to
the group to be changed, hold down your SHIFT key and click on
the entities you want to add. You’ll see them become highlighted,
indicating that they’re now included in the group you windowed!
This “shift-click” function also works in reverse: If your window
accidently selected an entity you did not want to include in the
group, use shift-click to deselect it. You’ll see the entity unhighlight, to indicate that it is no longer a member of the selected
group.
136
NC-CAM 6 User's Guide
[WS] Window
Stretch
The WS Window Stretch function is used to “lengthen” a board
profile by moving an edge in or out. When this function is
activated, you will be asked to select an entity or select a group of
entities using the click-drag window method to stretch.
When the group of entities is selected, there will be two types of
highlighted entities on the screen. The first type will be the
entities highlighted in white. These entities will simply be moved
to their new location.
The second type of entity that will appear will be red highlighted
entities. These are the entities that will be stretched. The
endpoint of these entities that falls in the selected window will be
moved to its new location, while the endpoint that fell out of the
selected window will stay anchored.
After the entities have been selected, you will be asked to specify
the move vector. The process of establishing the from/to positions
for the entities to move is exactly the same as creating a line.
This means you can use the same tricks you’d use in making a
line to determine the exact positions the window moves from and
to. The function works the same as WM Window Move.
Chapter 5, CAD command reference
137
[SW] Window
Scale
The SW Window Scale function allows you to stretch or shrink the
windowed entities by the factor you enter, referenced from a point
you select.
Window Scale can alter the windowed group differently in the
horizontal and vertical directions, if you wish. If you do scale a
window asymmetrically, the circles and arcs receive special
treatment: Circles remain circular when scaled asymmetrically,
but the radius of each circle will be altered by the product of the
two scale factors. This means that if you scale a window by 2.0
in the horizontal axis, and 0.3 in the vertical axis, the radii of any
circles you’ve selected will be scaled by 2.0 times 0.3, resulting
in a scale of 0.6:1.
Arcs, on the other hand, actually are scaled asymmetrically. The
treatment given to the arcs follows this procedure: First each arc
has an added point computed for it, the point being the arc’s
midpoint (see the SM function for a definition of this). Then, the
arc’s midpoint, start point, and end point are scaled according to
the two different scale factors you’ve selected. Finally, the arcs
are reconstructed, using the math of the A3 Three-Point Arc
function to reestablish each arc using the three scaled points. This
rather complex process does allow for asymmetrical scaling of
arcs, albeit with arc centers that move as necessary to maintain
equal start and end radii.
[WC] Window
Copy
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
138
NC-CAM 6 User's Guide
[WI] Window
Mirror
The WI Window Mirror function copies all of the selected
entities, mirroring around an arbitrary axis line. This powerful
function is very handy for creating copies of individual entities at
odd angles.
It’s probably best for you to experiment with the WI Window
Mirror function a bit before you use it in a live drawing. The
mirror around an arbitrary line tends to be a little confusing, until
you realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[WF] Window Flip
The WF Window Flip function moves all of the selected entities,
mirroring around an arbitrary axis line. This powerful function is
very handy for moving entities to odd angles.
It’s probably best for you to experiment with the WF Window Flip
function a bit before you use it in a live drawing. The mirror
around an arbitrary line tends to be a little confusing, until you
realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[MC] Matrix
Copy
The MC Matrix Copy function produces from one to ninety-nine
copies of the selected entities in the X and Y direction, evenly
distributing the copies in an array with spacing you specify.
[RC] Radial Copy
The RC Radial Copy function produces from one to ninety-nine
copies of the selected entities, evenly distributing the copies
across the angle you specify, around the center point you specify.
The icon for this function depicts a radial copy with a quantity of
three, an angle of 360 degrees, and a center point located just
above the bottom rectangle.
Chapter 5, CAD command reference
139
[RO] Rotate
The RO Rotate function simply rotates all of the selected entities
around a point. The function is extremely useful for working on
sections of drawings which are dimensioned off-axis. By using
the RO function, you can rotate your entire drawing to place the
needed section on-axis, do the editing you need to do, and then use
RO a second time to rotate the entire drawing back to its original
alignment.
[WE] Window
Erase
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
[OO] Undo
The OO Undo function allows you to reverse the effects of your
editing, one step at a time, back to the beginning of your session.
If you place your cursor over the Undo icon, the help text in the
Status Window will describe the function you’re about to reverse.
Note that when you pack the database (with the File/Pack
Database function), the Undo function’s memory is erased.
140
NC-CAM 6 User's Guide
[UU] Redo
The UU Redo function reverses the effect of the OO Undo
function, one step at a time. This button will be “grayed out” until
you’ve pressed the OO Undo button. As with the OO Undo icon,
if you place your cursor on the UU Redo icon, the help text will
describe the function you’re about to Redo if you press the button.
[OI] Object
Inspect
The OI Object Inspect function allows you to select any entity in
the drawing, and view the coordinates of the points making up the
entity. Further, once you’ve selected an entity with OI Object
Inspect, you can modify the entity by clicking on any of its
defining values, and typing in new values. When you do this, the
highlighted entity will instantly change on-screen, and turn red in
color. If you want to restore the entity to its original condition,
press ESC. To keep any change you’ve made, press ENTER.
[ME] Measure
The ME Measure function allows you to measure from any
construction point in your drawing to any other. Further, you may
measure angles by defining a baseline with your first two clicks,
and an angle with the third mouse click.
To reverse the angle reading in the measure mode, click your
mouse near the apex of the angle.
Chapter 5, CAD command reference
141
[SA] Select All
The SA Select All button is unavailable until you’ve selected any
of the window functions. With a window function selected, SA
will automatically select all of the entities in your drawing.
There’s a special capability available with the SA Select All
function. If you want to select everything in your drawing except
what’s inside a window, follow these steps: First, select the
window function you want. Second, window the group you want
excluded from the window operation, and they’ll highlight. Last,
hold the SHIFT key and press the SA Select All button. This will
reverse the selections you’ve made. You may then proceed with
the remaining steps of the window function you originally
selected.
[ZW] Zoom In
The ZW Zoom Window function allows you to window a portion
of the screen you want to zoom in on. The creation of this
window is identical to the process of creating a rectangle. After
the zoom region is specified, the work area is redrawn, focusing
in on the area you selected.
The counterpart to this function is the ZB Zoom Back function,
which can be used to decrease the magnification.
A useful new feature of NC-CAM is the ability to pan with a
simple ALT-click-drag combination. If the display was magnified
to show the upper-left-hand portion of your drawing, and you
wanted to "slide" the view over towards the upper-right-hand side
of the drawing, the new pan feature can be used. Hold down the
ALT key, left-click with the mouse on the right-hand side of the
drawing, and drag that location to the left-hand side of the
drawing. In essence, the new pan feature "picks up and drags the
work area," just as you would move a sheet of paper to center in
front of you the area that you wanted to work on.
To repeatedly pick up and move the drawing in this manner, keep
holding down the ALT key, let go of the left mouse button, drag the
mouse to the opposite side of the drawing, left-click the mouse,
and drag back. Advanced users of NC-CAM will learn the clickdrag, click-drag, click-drag motion and grow to use it more often.
142
NC-CAM 6 User's Guide
[ZA] Zoom All
The ZA Zoom All function redraws the screen at a scale which
will show all of the entities in your drawing.
[ZB] Zoom Out
The ZB Zoom Back function reduces the magnification of the
screen by a factor of two.
The counterpart to this function is the ZW Zoom Window
function, which can be used to increase the magnification.
[PA] Pan
The PA Pan function, although now mostly obsolete, is included
to keep backwards compatibility with NC-CAM 5. This function
is replaced by the new scheme whereby you hold down the ALT
key, and depress the left mouse button to pan the screen.
With this pan function, however, you will be asked to select a
new center for the screen. When you click the mouse, the
location you select will be the new center of the visible viewing
area, with the same zoom factor.
[OE] Delete
Entity(s)
OE Delete Entity(s) is the same function as WE Window Erase.
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
Chapter 5, CAD command reference
143
[FR] Fillet Radius
The FR Fillet Radius function allows you to set the radius that
will be used by the FL Fillet Lines function. The units are
entered in the current (Metric/Inch) mode.
[NX] Number in X
The NX Number in X function sets the number of copies made in
the X direction when using the MC Matrix Copy function.
[NY] Number in Y
The NY Number in Y function sets the number of copies made in
the Y direction when using the MC Matrix Copy function.
[XS] X Increment
The XS X Increment function sets the distance between copies
made in the X direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[YS] Y Increment
The YS Y Increment function sets the distance between copies
made in the Y direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[TD] Total
Degrees
The TD Total Degrees function sets the total degrees used during
a RC Radius Copy.
[NC] Number of
Copies
The NC Number of Copies function sets the number of copies
made during a RC Radius Copy.
144
NC-CAM 6 User's Guide
[RD] Redraw
The RD Redraw function redraws the workspace area. This is
especially useful if you have deleted several entities, and the
deleted entities have "covered" part or all of some entities that
remain.
[NP] Snap Near
Point
The NP Snap Near Point function, although only available from
the keyboard, is one of the most useful snap functions in the CAD
snap set. It allows the user to make “perfect” drawings where
there are no gaps left in the corners of a board profile that might
be left if you use freehand drawing.
If you have a 3-button mouse on your computer, the middle button
works as an NP snap. Simple move the cursor near a point and
press the middle mouse button once to snap to the point.
[CA] Chamfer
Distance 1
This function sets the first chamfer distance used in CH Chamfer
Lines.
[CB] Chamfer
Distance 2
This function sets the second chamfer distance used in CH
Chamfer Lines.
[MO] Absolute
Mode
This command turns off relative mode which can be used to enter
coordinates in the user panel. This function turns off the relative
mode regardless of the state of the MR Relative Mode button.
Chapter 5, CAD command reference
145
[OC] Copy
The OC Copy function in the same as the WC Window Copy
function.
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
[WO] Window
Delete Outside
The WO Window Delete Outside function behaves much like the
WE Window Erase function, with the exception that the entities
deleted are the entities outside of the click-dragged window, not
the entities on the inside.
[LS] Target Layer
The LS Target Layer function allows you to set the layer where
LO Layer Operation functions will land.
[TP] Test Path
The TP Test Path allows you to test a board profile in CAD
before going over to Rout and using FP Follow Profile or AR
Auto Rout to rout the profile. This helps find problems such as
unlinked paths and paths with multiple entities connected to one
point.
146
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
6
RoutEdit command reference
This chapter provides a command-by-command reference to the
NC-CAM 6 RoutEdit functions.
Chapter 6, RoutEdit command reference
147
The functions, in the order presented on the Rout button menu are:
DH Drill Hole
LI Rout Line
RS Rout Outside Rectangle
A2 Create 2-Point Routed Arc
A3 Create 3-Point Routed Arc
IR Rout Inside Rectangle
AT Auto Tab
SI Snap Intersection
SM Snap Midpoint
HL Comp Left
HN Comp None
HR Comp Right
AR Auto Rout Outside
RI Auto Rout Inside
FP Follow Profile
OR Turn on Ortho Snap
OA Ortho Angle
MR Relative Mode
PR Previous Cut
PL Next Cut
EN End Single Step
RW Previous Sequence
FF Next Sequence
DO Drawing Origin
WM Window Move
WS Window Stretch
SW Window Scale
WC Window Copy
WI Window Mirror
WF Window Flip
MC Matrix Copy
RC Radial Copy
RO Rotate
WE Window Erase
OO Undo
UU Redo
OI Object Inspect
ME Measure
SA Select All
ZW Zoom In
ZA Zoom All
ZB Zoom Out
DF Do First
DB Do Before
DL Do Last
148
NC-CAM 6 User's Guide
[DH] Drill Hole
The DH Drill Hole function allows you to drill a single hole in a
specified location. It is very similar to the PO Create Point
function in CAD.
This function is primarily used in DrillEdit, however, it is also
available in RoutEdit for creating holes that will be stored at
output time as G05 holes.
[LI] Rout Line
The LI Rout Line function can be used to create Rout programs
one cut at a time. This is useful if you are creating simple square
routs or for adding a quick internal cut. The function works much
the same way that LI Create Line in CAD works, with one
notable exception. When the command is used, you will be
prompted for the first point. After you do, you will notice a
"rubber-banded" line from the first point to the cursor. When you
define the second point, you will notice that a linear cut is added
to the database.
In addition, you will also notice that there is now a rubber-banded
line from the last point you created to the cursor. Once again,
when you define another point, another linear cut is added to the
database. With this command, you can create consecutive cuts
until you reach the lift point of the cutter. At this point, you will
need to exit the consecutive cut mode by right-clicking with the
mouse, or hitting ESC.
Should you wish to use Rout Line in conjunction with A2 Rout 2Point Arc or A3 Rout 3-Point Arc, switching to either of these two
commands will not shut off the rubber band. Instead, you can
continue creating cuts without inserting a lift-plunge in the
database.
Additionally, should you with to continue with this function after
already hitting ESC, you can use NP (Snap Near Point) or SC
(Snap Closest) to "attach" to the rout profile and continue adding
cuts.
As in CAD, you may use ortho mode by holding down the CTRL
key.
Chapter 6, RoutEdit command reference
149
[RS] Rout
Outside
Rectangle
The RS Rout Outside Rectangle function is used for adding
simple square profiles to the rout database. The direction of
travel is determined by the current compensation which is set
using HL Comp Left, HN Comp None, HR Comp Right.
The RS Rout Outside Rectangle works very similar to the RE
Create Rectangle command.
When the RS Rout Outside Rectangle function is selected, you
will be prompted to select the first corner of the rectangle. Note
that this also determines the plunge point for the router bit. Once
the first corner is selected, a rubber-banded rectangle will be
shown on screen from the first corner to the current cursor
position. You will be prompted for the second corner. Once this
corner is selected, the routed rectangle will be added to the rout
database and shown on screen.
[A2] Create 2Point Routed Arc
The A2 Two-Point Routed Arc function creates a circular cut as
defined by an arc. The arc is defined in a slightly different order
than in CAD, so that the user may continue defining attached arcs
without a lift-plunge being inserted in the database. An arc in rout
is defined by first choosing the start point, then the arc's center
point, and finally its endpoint. The center point is like the place
you'd anchor a compass if you were drawing an arc on a drafting
table. Once the start point is defined, you'll get a rubber-banded
straight line attached to your cursor, until you define the center
point.
A two-point arc's center point defines both the angle from the start
to the center, as well as fixing the arc's radius. After the center
point is defined, the rubber-banded arc you'll see attached to your
cursor has a radius that's fixed at the distance from the center
point. When you're defining the end point, all you're actually
setting is the ending angle of the arc, even if you use a snap
function to enter it.
In addition, you will also notice that there is now a rubber-banded
line from the last point you created to the cursor. Once again,
when you define another center and end point, another circular cut
is added to the database. With this command, you can create
consecutive cuts until you reach the lift point of the cutter.
150
NC-CAM 6 User's Guide
Should you wish to use A2 Create 2-Point Routed Arc in
conjunction with LI Rout Line or A3 Create 3-Point Routed Arc,
switching to either of these two commands will not shut off the
rubber band. Instead, you can continue creating cuts without
inserting a lift-plunge in the database.
Additionally, should you with to continue with this function after
already hitting ESC, you can use NP (Snap Near Point) or SC
(Snap Closest) to "attach" to the rout profile and continue adding
cuts.
[A3] Create 3Point Arc
The A3 Create Three-Point Routed Arc function creates a
circular cut as defined by an arc. The arc is made by selecting
one endpoint, then a point along the arc, and finally the other
endpoint. This means that the radius is not actually set until the
third and final point has been entered. The resulting rubber-band
effect is quite unusual, as the arc's center and radius change
fluidly as you move the mouse while defining the second end
point.
In addition, you will also notice that there is now a rubber-banded
line from the last point you created to the cursor. Once again,
when you define another second and end point, another circular
cut is added to the database. With this command, you can create
consecutive cuts until you reach the lift point of the cutter.
You may switch to creating Routed Lines or 2-Point arcs, and can
also resume drawing 3-Point Arcs as explained in A2 Create 2Point Routed Arc.
[IR] Rout Inside
Rectangle
The IR Rout Inside Rectangle function is the same as the RS
Rout Outside Rectangle function except that this function is meant
for creating cutouts inside a board profile. The direction of travel
is determined by the current compensation which is set using HL
Comp Left, HN Comp None, HR Comp Right.
The IR Rout Inside Rectangle works very similar to the RE
Create Rectangle command in CAD.
Chapter 6, RoutEdit command reference
151
When the IR Create Inside Rectangle function is selected, you
will be prompted to select the first corner of the rectangle. Note
that this is also determines the plunge point for the router bit.
Once the first corner is selected, a rubber-banded rectangle will
be shown on screen from the first corner to the current cursor
position. You will be prompted for the second corner. Once this
corner is selected, the routed rectangle will be added to the rout
database and shown on screen.
[AT] Auto Tab
The AT Auto Tab function is a method for adding quick
breakaway tabs to any rout profile. This function should be
selected after the board outline has already been routed using FP
Follow Profile or AR Auto Rout Outside.
When the AT Auto Tab function is selected, you will notice the
“Configure Tabs” prompt in the Command Window. By selecting
this prompt with your mouse, you can define the tab style of your
breakaway tabs. See the help section for Configuring Tabs.
When the correct style tab has been configured, you will be
prompted for the edge of the board on which you wish to place the
breakaway tab. The selected entity will be highlighted in white
and a rubber-banded line will appear from the current cursor
position perpendicular to the selected rout cut. At this point you
can specify the position of the tab in the following ways:
1) You may press the cursor in the workspace at the
perpendicular location where you wish to place the tab.
2) You may key the perpendicular coordinates in the user panel.
3) You may select the SM Snap Midpoint function to place the
tab in the middle of the currently selected rout cut.
4) You may select the SI Snap Intersection function to place the
tab at the intersection of the currently selected rout entity and a
CAD entity of your choice. This is useful if the location is
specified by a line in the cad drawing.
5)You may key in an X or Y aligned coordinate by keying in
X=1.100, or Y=2.45, or something similar.
The tab will now be shown as it is added to the database.
152
NC-CAM 6 User's Guide
[SI] Snap
Intersection
The SI Snap Intersection function is used when you’re entering a
coordinate, and you want it to be at precisely the point where two
existing entities intersect. The process of using snap intersection,
as described in the progress prompt, is to select the two
intersecting entities, one at a time. Rout then computes the
location of the intersection of the two entities, and enters the
needed coordinate at that location.
In RoutEdit, the SI Snap Intersection command is used for placing
breakaway tabs at positions determined by intersecting CAD
lines. This is particularly useful if you want to place a tab at a
location dimensioned in your CAD data. First select the AT Auto
Tab function and click on the rout segment that you wish to break.
This segment will highlight as a dotted entity. Select the SI
command and you will be prompted in the Command Window to
pick the Select Entity - Intersect. Now you can click on the CAD
line which locates the tab on the routed segment. The tab will
appear where this CAD line intersects the rout.
This snap can be used on routed arcs as well as straight cuts.
Note that the snap intersection function does not require that the
two entities actually intersect; only that they could intersect if they
were long enough to touch each other.
Chapter 6, RoutEdit command reference
153
[SM] Snap
Midpoint
The SM Snap Midpoint function snaps to the midpoint of the line
or arc you select next. The line midpoint chosen is exactly
halfway between its two endpoints.
If you select an arc with the Snap Midpoint function, the
coordinate you’ll snap to is the arc’s midpoint, not its center.
The midpoint of an arc is a point along the arc, such that the point
bisects the arc as shown above.
In RoutEdit, the SM Snap Midpoint command is used for placing
breakaway tabs at the midpoint of the routed segment. First
select the AT Auto Tab function and click on the rout segment
that you wish to break. This segment will highlight as a dotted
entity and a rubber-banded line will appear perpendicular to the
selected entity. Now simple type SM and the breakaway will be
added at the midpoint of the routed segment.
This snap can be used on routed arcs as well as straight cuts.
154
NC-CAM 6 User's Guide
[HL] Comp Left
The HL Comp Left function sets the current comp type to left
compensation. All entities added after this selection will be
comped to the left.
[HN] Comp None
The HN Comp None function sets the current comp type to no
compensation. All entities added after this selection will have no
compensation.
[HR] Comp Right
The HR Comp Right function sets the current comp type to right
compensation. All entities added after this selection will be
comped to the right.
Chapter 6, RoutEdit command reference
155
[AR] Auto Rout
Outside
The AR Auto Rout Outside function is used to create a rout path
using data that exists in the CAD database. When this function is
selected, you must have the CAD data you wish to rout currently
displayed on the screen.
The compensation is selected by using the HL Comp Left, HN
Comp None, HR Comp Right.
When you select this function, you will be prompted to select an
entity to chase. You may select any entity in the CAD database.
Once you have selected the appropriate entity, AR Auto Rout
Outside will follow all the entities connected end to end until one
of three things happens:
1) The chaser finds no more connected entities. It terminates
abnormally, giving you an error indicating that AR Auto Rout
Outside could not link a closed path.
2) The chaser loops back upon itself. It terminates normally,
showing you the closed path it has created.
3) The chaser connects to more than one entity, and can’t figure
out which way to go. In this case, you will be prompted for which
branch to follow. You have two options here. You can stop by
selecting “Stop Here” or you can select OK and select the
direction in which you wish to continue. Notice that the path
already visited is highlighted in white, and the undetermined
directions are highlighted in red. Choose one of the red entities or
press ESC to stop at the current point. Notice that if you stop
before completing the path, the error mentioned in 1) will occur.
Once the AR Auto Rout Outside function terminates, the path will
be added to the Rout database, and shown on-screen.
156
NC-CAM 6 User's Guide
[RI] Auto Rout
Inside
The RI Auto Rout Inside function is very similar to the AR Auto
Rout Outside function. It is used to create a rout path using data
that exists in the CAD database. When this function is selected,
you must have the CAD data you wish to rout currently displayed
on the screen.
The compensation is selected by using the HL Comp Left, HN
Comp None, HR Comp Right.
When you select this function, you will be prompted to select an
entity to chase. You may select any entity in the CAD database.
Once you have selected the appropriate entity, RI Auto Rout
Inside will follow all the entities connected end to end until one of
three things happens:
1) The chaser finds no more connected entities. It terminates
abnormally, giving you an error indicating that RI Auto Rout
Inside could not link a closed path.
2) The chaser loops back upon itself. It terminates normally,
showing you the closed path it has created.
3) The chaser connects to more than one entity, and can’t figure
out which way to go. In this case, you will be prompted for which
branch to follow. You have two options here. You can stop by
selecting “Stop Here” or you can select OK and select the
direction in which you wish to continue. Notice that the path
already visited is highlighted in white, and the undetermined
directions are highlighted in red. Choose one of the red entities or
press ESC to stop at the current point. Notice that if you stop
before completing the path, the error mentioned in 1) will occur.
Once the RI Auto Rout Inside function terminates, the path will
be added to the Rout database, and shown on-screen.
Chapter 6, RoutEdit command reference
157
[FP] Follow Profile
The FP Follow Profile function is used to create a rout path using
data that exists in the CAD database. When this function is
selected, you must have the CAD data you wish to follow
currently displayed on the screen.
The compensation is selected by using the HL Comp Left, HN
Comp None, HR Comp Right.
When you select this function, you will be prompted to select an
entity to chase. You may select any entity in the CAD database.
Once the entity is selected, you will be asked to select the
direction in which to Rout. This is done by selecting the end of
the entity towards which the cutter will travel. To select this end,
press both the left and right mouse buttons at the same time. You
may also change the entity you selected by simply clicking on
another entity.
Once you have selected the appropriate entity and the direction for
travel, FP Follow Profile will follow all the entities connected
end to end until one of three things happens:
1) The chaser finds no more connected entities. It terminates
normally, showing you the path it has created.
2) The chaser loops back upon itself. It terminates normally,
showing you the closed path it has created.
3) The chaser connects to more than one entity, and can’t figure
out which way to go. In this case, you will be prompted for which
branch to follow. You have two options here. You can stop by
selecting “Stop Here” or you can select OK and select the
direction in which you wish to continue. Notice that the path
already visited is highlighted in white, and the undetermined
directions are highlighted in red. Choose one of the red entities or
press ESC to stop at the current point.
Once the Follow Profile function terminates, the path will be
added to the Rout database, and shown on-screen.
158
NC-CAM 6 User's Guide
[OR] Turn on
Ortho Snap
OR Ortho Mode applies a constraint to the cursor motion once a
point has been entered. The constraint acts to force the rout line
you’re creating to be square to the axes, or to the angle you’ve
entered with the OA Ortho Angle function described on the
following page.
When it’s turned on, the Ortho Mode will force newly-created
rout lines square to the ortho angle, even if you snap the second
end of a line you’re creating to some other object.
In one respect, ortho mode acts a bit like the ST Snap Tangent
CAD function described earlier: Once it’s locked on to an axis,
say the “X” axis for example, it stays locked on to that axis no
matter how far you move your mouse along the other axis.
To get the line to swap from being locked on one axis to being
locked on the other, you must move your cursor very close to the
start point of the line.
One final note about Ortho Mode: You may instantly reverse
Ortho Mode’s on/off state by holding down the CTRL key. This is
much quicker than actually pushing the button on the menu.
Chapter 6, RoutEdit command reference
159
[OA] Ortho Angle
The OA Ortho Angle function allows you to set the angle of the
axes used by the OR Ortho Mode to any angle you wish. This is
incredibly handy for routing lines which have a known angle, and
one endpoint you can create with a snap or a keyboarded
coordinate.
The angles you specify with the ortho angle function are measured
in degrees, and the positive angles run counterclockwise with
respect to the right-hand horizontal axis (usually the X+ axis).
Using the ortho angle function automatically turns on ortho mode,
as you’ll see when the ortho mode button automatically flips to the
“on” state when you enter a new ortho angle.
The only catch with using ortho angle is that it’s persistent: Once
you set it to an odd angle, that angle remains the effecive ortho
angle until you select OA a second time, and set the angle back
to zero.
160
NC-CAM 6 User's Guide
[MR] Relative
Mode
The MR Relative Mode toggle affects the way coordinates you
enter are interpreted. Ordinarily, all of the coordinates you enter
are relative to the zero point of your drawing. Sometimes,
however, it’s advantageous for you to be able to enter a coordinate
as a distance from the previous coordinate. That’s what the MR
Relative Mode toggle allows you to do.
Assume for a moment that you have a dimension on a drawing
that’s given as being one-half inch to the right of the upper-right
corner of a rectangle. You could either inspect the rectangle’s
upper right corner, write down its coordinate, add half an inch in
the X axis, and type in the resulting coordinate, or you could use
the MR mode to enter the point.
As shown above, if the point you most recently created is not the
point you’ve got to enter a coordinate relative to, just use NP or
SC to snap the start of a new line to your desired reference point,
then press ESC. Turn on MR, and the numbers you enter will be
relative to that reference point.
Chapter 6, RoutEdit command reference
161
There’s one added point worthy of special mention here: It’s best
to make sure you turn off the MR Relative Mode as soon as
you’re done using it. Forgetting that you’re in relative mode can
lead to some frustration when you later enter coordinates, and
discover that they’re not ending up where you intended them to be.
[PR] Previous Cut
The PR Previous Cut function is active only during single
stepping. It displays the previous cut.
[PL] Next Cut
The PL Next Cut function is active only during single stepping. It
displays the next cut in the Rout database.
[EN] End Single
Step
The EN End Single Step function terminates the single step
process and redisplays the database.
This function is only active during the single step process.
[RW] Previous
Sequence
The RW Previous Sequence function is active only during the
single step process. It rewinds the single step process to the
previous head up.
[FF] Next
Sequence
The FF Next Sequence function allows you to fast forward the
single step process to the next head lift in the database.
162
NC-CAM 6 User's Guide
[DO] Drawing
Origin
The DO Drawing Origin command moves all of the data in your
drawing relative to the drawing origin. This is useful for
temporarily setting the drawing’s origin during editing, as well as
finally establishing the zero point for routing.
[WM] Window
Move
The WM Window Move command allows you to click on an
entity, or click-drag a window around a group of entities, and then
move them.
The process of establishing the from/to positions for the entities to
move is exactly the same as creating a line. This means you can
use the same tricks you’d use in making a line to determine the
exact positions the window moves from and to.
As with many Rout functions, there’s a hidden feature in the
window move, as well as all of the other window functions which
follow: When you select a window full of objects, they become
highlighted on the screen. If you want to add selected entities to
the group to be changed, hold down your SHIFT key and click on
the entities you want to add. You’ll see them become highlighted,
indicating that they’re now included in the group you windowed!
This “shift-click” function also works in reverse: If your window
accidently selected an entity you did not want to include in the
group, use shift-click to deselect it. You’ll see the entity unhighlight, to indicate that it is no longer a member of the selected
group.
Chapter 6, RoutEdit command reference
163
[WS] Window
Stretch
The WS Window Stretch function is used to “lengthen” a board
profile by moving an edge in or out. When this function is
activated, you will be asked to select an entity or select a group of
entities using the click-drag window method to stretch.
When the group of entities is selected, there will be two types of
highlighted entities on the screen. The first type will be the
entities highlighted in white. These entities will simply be moved
to their new location.
The second type of entity that will appear will be red highlighted
entities. These are the entities that will be stretched. The
endpoint of these entities that falls in the selected window will be
moved to its new location, while the endpoint that fell out of the
selected window will stay anchored.
After the entities have been selected, you will be asked to specify
the move vector. The process of establishing the from/to positions
for the entities to move is exactly the same as creating a line.
This means you can use the same tricks you’d use in making a
line to determine the exact positions the window moves from and
to. The function works the same as WM Window Move.
164
NC-CAM 6 User's Guide
[SW] Window
Scale
The SW Window Scale function allows you to stretch or shrink the
windowed entities by the factor you enter, referenced from a point
you select.
Window Scale can alter the windowed group differently in the
horizontal and vertical directions, if you wish. If you do scale a
window asymmetrically, the circles and arcs receive special
treatment: Circles remain circular when scaled asymmetrically,
but the radius of each circle will be altered by the product of the
two scale factors. This means that if you scale a window by 2.0
in the horizontal axis, and 0.3 in the vertical axis, the radii of any
circles you’ve selected will be scaled by 2.0 times 0.3, resulting in
a scale of 0.6:1.
Arcs, on the other hand, actually are scaled asymmetrically. The
treatment given to the arcs follows this procedure: First each arc
has an added point computed for it, the point being the arc’s
midpoint (see the SN function for a definition of this). Then, the
arc’s midpoint, start point, and end point are scaled according to
the two different scale factors you’ve selected. Finally, the arcs
are reconstructed, using the math of the A3 Three-Point Arc
function to reestablish each arc using the three scaled points. This
rather complex process does allow for asymmetrical scaling of
arcs, albeit with arc centers that move as necessary to maintain
equal start and end radii.
[WC] Window
Copy
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
Chapter 6, RoutEdit command reference
165
[WI] Window
Mirror
The WI Window Mirror function copies all of the selected
entities, mirroring around an arbitrary axis line. This powerful
function is very handy for creating copies of individual entities at
odd angles.
It’s probably best for you to experiment with the WI Window
Mirror function a bit before you use it in a live drawing. The
mirror around an arbitrary line tends to be a little confusing, until
you realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[WF] Window Flip
The WF Window Flip function moves all of the selected entities,
mirroring around an arbitrary axis line. This powerful function is
very handy for moving entities to odd angles.
It’s probably best for you to experiment with the WF Window Flip
function a bit before you use it in a live drawing. The mirror
around an arbitrary line tends to be a little confusing, until you
realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[MC] Matrix
Copy
The MC Maxtrix Copy function produces from one to ninety-nine
copies of the selected entities in the X and Y direction, evenly
distributing the copies with spacing you specify.
[RC] Radial Copy
The RC Radial Copy function produces from one to ninety-nine
copies of the selected entities, evenly distributing the copies
across the angle you specify, around the center point you specify.
The icon for this function depicts a radial copy with a quantity of
three, an angle of 360 degrees, and a center point located just
above the bottom rectangle.
166
NC-CAM 6 User's Guide
[RO] Rotate
The RO Rotate function simply rotates all of the selected entities
around a point. The function is extremely useful for working on
sections of drawings which are dimensioned off-axis. By using
the RO function, you can rotate your entire drawing to place the
needed section on-axis, do the editing you need to do, and then use
RO a second time to rotate the entire drawing back to its original
alignment.
[WE] Window
Erase
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
[OO] Undo
The OO Undo function allows you to reverse the effects of your
editing, one step at a time, back to the beginning of your session.
If you place your cursor over the Undo icon, the help text in the
Status Window will describe the function you’re about to reverse.
Note that when you pack the database (with the File/Pack
Database function), the Undo function’s memory is erased.
[UU] Redo
The UU Redo function reverses the effect of the OO Undo
function, one step at a time. This button will be “grayed out” until
you’ve pressed the OO Undo button. As with the OO Undo
icon, if you place your cursor on the UU Redo icon, the help text
will describe the function you’re about to Redo if you press the
button.
Chapter 6, RoutEdit command reference
167
[OI] Object
Inspect
The OI Object Inspect function allows you to select any entity in
the drawing, and view the coordinates of the points making up the
entity. Further, once you’ve selected an entity with OI Object
Inspect, you can modify the entity by clicking on any of its
defining values, and typing in new values. When you do this, the
highlighted entity will instantly change on-screen, and turn red in
color. If you want to restore the entity to its original condition,
press ESC. To keep any change you’ve made, press ENTER.
[ME] Measure
The ME Measure function allows you to measure from any
construction point in your drawing to any other. Further, you may
measure angles by defining a baseline with your first two clicks,
and an angle with the third mouse click.
Once you’ve clicked on three points, you may “pick up” the
endpoints by clicking on them a second time. To reverse the
angle reading in the measure mode, click your mouse near the
apex of the angle.
[SA] Select All
The SA Select All button is unavailable until you’ve selected any
of the window functions. With a window function selected, SA
will automatically select all of the entities in your drawing.
There’s a special capability available with the SA Select All
function. If you want to select everything in your drawing except
what’s inside a window, follow these steps: First, select the
window function you want. Second, window the group you want
excluded from the window operation, and they’ll highlight. Last,
hold the SHIFT key and press the SA Select All button. This will
reverse the selections you’ve made. You may then proceed with
the remaining steps of the window function you originally
selected.
168
NC-CAM 6 User's Guide
[ZW] Zoom In
The ZW Zoom Window function allows you to window a portion
of the screen you want to zoom in on. The creation of this
window is identical to the process of creating a rectangle. After
the zoom region is specified, the work area is redrawn, focusing
in on the area you selected.
The counterpart to this function is the ZB Zoom Back function,
which can be used to decrease the magnification.
A useful new feature of NC-CAM is the ability to pan with a
simple ALT-click-drag combination. If the display was magnified
to show the upper-left-hand portion of your drawing, and you
wanted to "slide" the view over towards the upper-right-hand side
of the drawing, the new pan feature can be used. Hold down the
ALT key, left-click with the mouse on the right-hand side of the
drawing, and drag that location to the left-hand side of the
drawing. In essence, the new pan feature "picks up and drags the
work area," just as you would move a sheet of paper to center in
front of you the area that you wanted to work on.
To repeatedly pick up and move the drawing in this manner, keep
holding down the ALT key, let go of the left mouse button, drag the
mouse to the opposite side of the drawing, left-click the mouse,
and drag back. Advanced users of NC-CAM will learn the clickdrag, click-drag, click-drag motion and grow to use it more often.
[ZA] Zoom All
The ZA Zoom All function redraws the screen at a scale which
will show all of the entities in your drawing.
[ZB] Zoom Out
The ZB Zoom Back function reduces the magnification of the
screen by a factor of two.
The counterpart to this function is the ZW Zoom Window
function, which can be used to increase the magnification.
Chapter 6, RoutEdit command reference
169
[DF] Do First
The DF Do First function allows you to control the sequence of
the cuts in the rout database. This function, with the help of
View|Sequence Number, allows you complete control over the
sequence that the router performs its cuts.
When this function is selected, you are prompted for either an
entity of a window containing several entities. When you select
the entity or group of entities, they will immediately be moved to
the front of the output rout file. With the sequence numbers
showing, you will see the selected entity or group of entities
moved to number 1, etc..
[DB] Do Before
The DB Do Before function is similar to the DF Do First and
DL Do Last functions, with the exception that this function allows
you to shift-click select and unselect group items, and select
where in the rout sequence the selected items are placed.
When you select the DB Do Before function, it will prompt you to
select either an entity or a group of entities. You may either click
on an entity to select just that entity, or you may click-drag a
window around a group of entities. After you select an entity or
group of entities, you can use shift-click to include or exclude cuts
from the group you have selected, in a similar fashion to CAD
window functions.
After you have selected a group of entities to operate on, you will
be prompted to select an entity to place the group before.
The most useful aspect of this function is to do internal cutouts
before cutting the outline of the board loose. To do this, select all
the internal cutouts, then click on the board outline, and all the
internal cutouts will now be routed before the board is cut loose.
You can use Single Step to verify the order visually.
170
NC-CAM 6 User's Guide
[DL] Do Last
The DL Do Last function allows you to control the sequence of
the cuts in the rout database. This function, with the help of
View|Sequence Number, allows you complete control over the
sequence that the router performs its cuts.
When this function is selected, you are prompted for either an
entity of a window containing several entities. When you select
the entity or group of entities, they will immediately be moved to
the end of the output rout file. With the sequence numbers
showing, you will see the selected entity or group of entities
moved to the last number.
[PA] Pan
The PA Pan function, although now mostly obsolete, is included
to keep backwards compatibility with NC-CAM 5. This function
is replaced by the new scheme whereby you hold down the ALT
key, and depress the left mouse button to pan the screen.
With this pan function, however, you will be asked to select a new
center for the screen. When you click the mouse, the location you
select will be the new center of the visible viewing area, with the
same zoom factor.
[OE] Delete
Entity(s)
OE Delete Entity(s) is the same function as WE Window Erase.
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
Chapter 6, RoutEdit command reference
171
[NX] Number in X
The NX Number in X function sets the number of copies made in
the X direction when using the MC Matrix Copy function.
[NY] Number in Y
The NY Number in Y function sets the number of copies made in
the Y direction when using the MC Matrix Copy function.
[XS] X Increment
The XS X Increment function sets the distance between copies
made in the X direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[YS] Y Increment
The YS Y Increment function sets the distance between copies
made in the Y direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[TD] Total
Degrees
The TD Total Degrees function sets the total degrees used during
a RC Radius Copy.
[NC] Number of
Copies
The NC Number of Copies function sets the number of copies
made during a RC Radius Copy.
[RD] Redraw
The RD Redraw function redraws the workspace area. This is
especially useful if you have deleted several entities, and the
deleted entities have "covered" part or all of some entities that
remain.
172
NC-CAM 6 User's Guide
[NP] Snap Near
Point
The NP Snap Near Point function, although only available from
the keyboard, is one of the most useful snap functions in the CAD
snap set. It allows the user to make “perfect” drawings where
there are no gaps left in the corners of a board profile that might
be left if you use freehand drawing.
If you have a 3-button mouse on your computer, the middle button
works as an NP Snap. Simply move the cursor near a point and
press the middle mouse button once to snap to the point.
[MO] Absolute
Mode
This command turns off relative mode which can be used to enter
coordinates in the user panel. This function turns off the relative
mode regardless of the state of the MR Relative Mode button.
[OC] Copy
The OC Copy function in the same as the WC Window Copy
function.
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
[WO] Window
Delete Outside
The WO Window Delete Outside function behaves much like the
WE Window Erase function, with the exception that the entities
deleted are the entities outside of the click-dragged window, not
the entities on the inside.
Chapter 6, RoutEdit command reference
173
[CT] Configure
Tabs
The CT Configure Tabs function allows you to precisely
configure the way that a breakaway tab is inserted into a rout
program when using the AT Auto Tab function.
The large buttons on the left side of the configuration box describe
the available tab types. One of the tab styles features cut-ins,
commonly used to avoid having remaining material from the
breakaway tab stick out over the edge of the profile. Either tab
style may also include drilled holes, to assist in breakability.
The breakaway holes are added to the rout database. They are
output as a G05 command at the end of the rout file.
[AU] Configure
Auto Rout
The AU Configure Auto Rout function allows you to choose
between the different Auto Rout styles, and set specific distances
as they relate to the Auto Rout plunge styles. The diagrams
included on the large buttons on the left side of the dialog box
describe the plunge style, and show how the specifications apply
to that style. The style is selected by pressing the appropriate
button down.
[LF] Link
Sequence First
The LF Link Sequence First function is the same as the DF Do
First function. It allows you to control the sequence of the cuts in
the rout database. This function, with the help of View|Sequence
Number, allows you complete control over the sequence that the
router performs it’s cuts.
When this function is selected, you are prompted for either an
entity of a window containing several entities. When you select
the entity or group of entities, they will immediately be moved to
the front of the output rout file. With the sequence numbers
showing, you will see the selected entity or group of entities
moved to number 1, etc..
174
NC-CAM 6 User's Guide
[EX] Reverse Rout
Path
The EX Reverse Rout Path function allows you to change the
order of the cuts in a specific link to be reversed. Notice that this
function does not change the compensation type, so the path made
by the cutter switches to the other side of the profile edge if the
compensation is set to anything but NONE.
This function is useful for taking internal cutouts that use no
compensation and reversing their order so that the smooth edge of
a one pass routed slot can be changed.
[SR] Step &
Repeat
The SR Step & Repeat function allows you to automatically
create a Step & Repeat pattern for panelization. The inputs for
this function are the number of steps in the X and Y direction, and
the distance between the parts.
When this function is selected, you will be asked to select an
entity or a window. Typically you would select the entire part,
including internal cutouts. Once the part is selected, you may
shift-click to include or exclude different cuts, in the same fashion
as the window operations in CAD.
Once you have selected the appropriate cuts for the Step &
Repeat pattern, you will be asked to confirm the operation by
either hitting ENTER or clicking in the workspace. When you
confirm the operation, you will see the dialog box that allows you
to set the matrix parameters for the Step & Repeat pattern.
The NESTED STEPS checkbox allows you to specify the format
of the Step & Repeat list. If you select nested steps, the resulting
steplist will contain an M01, the list of steps in the X direction,
another M01, and a list of steps in the Y direction. If you deselect
this checkbox, the step list will explicitly list all the steps, with
only one M01.
When OK is selected, the Step & Repeat list is added to the
RoutEdit database and the steps are shown on-screen.
Chapter 6, RoutEdit command reference
175
[SE] Step &
Repeat Edit
The SE Step & Repeat Edit function allows you to edit a Step &
Repeat List already in the database. After you have finished the
edit, the changes will immediately show up on the screen. You
will note that the separate nesting levels are represented by using
multiple edit windows separated by a vertical bar.
[SD] Step &
Repeat Delete
The SD Step & Repeat Delete function allows the user to delete
an existing Step & Repeat pattern from the database.
When the function is selected, it will ask for either an entity or a
group of entities which may be selected using the click-drag
method. Once the entity or group of entities are selected, all the
Step & Repeat information associated with those entities is
immediately deleted.
The results of the delete will be immediately displayed.
[CS] Create Step
& Repeat
The CS Create Step & Repeat allows you to interactively create a
Step & Repeat list in an edit window.
When the function is selected, like SR Step & Repeat, the
function will ask you for an entity or group of entities to which to
apply the Step and Repeat list. Once you have selected the
entities, you may add or delete entities by shift-clicking on
entities.
Once you have established the group of entities to which you wish
to apply the function, you need to confirm the operation by
clicking in the workspace or pressing ENTER. Once you have
confirmed the operation, an edit screen will appear where you can
enter the Step & Repeat list. Once the Step & Repeat is entered,
and the OK button is selected, the Step & Repeat list is applied to
all the selected entities, and displayed in the workspace.
176
NC-CAM 6 User's Guide
[AS] Add to Step
& Repeat
The AS Add to Step & Repeat function is used to add a cut or set
of cuts to an existing Step and Repeat list. This function is
especially useful when adding an internal cut to a part that has
already been panelized using Step & Repeats.
When the function is selected, it will ask you to select either an
entity or group of entities by clicking on an entity or click-dragging
a window around a group of entities. You may add or subtract
entities from the selected group by shift-clicking on the entities.
Once you have selected the group on which to apply the operation,
you must select a stepped entity which has the appropriate Step &
Repeat list to copy.
[XP] Expand Step
& Repeat
The XP Expand Step & Repeat function allows you to expand an
entity or group of entities that are affected by a Step & Repeat list
into the database. This function is useful when there is a need to
modify one part in a panel. Since you cannot modify one part that
is stepped without affecting all the other parts, you must expand
the Step & Repeat list so that each part is routed individually.
When this function is activated, you will be asked to select an
entity or group of entities that are affected by a Step & Repeat
list. They may be selected by clicking on an entity, or selecting a
group of entities by click-dragging a window around them. The
steps are immediately expanded and displayed on the screen.
Chapter 6, RoutEdit command reference
177
[RT] Full Panel
Autorout
The RT Full Panel Autorout function is used to do pocket routing
and create rout programs when the outline of the cutter path is
fully defined in a CAD file. Full Panel Autorout uses the
currently selected cutter and works on all selected active CAD
layers. For each closed polygon that Full Panel Autorout finds, it
creates a fully defined rout path to rout that polygon. If the
polygon contains a large enough region in the middle, two pases
will be created. The first pass will mill out the middle of all of
the polygons. The second pass will cut the outside edges of the
polygons.
As an example of what Full Panel Autorout is capable of, the
following figure illustrates a CAD drawing that fully defines the
rout pathways for a board.
After executing Full Panel Autorout, the workspace would display
the fully defined rout path, as in the following figure.
178
NC-CAM 6 User's Guide
In order for Full Panel Autorout to work, the CAD drawings must
follow several rules. The drawing cannot contain multiple paths
that the algorithm would have to chose from. The polygons must
all be closed off, that is, each polygon must be connected back on
itself. Each entity, line or arc, that is in a polygon must be
connected at both ends to other entities, with no gaps between
them. A polygon cannot cross over itself, for example, in a
bowtie shape, or figure-eight. All pathways in the polygon must
be at least as large as the cutter diameter that will be used. If any
of these rules are broken, the output of Full Panel Autorout is
undefined. Fortunately, like all NC-CAM 6 commands, Full
Panel Autorout can be undone simply by executing OO Undo.
Removing all of the additional information in a CAD drawing
before executing Full Panel Autorout will yield the best results.
Specifically, dimension lines and text must be erased, along with
all other data that is not meant to be routed. If a drawing contains
multiple pathways or is not fully connected, or has chorded arcs,
executing an Automatic Cleanup before attempting a Full Panel
Autorout might take care of all or most of these problems.
Chapter 6, RoutEdit command reference
179
[PC] Pocket Rout
The PC Pocket Rout function allows you to “hog-out” an area of
circuit board as described by a closed path in CAD.
When this function is selected, you will be asked to select a CAD
entity. The cad entity can be any part of a closed polygon in
CAD. Once the CAD entity is selected, the hogged out section of
panel will be added to the rout database, and displayed in the
workspace.
The Pocket Rout function behaves exactly like RT Full Panel
Autorout in all other respects. The most useful aspect of Pocket
Rout is that extraneous data can still be a part of the CAD
drawing, as long as an entity from a polygon which follows all of
the rules listed in RT Full Panel Autorout is selected. In this
manner, single polygons can be selected for automatic routing,
one at a time.
[GC] G32/G33
Circle
The GC G32/G33 Circle command will add a routed circle to the
rout database, by defining the circle’s center point, and secondly,
a point on the edge of the circle. Once you define a center point,
you’ll get a rubber-banded circle that is attached to your cursor,
until you define the point on the circle.
Notice that the routed circle you define is defined just like a G32/
G33 command. The radius of the circle specifies the outside edge
of the routed circle, not the center.
The direction of the routed circle is determined by the current
compensation type. Usually for this function, you want to have
the comp type set to Right Compensation, since this produces the
cleanest routed edge.
180
NC-CAM 6 User's Guide
Chapter 6, RoutEdit command reference
181
182
NC-CAM 6 User's Guide
C
H
A
P
T
E
R
7
DrillEdit command reference
This chapter provides a command-by-command reference to the
NC-CAM 6 DrillEdit functions.
Chapter 7, DrillEdit command reference
183
The functions, in the order presented on the DrillEdit button menu are:
DH Drill Hole
DC Drill Circle
HC Convert Hole To Circle
DT Drill Text
DS Drill Slot
CD Convert Holes to Slot
SC Snap Closest Endpoint
SH Single Hole Slot
HT Convert Single Hole To Slot
TC Window Tool Change
LO Layer Operation
DO Drawing Origin
WM Window Move
MR Relative Mode
SW Window Scale
WC Window Copy
WI Window Mirror
WF Window Flip
MC Matrix Copy
RC Radial Copy
RO Rotate
WE Window Erase
OO Undo
UU Redo
OI Object Inspect
ME Measure
SA Select All
ZW Zoom In
ZA Zoom All
ZB Zoom Out
184
NC-CAM 6 User's Guide
[DH] Drill Hole
The DH Drill Hole function allows you to drill a single hole in a
specified location. It is very similar to the PO Create Point
function in CAD.
This function is primarily used in DrillEdit, however, it is also
available in RoutEdit for creating holes that will be stored at
output time as G05 holes.
[DC] Drill Circle
The DC Drill Circle function creates a drilled circle (G84) in the
drill database, by defining the circles’ center point, and secondly,
a point on the edge of the circle. Once you define a center point,
you’ll get a rubber-banded circle that is attached to your cursor,
until you define the point on the circle.
Notice that the drilled circle you define is defined just like a G84
command. The radius of the circle specifies the outside edge of
the drilled circle, not the center.
[HC] Convert
Hole To Circle
The HC Convert Hole to Circle function is used to convert a hole
in the drill database to a Drilled Circle. When you select the HC
Convert Hole to Circle function, you will notice the blue words
“Configure Circle” appear in the user panel. This is where you
select the radius of the circle. When you click on the text
“Configure Circle”, a dialog box will appear with the current
radius value.
The HC Convert Hole to Circle function acts like a snap
command. When you select the function, you will need to select
the hole which to convert. By clicking in the workspace, you will
select the closest active hole and convert it to a circle.
Chapter 7, DrillEdit command reference
185
[DT] Drill Text
The DT Drill Text function creates a drilled text command (M97/
M98) in the drill database, by defining the lower left corner of the
drilled text’s first letter. (Note: if you are adding vertical text, the
point selected actually refers to the lower right of the drilled text,
due to the 90 degree rotation.) Once the location is selected (by
either clicking in the workspace with the mouse or typing the
coordinates in the user panel), a dialog will appear asking for the
text and the orientation of the text. After selecting OK, the text
will appear in the workspace.
Note: The text does not need to be entered with commas
seperating the words instead of spaces, as is neccesary in an
Excellon drill program. DrillEdit automatically substitutes the
spaces with commas at output time.
[DS] Drill Slot
The DS Drill Slot function allows you to add a drilled slot (G85)
command to the drill database. The slot may optionally be
expanded at output time.
When you create a slot, you will be prompted to enter the first
endpoint. After you do, you’ll notice a “rubber-banded” line
connecting the first endpoint to the cursor. When you define the
second endpoint, the rubber-banded line will change to a drilled
slot in the drill database.
Note that in order to use this function, you must know both
endpoints of the slot. If you have a center point, angle and length
specification for the slot, use the SH Single Hole Slot function
instead.
[CD] Convert
Holes to Slot
The CD Convert Holes to Slot (Convert Double) function is used
to create a slot in the drill database whose length and orientation
is specified by two existing holes in the database. When this
function is selected, you will simply be promted for the two holes
that specify the slot. Select the two holes that define the slot, and
the two holes will be deleted from the database, replaced by a
slot.
186
NC-CAM 6 User's Guide
[SC] Snap Closest
Endpoint
The SC Snap Closest function is used when you’re entering a
coordinate and you want it to be exactly the same as an existing
coordinate in the drawing. To use snap closest, you simply select
the function, then move the cursor close to the point you wish to
snap to, and press your left mouse button.
There’s a similar function that’s actually used more often than
SC by experienced CAD users, and that is the NP Near Point
function. Unlike the SC function, NP does not require that you
click your left mouse button. Instead, it snaps immediately when
you enter NP on the keyboard. This immediate snap, and the fact
that you don’t have to move your mouse over to the menu and then
back to the desired point, save a considerable amount of time.
Obviously, there’s no point in having a menu button for NP,
because you’d have to have your mouse on the menu and not near
the snap point in order to press the button! An alternate way to
select NP is to click the middle mouse button, if you have a
three-button mouse.
There’s one aspect of SC and NP that’s not obvious to first-time
users: There are more snappable points than you can ordinarily
see on the screen. This is because both arcs and circles have
construction points at their centers. These points become visible
only when you turn on the View|Const Points function, but they
may always be used for snapping.
If you have a 3-button mouse on your computer, the middle button
works as an SP Snap. Simply move the cursor near a point and
press the middle mouse button once to snap to the point.
Chapter 7, DrillEdit command reference
187
[SH] Single Hole
Slot
The SH Single Hole Slot function is used to add a drilled slot
(G85) command to the database. To add a slot to the database
using this function, you must know the center point of the slot, it’s
orientation (in degrees) and the length of the slot. If the slot
specification you have specifies two endpoints instead, use the
DS Drill Slot command instead.
When you select the SH Single Hole Slot function, you will notice
a blue “Configure Slots” prompt in the user panel. Use your
mouse to click on this prompt to enter the orientation and the
length of the slot. Once you have entered the orientation and
length, select OK.
You will then be prompted for the center point of the slot. You
may either key in the coordinates in the user panel or select the
location using the cursor in the workspace. Once the point is
selected, the drilled slot will appear as it is added to the drill
database.
[HT] Convert
Single Hole To Slot
The HT Convert Single Hole To Slot function is used to add a
drilled slot (G85) command to the database, using an existing hole
as the center location. To add a slot to the database using this
function, you must know the slot's orientation (in degrees) and the
length of the slot. If the slot specification you have specifies two
endpoints instead, use the CD Convert Two Holes to Slot
command instead.
When you select the HT Convert Single Hole To Slot function,
you will notice a blue “Configure Slots” prompt in the user panel.
Use your mouse to click on this prompt to enter the orientation
and the length of the slot. Once you have entered the orientation
and length, select OK.
You will then be prompted for the holes specifying the center
point of the slot. Use the cursor to select the drilled hole you wish
to convert. Once the hole is selected, the hole will be deleted,
and a drilled slot will appear as it is added to the drill database.
188
NC-CAM 6 User's Guide
[TC] Window Tool
Change
The TC Window Tool Change function allows you to select
multiple drilled holes and change them all to one tool number.
When this function is selected, it will ask for a new tool number.
Once the tool number is selected, you may select any entity or
group of entities which will be immediately changed, and the
display will show the altered holes. Selection of entities is
identical to the selection method for Window Erase.
[LO] Layer
Operation
The LO Layer Operation function allows you to move entities
from one layer to another. This function may be used in the
following two ways:
1) When this button is pressed by itself, the function acts like
WE Window Erase, with one difference. The selected entities
are not erased, they are merely moved to the layer specified in the
user panel. The selection of entities, however, is exactly the
same as WE Window Erase. You can use Layer Operation to
move either single entities or windowed groups of entities. This
window function does not, however, allow you to select multiple
entities using the shift-click approach described in the WM
Window Move function: When you select an entity by clicking on
it, or a group of entities with a click-drag window, they are moved
immediately.
2) The Layer Operation function may be applied to any window
edit function as well. To do so, first pick the operation you wish
to perform. Then select Layer Operation. The result of the
operation, instead of landing on the construction layer, will be
placed on the layer selected in the user panel instead. Notice that
doing a Window Move still requires you to select the offset when
using this function.
Chapter 7, DrillEdit command reference
189
[DO] Drawing
Origin
The DO Drawing Origin command moves all of the data in your
drawing relative to the drawing origin. This is useful for
temporarily setting the drawing’s origin during editing, as well as
finally establishing the zero point for routing.
[WM] Window
Move
The WM Window Move command allows you to click on an
entity, or click-drag a window around a group of entities, and then
move them.
The process of establishing the from/to positions for the entities to
move is exactly the same as creating a line. This means you can
use the same tricks you’d use in making a line to determine the
exact positions the window moves from and to.
As with many CAD functions, there’s a hidden feature in the
window move, as well as all of the other window functions which
follow: When you select a window full of objects, they become
highlighted on the screen. If you want to add selected entities to
the group to be changed, hold down your SHIFT key and click on
the entities you want to add. You’ll see them become highlighted,
indicating that they’re now included in the group you windowed!
This “shift-click” function also works in reverse: If your window
accidently selected an entity you did not want to include in the
group, use shift-click to deselect it. You’ll see the entity unhighlight, to indicate that it is no longer a member of the selected
group.
190
NC-CAM 6 User's Guide
[MR] Relative
Mode
The MR Relative Mode toggle affects the way coordinates you
enter are interpreted. Ordinarily, all of the coordinates you enter
are relative to the zero point of your drawing. Sometimes,
however, it’s advantageous for you to be able to enter a coordinate
as a distance from the previous coordinate. That’s what the MR
Relative Mode toggle allows you to do.
Assume for a moment that you have a dimension on a drawing
that’s given as being one-half inch to the right of the upper-right
corner of a rectangle. You could either inspect the rectangle’s
upper right corner, write down its coordinate, add half an inch in
the X axis, and type in the resulting coordinate, or you could use
the MR mode to enter the point.
As shown above, if the point you most recently created is not the
point you’ve got to enter a coordinate relative to, just use NP or
SC to snap the start of a new line to your desired reference point,
then press ESC. Turn on MR, and the numbers you enter will be
relative to that reference point.
Chapter 7, DrillEdit command reference
191
There’s one added point worthy of special mention here: It’s best
to make sure you turn off the MR Relative Mode as soon as
you’re done using it. Forgetting that you’re in relative mode can
lead to some frustration when you later enter coordinates, and
discover that they’re not ending up where you intended them to be.
[SW] Window
Scale
The SW Window Scale function allows you to stretch or shrink the
windowed entities by the factor you enter, referenced from a point
you select.
Window Scale can alter the windowed group differently in the
horizontal and vertical directions, if you wish. If you do scale a
window asymmetrically, the circles and arcs receive special
treatment: Circles remain circular when scaled asymmetrically,
but the radius of each circle will be altered by the product of the
two scale factors. This means that if you scale a window by 2.0
in the horizontal axis, and 0.3 in the vertical axis, the radii of any
circles you’ve selected will be scaled by 2.0 times 0.3, resulting
in a scale of 0.6:1.
Arcs, on the other hand, actually are scaled asymmetrically. The
treatment given to the arcs follows this procedure: First each arc
has an added point computed for it, the point being the arc’s
midpoint (see the SN function for a definition of this). Then, the
arc’s midpoint, start point, and end point are scaled according to
the two different scale factors you’ve selected. Finally, the arcs
are reconstructed, using the math of the A3 Three-Point Arc
function to reestablish each arc using the three scaled points. This
rather complex process does allow for asymmetrical scaling of
arcs, albeit with arc centers that move as necessary to maintain
equal start and end radii.
[WC] Window
Copy
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
192
NC-CAM 6 User's Guide
[WI] Window
Mirror
The WI Window Mirror function copies all of the selected
entities, mirroring around an arbitrary axis line. This powerful
function is very handy for creating copies of individual entities at
odd angles.
It’s probably best for you to experiment with the WI Window
Mirror function a bit before you use it in a live drawing. The
mirror around an arbitrary line tends to be a little confusing, until
you realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[WF] Window Flip
The WF Window Flip function moves all of the selected entities,
mirroring around an arbitrary axis line. This powerful function is
very handy for moving entities to odd angles.
It’s probably best for you to experiment with the WF Window Flip
function a bit before you use it in a live drawing. The mirror
around an arbitrary line tends to be a little confusing, until you
realize that the arbitrary line acts just like a “fold” in your
drawing. A reasonable metaphor for the function would be that
the windowed entities are “folded” around your arbitrary line.
[MC] Matrix
Copy
The MC Maxtrix Copy function produces from one to ninety-nine
copies of the selected entities in the X and Y direction, evenly
distributing the copies with spacing you specify.
[RC] Radial Copy
The RC Radial Copy function produces from one to ninety-nine
copies of the selected entities, evenly distributing the copies
across the angle you specify, around the center point you specify.
The icon for this function depicts a radial copy with a quantity of
three, an angle of 360 degrees, and a center point located just
above the bottom rectangle.
Chapter 7, DrillEdit command reference
193
[RO] Rotate
The RO Rotate function simply rotates all of the selected entities
around a point. The function is extremely useful for working on
sections of drawings which are dimensioned off-axis. By using
the RO function, you can rotate your entire drawing to place the
needed section on-axis, do the editing you need to do, and then use
RO a second time to rotate the entire drawing back to its original
alignment.
[WE] Window
Erase
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
[OO] Undo
The OO Undo function allows you to reverse the effects of your
editing, one step at a time, back to the beginning of your session.
If you place your cursor over the Undo icon, the help text in the
Status Window will describe the function you’re about to reverse.
Note that when you pack the database (with the File/Pack
Database function), the Undo function’s memory is erased.
[UU] Redo
The UU Redo function reverses the effect of the OO Undo
function, one step at a time. This button will be “grayed out” until
you’ve pressed the OO Undo button. As with the OO Undo
icon, if you place your cursor on the UU Redo icon, the help text
will describe the function you’re about to Redo if you press the
button.
194
NC-CAM 6 User's Guide
[OI] Object
Inspect
The OI Object Inspect function allows you to select any entity in
the drawing, and view the coordinates of the points making up the
entity. Further, once you’ve selected an entity with OI Object
Inspect, you can modify the entity by clicking on any of its
defining values, and typing in new values. When you do this, the
highlighted entity will instantly change on-screen, and turn red in
color. If you want to restore the entity to its original condition,
press ESC. To keep any change you’ve made, press ENTER.
[ME] Measure
The ME Measure function allows you to measure from any
construction point in your drawing to any other. Further, you may
measure angles by defining a baseline with your first two clicks,
and an angle with the third mouse click.
Once you’ve clicked on three points, you may “pick up” the
endpoints by clicking on them a second time. To reverse the
angle reading in the measure mode, click your mouse near the
apex of the angle.
[SA] Select All
The SA Select All button is unavailable until you’ve selected any
of the window functions. With a window function selected, SA
will automatically select all of the entities in your drawing.
There’s a special capability available with the SA Select All
function. If you want to select everything in your drawing except
what’s inside a window, follow these steps: First, select the
window function you want. Second, window the group you want
excluded from the window operation, and they’ll highlight. Last,
hold the SHIFT key and press the SA Select All button. This will
reverse the selections you’ve made. You may then proceed with
the remaining steps of the window function you originally
selected.
Chapter 7, DrillEdit command reference
195
[ZW] Zoom In
The ZW Zoom Window function allows you to window a portion
of the screen you want to zoom in on. The creation of this
window is identical to the process of creating a rectangle. After
the zoom region is specified, the work area is redrawn, focusing
in on the area you selected.
The counterpart to this function is the ZB Zoom Back function,
which can be used to decrease the magnification.
A useful new feature of NC-CAM is the ability to pan with a
simple ALT-click-drag combination. If the display was magnified
to show the upper-left-hand portion of your drawing, and you
wanted to "slide" the view over towards the upper-right-hand side
of the drawing, the new pan feature can be used. Hold down the
ALT key, left-click with the mouse on the right-hand side of the
drawing, and drag that location to the left-hand side of the
drawing. In essence, the new pan feature "picks up and drags the
work area," just as you would move a sheet of paper to center in
front of you the area that you wanted to work on.
To repeatedly pick up and move the drawing in this manner, keep
holding down the ALT key, let go of the left mouse button, drag the
mouse to the opposite side of the drawing, left-click the mouse,
and drag back. Advanced users of NC-CAM will learn the clickdrag, click-drag, click-drag motion and grow to use it more often.
[ZA] Zoom All
The ZA Zoom All function redraws the screen at a scale which
will show all of the entities in your drawing.
[ZB] Zoom Out
The ZB Zoom Back function reduces the magnification of the
screen by a factor of two.
The counterpart to this function is the ZW Zoom Window
function, which can be used to increase the magnification.
196
NC-CAM 6 User's Guide
[PA] Pan
The PA Pan function, although now mostly obsolete, is included
to keep backwards compatibility with NC-CAM 5. This function
is replaced by the new scheme whereby you hold down the ALT
key, and depress the left mouse button to pan the screen.
With this pan function, however, you will be asked to select a new
center for the screen. When you click the mouse, the location you
select will be the new center of the visible viewing area, with the
same zoom factor.
[OE] Delete
Entity(s)
OE Delete Entity(s) is the same function as WE Window Erase.
The WE Window Erase function erases single entities, or
windowed groups of entities. This is the only window function
which does not allow you to select multiple entities with the shiftclick approach described in the WM Window Move function:
When you select an entity by clicking on it, or a group of entities
with a click-drag window, they are deleted immediately.
Because the windowing functions in NC-CAM’s CAD editor also
allow you to select an individual entity by doing a simple click
(instead of a click-drag), this function is also used for individual
deletes. This replaces the OE Object Erase function GCADD
users will be familiar with.
[NX] Number in X
The NX Number in X function sets the number of copies made in
the X direction when using the MC Matrix Copy function.
[NY] Number in Y
The NY Number in Y function sets the number of copies made in
the Y direction when using the MC Matrix Copy function.
Chapter 7, DrillEdit command reference
197
[XS] X Increment
The XS X Increment function sets the distance between copies
made in the X direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[YS] Y Increment
The YS Y Increment function sets the distance between copies
made in the Y direction when using the MC Matrix Copy
function. You can not reach this command directly, it is only a
part of the MC Matrix Copy command.
[TD] Total
Degrees
The TD Total Degrees function sets the total degrees used during
a RC Radius Copy.
[NC] Number of
Copies
The NC Number of Copies function sets the number of copies
made during a RC Radius Copy.
[RD] Redraw
The RD Redraw function redraws the workspace area. This is
especially useful if you have deleted several entities, and the
deleted entities have "covered" part or all of some entities that
remain.
[NP] Snap Near
Point
The NP Snap Near Point function, although only available from
the keyboard, is one of the most useful snap functions in the CAD
snap set. It allows the user to make “perfect” drawings where
there are no gaps left in the corners of a board profile that might
be left if you use freehand drawing.
198
NC-CAM 6 User's Guide
The NP Snap Near Point function requires only that you move the
mouse near the point you want to snap on and then type NP. If
you have a 3-button mouse, clicking on the middle button does the
same thing as type NP.
[MO] Absolute
Mode
This command turns off relative mode which can be used to enter
coordinates in the user panel. This function turns off the relative
mode regardless of the state of the MR Relative Mode button.
[OC] Copy
The OC Copy function in the same as the WC Window Copy
function.
The WC Window Copy function allows you to copy all of the
selected entities. After you select the entity or entities to be
copied, you define the point to copy from, and the point to copy to.
The “from” and “to” points may be entered as you’d enter any
coordinate, but usually you’ll want to use a snap or key in the
values.
[WO] Window
Delete Outside
The WO Window Delete Outside function behaves much like the
WE Window Erase function, with the exception that the entities
deleted are the entities outside of the click-dragged window, not
the entities on the inside.
Chapter 7, DrillEdit command reference
199
[LR] Target Layer
The LR Target Layer function allows you to set the layer where
LO Layer Operation functions will land.
[SR] Step &
Repeat
The SR Step & Repeat function allows you to automatically
create a Step & Repeat pattern for panelization. The inputs for
this function are the number of steps in the X and Y direction, and
the distance between the parts.
When this function is selected, you will be asked to select an
entity or a window. Typically you would select the entire part.
Once the part is selected, you may shift-click to include or
exclude different holes, in the same fashion as the window
operations in CAD.
Once you have selected the appropriate holes for the Step &
Repeat pattern, you will be asked to confirm the operation by
either hitting ENTER or clicking in the workspace. When you
confirm the operation, you will see the dialog box that allows you
to set the matrix parameters for the Step & Repeat pattern.
The NESTED STEPS checkbox allows you to specify the format
of the Step & Repeat list. If you select nested steps, the resulting
steplist will contain an M01, the list of steps in the X direction,
another M01, and a list of steps in the Y direction. If you deselect
this checkbox, the step list will explicitly list all the steps, with
only one M01.
When OK is selected, the Step & Repeat list is added to the
DrillEdit database and the steps are shown on-screen.
200
NC-CAM 6 User's Guide
[SE] Step &
Repeat Edit
The SE Step & Repeat Edit function allows you to edit a Step &
Repeat List already in the database. After you have finished the
edit, the changes will immediately show up on the screen. You
will note that the separate nesting levels are represented by using
multiple edit windows separated by a vertical bar.
[SD] Step &
Repeat Delete
The SD Step & Repeat Delete function allows the user to delete
an existing Step & Repeat pattern from the database.
When the function is selected, it will ask for either an entity or a
group of entities which may be selected using the click-drag
method. Once the entity or group of entities are selected, all the
Step & Repeat information associated with those entities is
immediately deleted.
The results of the delete will be immediately displayed.
[CS] Create Step
& Repeat
The CS Create Step & Repeat allows you to interactively create a
Step & Repeat list in an edit window.
Chapter 7, DrillEdit command reference
201
When the function is selected, like SR Step & Repeat, the
function will ask you for an entity or group of entities to which to
apply the Step and Repeat list. Once you have selected the
entities, you may add or delete entities by shift-clicking on
entities.
Once you have established the group of entities to which you wish
to apply the function, you need to confirm the operation by
clicking in the workspace or pressing ENTER. Once you have
confirmed the operation, an edit screen will appear where you can
enter the Step & Repeat list. Once the Step & Repeat is entered,
and the OK button is selected, the Step & Repeat list is applied to
all the selected entities, and displayed in the workspace.
[AS] Add to Step
& Repeat
The AS Add to Step & Repeat function is used to add a hole or set
of holes to an existing Step and Repeat list. This function is
especially useful when adding holes to a part that has already been
panelized using Step & Repeats.
When the function is selected, it will ask you to select either an
entity or group of entities by clicking on an entity or click-dragging
a window around a group of entities. You may add or subtract
entities from the selected group by shift-clicking on the entities.
Once you have selected the group on which to apply the operation,
you must select a stepped entity which has the appropriate Step &
Repeat list to copy.
[XP] Expand Step
& Repeat
The XP Expand Step & Repeat function allows you to expand an
entity or group of entities that are affected by a Step & Repeat list
into the database. This function is useful when there is a need to
modify one part in a panel. Since you cannot modify one part that
is stepped without affecting all the other parts, you must expand
the Step & Repeat list so that each part is routed individually.
202
NC-CAM 6 User's Guide
When this function is activated, you will be asked to select an
entity or group of entities that are affected by a Step & Repeat
list. They may be selected by clicking on an entity, or selecting a
group of entities by click-dragging a window around them. The
steps are immediately expanded and displayed on the screen.
[HS] Configure
Single Hole Slot
This function configures what a slot will look like when you
create a slot using SH Single Hole Slot. When this function is
selected a dialog will appear with the angle of the slot, and the
length of the slot.
[CE] Configure
Single Hole Circle
This function describes what a drilled circle created by HC
Convert Hole to Circle will look like. The only thing to configure
here is the radius of the drilled circle.
Chapter 7, DrillEdit command reference
203
204
NC-CAM 6 User's Guide
P
A
R
T
3
Appendices
Appendix A, In case of difficulty
205
206
NC-CAM 6 User's Guide
A
P
P
E
N
D
I
X
A
In case of difficulty
This appendix provides information on solving problems one might
encounter when installing or configuring NC-CAM.
Appendix A, In case of difficulty
207
READ.ME for NC-CAM 6
Be sure to read the READ.ME that is included with your
NC-CAM distribution!
IMPORTANT INSTRUCTIONS for first time users:
You must install lock drivers to allow this software to talk to the
software security lock. If you fail to do this, the software will not
run. The instructions follow below:
Windows NT
Users only:
1. Under the Microsoft Windows NT Main group, double click
on “Command Prompt”.
2. Change drive to the drive containing the NC-CAM 6 files.
Change directory to WIN_NT subdirectory. The current path
should now be something like C:\NCCAM6\WIN_NT>
3. Type “INSTALL.BAT” at the command prompt. There are
two command line options: (See the INSTALL.BAT file for
examples.) 1. /q Quiet mode. Normal dialogs described below
are not displayed. Error messages are displayed. 2. /pxxx Path,
where xxx is the path of files to be installed. Specify the path of
files to be installed. Otherwise, files will be copied from the
default directory.
4. A window with the title bar “Sentinel Driver Setup Program”
is displayed.
5. Select “Functions” and then “Install Sentinel Driver” from
the menu bar.
6. A dialog box with the default path for the NT driver is
displayed. Change the drive letter if necessary and click “OK”.
7. The Sentinel Driver and associated files are copied to the
hard disk. One of the DLLs, SNTI386.DLL, SNTMIPS.DLL,
SNTALPHA.DLL, or SNTPPC.DLL and SENTTEMP.HLP are
copied to \%SYSTEMROOT%\SYSTEM32. SENTTEMP.SYS is
copied to the file
\%SYSTEMROOT%\SYSTEM32\DRIVERS\SENTINEL.SYS.
%SYSTEMROOT% is the directory where Microsoft Windows
NT has been installed.
208
NC-CAM 6 User's Guide
8. If the driver installation is successful, a dialog box with the
message “Sentinel Driver Files Copied Successfully” is
displayed.
9. When complete, a dialog box with the message “Driver
Installed! Restart your system” is displayed.
10. Click “OK” to continue.
11. Restart your computer.
Windows
95/98/2000:
1. Start Windows. Select “Run” from the Taskbar and run the
file SENTW95.EXE in the \NCCAM6\WIN_95 (98 or 2000)
subdirectory on the drive where NC-CAM 6 is installed. There
are two command line options: 1. /q Quiet mode. Normal
dialogs described below are not displayed. Error messages are
displayed. 2. /pxxx Path, where xxx is the path of files to be
installed. Specify the path of files to be installed. Otherwise, files
will be copied from the default directory.
2. Select “Install Sentinel Driver” from the “Functions” menu.
3. Click “OK” when the “Driver installed! Restart your
system.” message appears. Restart Windows.
4. The following files have been created on your hard disk:
WINDOWS\SYSTEM\SENTINEL.VXD
WINDOWS\SYSTEM\RNBOSENT\SENTW95.EXE
WINDOWS\SYSTEM\RNBOSENT\SENTW95.DLL
WINDOWS\SYSTEM\RNBOSENT\SENTW95.HLP
WINDOWS\SYSTEM\RNBOSENT\SENTINEL.SAV
Appendix A, In case of difficulty
209
General
equipment
requirements
NC-CAM 6 is a Windows Native 32-bit program. You need to
have either Windows NT (3.5 and up) Windows 95, 98 or 2000 to
run this software.
The recommended system(s) for NC-CAM are as follows:
Windows with the latest Service Packs installed. (Please see the
note below on service packs). A Pentium 90 or faster. 32 megs
of RAM.
The minimum platform for Windows is a 486-DX2-66 with 32
megs of RAM.
Notice that the above requirements are the requirements that
Microsoft sets for a machine as an absolute minimum to run the
operating system. We do NOT recommend attemptin to run NCCAM on a system configured as such, since the speed will greatly
suffer.
Please use Microsoft’s Web Site, http://www.microsoft.com, to
download the latest service packs. These service packs fix
operating system bugs, which may cause an application to behave
incorrectly. When you call for Tech Support from
FASTechnologies, we will ask you to install the latest service
packs in order to aid us in correctly diagnosing your problem.
Lock authorization
Please contact FASTechnologies for authorization codes for this
product.
210
NC-CAM 6 User's Guide
A
P
P
E
N
D
I
X
B
Frequently-asked questions
This appendix provides a list of frequently-asked questions and
their answers.
Appendix B, Frequently-asked questions
211
Q: Why doesn't NC-CAM recognize the lock?
Plug your FASTechnologies lock into your printer port first, before
any locks for other software products.
Q: How do I make sure my drill and rout output register to each other?
The best way to output drill and rout programs so that they register
together is to set the zero points you use in Drill, Rout, and CAD
to the zero point of your drill/routing machines. This eliminates
the need for G93 offsets and simplifies programming and
troubleshooting of finished files.
For this example, start in the lower left corner of the panel:
1)Program drill hits using the default position of the X-Y origin as
the zero-zero of the print data.
2)Panelize the data to the desired number up using Auto Step &
Repeat.
3)Draw a single board image in CAD
4)Move the origins of the Drill and CAD functions to the drill/
routing machine zero-zero. For drill and rout, move Job Datum to
zero and then set G93 offset to 0,0 by using Panel Origin
command. For CAD, move Drawing Origin to the machine zero.
At this point the CAD outline should register to the drill data
matching the information on the engineering drawing. It should
look like a finished PCB.
5)Use DXF CAD outline of board to program the rout for a single
board. The co-ordinates of the rout data will be absolute when
measured from the machine origin point with no offset.
6)Use Auto Step and Repeat to multiply the rout images.
7)Output drill file using Make Drill Tape command with Output
G93 Offset turned off.
8)There are options in the view menu to allow viewing of drill,
rout, and cad together in the Rout and CAD portions of the
software.
212
NC-CAM 6 User's Guide
Q: How do I read old Excellon Rout programs into CAD?
You can Import an Excellon rout file into the CAD portion of
NC-CAM 6 to create a DXF file of the board outline. The
Excellon data is automatically compensated and changed into an
editable DXF file.
Appendix B, Frequently-asked questions
213
214
NC-CAM 6 User's Guide
I
N
D
E
Symbols
D
2D CAD database 100
Delete Entity 143
dimensions 55
DO 136
double hits 106
Drawing Origin 136
drill program, output 110
duplicated lines 85
A
A2 76, 118
A3 118
Absolute Mode 145, 78
Angle 128
Arc 54, 76, 118
Arc Center 122
arcs, making 76
array, radial 139
B
Breaking lines 82, 133
C
C2 119
CA 145
CAD drawings 52
CB 145
Center, snap 59
CH 134
Chamfer 134
Chamfer Distance 67, 145
Check/Test Path 83
Circle 54, 119
Closest 119
Closest, Snap 59
Command Line 68
construction points 119
coordinate 55, 73, 129
coordinate entry mode 78
Copy 138, 146
cutting lines and arcs 79
Index
X
E
Entities 68
Erase 140
extend 79
F
File/Import 94
File/Make Drill Tape 110
File/Save 83
File/Save As... 75
File/Spacing Check 106
Fillet 69, 135
Fillet Radius 144
First Drill Program 94
first-hit/last-hit coupon 105
FL 69, 135
flash commands 117
FLH-COUP 105
Flip 139
FR 144
215
G
G93 97
gaps 85
Generic CADD 53
H
N
help, fly-by 53
I
Inspect 102, 141
Inspect, CAD 73
Insure your lock 14
Intersection 120
intersection, CAD, defined 66
intersection, selecting in CAD 66
Intersection, snap 59
J
JO 85, 132
Join 132
Join Lines 85
L
Layer Operation
layers? 94
Line 117
Lines 54
LO 126
LS 146
126
M
magnification 142
main part 97
Make Drill Tape 110
Matrix Copy 139
MC 139
ME 70, 141
Measure 70, 141
Measuring the distance between 2 holes 104
Measuring, in CAD 70
Midpoint 121
216
Midpoint, Snap 59
Mirror 139
MO 145
modal function 78
MR 78, 129
multiple hits 106
nanometer 10
NC 144
near double hits 106
Near Point 119
Nearest Point 59
NP 59, 119, 145
NX 144
NY 144
O
OA 117, 128
OB 82, 133
Object Break 82, 133
Object Erase 140
Object Inspect 73, 141
OC 146
OE 140, 143
OI 73, 141
OO 61, 140
OR 127
origin 136
Ortho Angle 117, 128
Ortho Mode 127
orthogonal 117
overlapping lines 85
P
PA 143
Pan 142, 143
Parallel 125
Path 146
Perpendicular 124
Perpendicular, snap 59
PO 117
Point 117
NC-CAM 6 User's Guide
Points 54, 68
profile-follower 84
Progress Prompt 68
R
Radial Copy 139
Radiused corners 69
RC 139
RD 85, 145
RE 118
Rectangle 118
Redo 62, 141
Redraw 145
Refresh 85
Relative Mode 78, 129
Relative mode 78
resolution 10
RM 80, 130
RO 140
Rotate 140
round-off 10
S
SA 142
SC 59, 62, 82, 119
Scale 138
second-drill 94
Select All 142
SI 59, 120
SL 125
SM 59, 77
SN 59, 122
Snap Arc Center 122
Snap Center 59
Snap Closest 59, 62, 82, 119
Snap Intersection 59, 120
Snap Midpoint 59, 77, 121
Snap Near Point 145
Snap Parallel 125
Snap Perpendicular 59, 124
Snap Tangent 59, 123
Snaps 59
Snaps with other functions 77
Index
SP 59, 124
Spacing check 106
ST 59, 123
Stretch 137
SW 138
T
Tangent 123
Tangent, snap 59
Target Layer 146
TD 144
Test Path 83, 146
Three-Point Arc 118
tool assignments 105
Tool tables 105
Tools/Show Tool Table 105
Tools/Sort Small Tool First 105
TP 146
trigonometric functions 60
Trim 130
Trim Line 80
Trims 79
Two-Point Arc 118
U
Undo 61, 140
units 103
UU 62, 141
V
View Input File 96
View Refresh 85
View/Zoom All 98
View/Units 103
W
WC 138
WE 85, 140
WF 139
WI 139
width 54
217
Window Copy 138
Window Delete Outside 146
Window editing 109
Window Erase 85, 140
Window Flip 139
Window Mirror 139
Window Move 136
Window Scale 138
Window Stretch 137
WM 136
WO 146
work area 10
X
XS 144
Y
YS 144
Z
ZA 143
ZB 83, 143
Zoom All 57, 143
Zoom Back 83, 143
Zoom Window 142, 143
ZW 142, 143
218
NC-CAM 6 User's Guide
Index
219
220
NC-CAM 6 User's Guide