ShopCAM 2006 Reference Guide


Five Steps of Part-Programming. 3

Picking Geometry. 3

Pick Modes. 3

Picking with a Window.. 3

Picking By Selecting. 4

Picking via Chain. 4

Pick lasso. 5

Pick last layer 5

Select layer 5

Quick Keys Chart 5


Crosshair Cursors. 6

Round Cursor [F2] 6

Box Cursor [F3] 6

Intersection CURSOR [F4] 6

Sprite Cursor 6

Trimming. 7

Trim Modal 8

Breaking. 8

Copying and Rotating. 9

Setup File, Tool & Material libraries. 9

The Setup File. 9

Setup File parameter summary. 9

First Operation Default 10

Determining The Tool Side. 11

Coordinates. 11

Cartesian Notation. 12

Zero Degrees. 12

Two Dimensional Angles. 12

Units of measurement 12


File Types. 13

Standard Operation Dialog. 14

Operation Dialog. 14

Standard parameter summary. 14

Standard Lathe parameter summary. 15


Command Menus – The command menus are the heart of the SHOPCAM system. All functions are performed by selecting one of these items.


Command Icons – The command icons are Shortcuts located on the toolbar. The command icons perform identical functions found in the Command Menus.


Operational Icons – When a command icon is selected, this area displays the icons that show the individual choices within that command.  For instance, the line icon will display all the commands for making lines.

Command Prompts – SHOPCAM displays messages on the Status Bar during each command. You should look at this area. If you are unsure what to do, refer to this prompt. If the display is empty, this is an indication that no function or command is active.


Pointer Location – The pointer location is the current X, Y, and Z position of your mouse.







Five Steps of Part-Programming

  Although it is not required to name your part until you save the file, it is good practice to name your file as soon as possible.  You can give your part program any name but, it must follow the Windows standard for file naming (refer to Windows documentation for more information).   Your file will be saved with the extension .PRT.


 Making a part-program to run your machine is done in five steps:


Setup               Load a setup file.

Geometry         Either import a DXF or create geometry.

Groups             Group geometry to perform operations on.

Operations       Use the operations to make toolpaths

Processing        Translates the partfile into a tapefile G-code



Picking Geometry

Pick Modes

The pick methods are used to select single or multiple geometry items for any command that needs geometry. Almost everything you do, will need to pick something first.


You need to pick geometry to copy, delete, group, edit, trim, rotate, stretch and create geoms based on other geoms.

Picking with a Window

To use a window to pick items, only the items that are ENTIRELY INSIDE of the window will be selected. This means both ends of a line must be enclosed for the line to be picked.

To use a window to select items, first indicate one corner. Any of the four corners of the window can be selected. When asked to indicate the other corner, it must be the diagonally opposed corner. Here, the cursor changes to a WINDOW to indicate the area enclosed.


Exception: When using a window to STRETCH items (via the EDIT MENU) Lines lying entirely inside of the window will be moved.

Picking By Selecting

When picking items with the SELECT method, continue picking single geometry items.  When you have picked all you need, click on the [done] button in the dialog box.



Picking via Chain

Picking with a chain is used when there is contiguous (connected end to end) geometry.  When selecting items via CHAIN, the system will ask you for the first item.  After picking, the system may ask for a "direction".  If the system can chain in more than one direction, the system will ask for a desired direction. This will place a bulls eye at the position where it could last determine. The programmer cannot indicate a direction by digitizing a location in the desired direction. The programmer must pick an item that has an endpoint at the center of the bulls eye.






The system can ask for a direction in any of the following:


There is a fork in the geometry, where three or more items meet at a common point.

A chosen a start point from where the chain could proceed in either of two or more directions.

There is a Z-only line hidden in the current view.

There are two or more identical geometry items that are "on top" of one another.


The chain will be complete under these two conditions:


The chain has returned to the start point.

No more common endpoints can be found.


Select chain is the preferred method for creating a group. The reason to always use the chain to create a group is that it guarantees the group is mathematically correct prior to generating an operation with it.  After entering one chain, the system will ask for another chain. If selected, the new chain will be appended to the first. This can be repeated any number of times.

Pick lasso

The lasso is similar to window except you will create an irregular pick area by digitizing points around the selected items.  Use this when you have to ‘snake’ around geometry you don’t want to include in the picked items.  The start and end points must overlap to close the lasso. Once the lasso is complete, select the icon again to execute the pick. All other Pick Windows terms apply.

Pick last layer

 Pick last layer will select the last layer used that contains information. By clicking on the icon  

 again, it will select the next to the last layer and so on. This makes it easy to delete completed


Select layer

Select layer icon will ask for the layer number to select.



Quick Keys Chart







Arc though 3 positions


Pan or Slide the display


Break two geoms at the intersection


Undo Last Command


Create a Circle


View All the geoms


Fillet on two geoms


View Window


Invert or reverse an Arc


Trim Both


View previous (jump back)


Set Z Depth


Create a Line




Set a temporary Origin


Select an End Point


Create a Point


Select a Mid or Center Point


Query a geom for information


Select an Intersect Point


Redraw or Refresh the screen


Rotates Sprite CCW 5°




Rotates Sprite CW 5°


Speeds Posting Graphic


Rotates Sprite CCW 1°


Slows Posting Graphic


Rotates Sprite CW 1°




Crosshair Cursors


The plus shape indicates an XY or Z must be entered or digitized on the screen.


The X shape indicates that a “pick” of the geometry can be chosen.


The   +s shape indicates that the filter mask is active


Round Cursor [F2]

    The round cursor indicates an ENDPOINT pick mode is enabled.


Box Cursor [F3]


    The box cursor indicates a CENTER-POINT pick mode is enabled.


Intersection CURSOR [F4]

The intersection cursor indicates sequential selections of two geoms whose intersection will be digitized.



Sprite Cursor

The sprite cursor is the actual shape of all the geometry that is digitize when using  the move, copy, rotate, mirror, merge or scale commands.






  After creating geometry, you may have to trim it to a different geom to form a sharp corner. You may have to break it to select a start point for a group.  The most common trim command is [Trim Both].  The quick key for ‘trim both’ is the ‘X’ key



When trimming, the system will look at where you digitize to determine what you want to keep and what gets trimmed off. You will select the geometry to keep. 


When breaking two geometries, it is not that critical where you pick because the all the geometry will remain. When you break two geometries, nothing appears to happen, but you will have four geometries instead of two.




This circle example is often confusing. The circle doesn’t appear to trim on the first trim.



Notice in the two examples on the left. Notice which part of the geometry gets trimmed off and what geometry remains.










Trim Modal

This instruction is used to trim off geometry items where they intersect another item. The system will ask for the trimming item first, then the items to be trimmed  off. Unlike the TRIM BOTH instruction, this one requires that you pick the geometry items along the portion to be trimmed

   off, not the portion to be retained.





In this example, the vertical lines must be trimmed at the horizontal line as shown. Using the TRIM MODAL command, the horizontal line is selected as the trimming item. The vertical lines are selected as the items to be trimmed. They must be picked along their portion that lies below the horizontal line, as that is the portion to be discarded.




  The most common use for breaking a geom is to specify a starting point for a group. Take a simple rectangle for instance.  If you group a rectangle without breaking one of the four lines, the group will start on one of the corners.  This may or may not be what you want.  If you want to sweep onto the shape with a arc, the start and end geometries must form a 180 degree included angle. The easiest way to accomplish this is by breaking a line or circle.  Another common use for breaking a geom is to specify a glue stop for a Wire EDM.

Copying and Rotating

  With the copy command, you must select the items to copy then specify the start point and the end point.  You may think of the start point as the ‘Reference Point or Anchor point’ and the end point as the ‘Destination Point’.  If the start and end points are the same, the system assumes you want to rotate and will display a dialog box to enter degrees. 







Setup File, Tool & Material libraries

The Setup File

  A Setup file allows you to set and save preferences.   Normally you would have a setup file defined for each unique machine tool.  Since the machine (Post-processor) is the most important part,  You may want to ‘save as’ a filename that incorporates the machine and control.  Change it from default.set so it doesn’t get stepped on incase you ever reinstall. 


Use the [Browse] buttons to change the file or the [Clear] button if you don’t want a library file.


Prior to saving a setup file, set the machine mode on the ‘Command Menu’ at the top of the screen.  The mode is located between the ‘Group’ and ‘Operation’ menus.


  Contour mode is the same as 2-axis mode.  If you use a Foam cutter, Waterjet, Plasma, Cutting torch or any two axis, select Contour

Setup File parameter summary

  How you set the system defaults will depend on what you are writing programs for. Below is a list of the key parameters and suggested settings.


Setup File

The setup file being used. 

Post Processor:

The post-processor to be used.

Material Library:

The material library to be loaded (optional)

Tool Library:

The tool library to be loaded (optional)

Inch or Metric:

This is for the post processor output. Most, but not all, posts support metric output. If you are in metric mode and the output is about 25 times to small, metric isn’t supported.  Contact your dealer to have metric output added. If you normally work in inch and receive a metric CAD file, use the [Scale] command to make your geometry inches.

Radius value or

Diameter value

In Lathe mode, it determines whether the X axis values you enter are diameters or radial.

Decimal Display

How many places to the right of the decimal do you want to display on the screen. Most people set this to four. A WEDM user may prefer 5 while a router user may only need 2, This has no effect on accuracy.


Normally this is set to the minimum move of your machine or .001 for a mill or lathe. It will also help with chaining.  This has no effect on accuracy

Toolchange X

Toolchange Y


Auto 1st Toolchange

This serves two purposes. It is used to ensure compatibility with older posts and it makes sure the 1st move squares properly on a 3 axis machine. These values should be set to coordinates off the table.  Check the ‘Auto 1st Toolchange’ and program a simple part. If the coordinates on the first couple moves are correct, leave it checked.  If these coordinates are output at every Toolchange, uncheck it.


First Operation Default

  With each setup file you can and should set the default operation parameters.  This is especially important if you don’t use a tool library.   2-Axis users (foam cutters, water jet, and burning tables) should set the these parameters as you do on all shapes.  That is usually tool ID number and changer set to ‘1’ and the tool width set to ‘0’. Also, set the tool to round and set a federate to something other than ‘0’.












Determining The Tool Side

Determining the tool side is very easy.  Imagine walking along the geometry you wish to cut.  Is the tool to the right or left of that geometry?  In the previous FINISH example, the Tool Side (Left of Geom) performed a Climb Cut.  Though the OUTLINE was defined in the opposite direction, the computer knew on which side and in which direction to cut from the Group Type and the Tool Side.


Cutter Compensation is also a factor.  It can be performed either by computer or machine tool.  In determining the preferred method, consider the following:

 Allow the computer to compensate for all roughing cycles.  Specify the tool side, tool width (and corner radius if any) and set CDC to OFF, which disables the machine compensation.


Allow the computer to compensate for most finishing cycles (Mill and Wire).  Enable CDC on the machine and set the machine compensation to correct for variations due to wear and cutting conditions.  You do not want to double compensate by having Shopcam offset the cutter and the machine do the same.





Cartesian Notation

The Cartesian coordinate system is a method of identifying any point in space. It uses three axis, called X, Y, and Z, to map a grid of cubes. The system identifies the three axis on the screen in the following manner:



X axis;   The X axis is the horizontal axis  Positive X is to the right, negative to the left.

Y axis;   The Y axis is the vertical axis. Positive Y is upward, negative is downward.

Z    The Z axis is perpendicular to the screen. A positive Z is toward you, negative is away.

Zero Degrees

   The 3 o'clock position is always considered to be a zero degree angle.  All angles are reference from 3:00 or 0 degrees. This means that a horizontal line is a zero degree or a 180-degree line, depending upon its direction.

Two Dimensional Angles

A positive angle means a counter-clockwise rotation.  For instance, a line going straight up on the screen is ninety degrees, but one going toward the lower right is a negative angle. All angles are normalized by the system (meaning a 270-degree angle is the same as a -90 degree angle. Angles are entered in decimal degrees. Enter the value as you would any other number to enter decimal degrees (to specify a 22.5-degree angle, enter: 22.5

Units of measurement

Units of measurements refer to the intervals used to measure distances. Normally, coordinates are either in inches or millimeters, however centimeters are also supported.  The part-program is not in any particular unit system. It consists of values that may represent inches or millimeters. In order for the system to generate a tapefile for the NC/CNC machine, it must know what units are to be used. The info table contains a selection for units. It is important that this is properly selected so that a tape can be generated correctly.


Expressions are permitted in any numeric response. These expressions are evaluated immediately and the result is used in the answer. For complex problems, use the CALCULATOR. 

Basic Operations

In expressions, the following operations are permitted:


[+]       Addition                       (e.g.: 2+2 is 4)

[-]        Subtraction                   (e.g.: 5-3 is 2)

[*]        Multiplication    (e.g.: 3*2 is 6)

[/]         Division                        (e.g.: 6/2 is 3)

[^]        Power                          (e.g.: 2^3 is 8)


Notice that the asterisk is used for multiplication. The letter [X] is never used for multiplication on computers because that would cause confusion about a variable [X] and multiplication itself.

The slash [/] indicates division. Be careful not to use the backslash [\] by mistake.



File Types

The following file types are used in Shopcam:



Shopcam part-program that contains a drawing or tool path


The ‘G-code’ text file for the machine control


The post-processor “Post”.  Creates a tap (G-code) file from the part file


Setup file; contains the post, tool & material libraries & default settings


Tool library.  For storing tool information


Material library.  For information about the material being machined


Standard Operation Dialog

  Here is the standard operation dialog used for mill and 2-axis.

Operation Dialog

  There are two ‘Operation Parameters’ dialog boxes, one for lathes and the standard one for all other modes.  Only the information that effects the operation you are working on can be modified.

Standard parameter summary

   Here is a summary of the key parameters.  Each parameter is described in the operation section of the Technical Manual.




Used for the XY step in roughing cycles



From Group

Determines how the Z-axis values are applied. Default will use the ‘R-Plane Z’ and ‘Full Depth Z’ from Z0.0.  From Group will be the incremental distance from the group Z


The plane the Z axis rapids too. Usually .100 or .050

Tool Side

Which side to keep the cutter on.


Cutter diameter compensation; Usually causes a G41/G42 in the tape file


CDC Register; Most posts use the tool number if set to 0.

Cap Radii

How the system treats sharp corners. Usually set to ‘Roll’.

Drill Cycle #

For canned drilling cycles; cycle 1 is system generated

Path Angle

To change the path angle on Zig Zag rough.

%Step Dev.

Allow the step to deviate to equalize passes

Max Cusp

Adjusts the resolution of the steps of 3D operations


If a material library is loaded, will figure RPM & feeds

From Tools

Loads the feeds and RPM from the tool library

From User

Allows you to set your own RPM & Feeds






Standard Lathe parameter summary

   Here is a summary of the key turning parameters.  Each parameter is described in the operation section of the Technical Manual.  Each operation will gray out the boxes it does not need.  A generic picture will show how the most important parameters will be used.





Used for the XZ step in profile cycles

Extra  Stock

Additional stock to leave on straight OD cuts


Where the Z axis positions for a pass; Absolute value.

Tool Side

Side to keep the cutter on.  Usually right for OD left for ID


Not usually used on a lathe

Path Angle

The ‘rough Turn’ path angle usually=0 or 90 for facing.

%Step Dev.

Allow the step to deviate to equalize passes


If a material library is loaded, will figure RPM & feed

From Tools

Loads the feed and RPM from the tool library

From User

Allows you to set your own RPM & Feed