Machine Define

A machine file (SMF file) contains a series of answers to questions about your machine tool. It contains information needed during code generation about topics such as number formatting, block numbering information, axis definitions, G and M code words for many standard functions, cycle time information, canned cycle format information, and much more.

A machine file is in effect even before processing a G-Code file. SmartCAM's modeling of toolpath via Verification utilizes the data from the machine file to simulate the specific machine tool characteristics. SmartCAM will use a default set of parameters if a machine file is not loaded at the time, so it is NOT a requirement until code time. This allows one model to represent many machine tools, by simply switching machine files.

Machine Files are created and maintained using SmartCAM Machine Define. Machine Define is a stand-alone program that manages the machine file data and allows the user to edit settings.


Machine Define is installed with SmartCAM and is found in the SmartCAM program group. Machine Define offers two different types of views of the questions. An Item List is the numerically sorted list of all the questions that pertain to your machine type. The Category List is numerically sorted and divided into user defined categories.

SMF files are classed by machine type, but Machine Define will read any and tailor itself to the type of machine the SMF file is for.

See Machine Define's online help for more information about using this utility.



Try it

Create the following simple toolpath model to see how the Machine File affects code output. This exercise is based on an inch model in the milling applications but can easily be adapted for any of the product families.

  1. Start your SmartCAM application and File - Open gsmill.pm5, found in your MDATA directory.
  2. Select Process - Planner, then select Job Info and select the Machine tab. Select the SMF and CGT files here.
  3. In the MACHINE directory, select lsmill.smf and lsmill.cgt. These are installed with your application in the SmartCAM data directory. Accept.
  4. Then Close the Planner.
  5. Process - Code and the label at the top should already display your machine (SMF and CGT). Enter a Code File name and Create Code.
  6. Use a text editor to examine the G-Code file. The first few lines should look like this: 
     G00 G40 G80 G90
 T2
 M03 S382
 X1.208 Y2.872

  7. Use Machine Define found in your SmartCAM Program Group to open the lsmill.SMF machine file.
  8. Select Select Categories and pick Formats, Units, Tolerances from the list. This narrows the displayed list of questions to just those that deal with these items.
  9. Scroll to question number 64 and set this to F2.0. Save the SMF.
  10. In the SmartCAM application select Code the model again and overwrite the first G-Code file. Then open the new G-Code file for examination. 
     G00 G40 G80 G90
 T02
 M03 S382
 X1.208 Y2.872

Note the tool number is now T02 (see the following section for more about these formats). In the Machine Define application you can set the View to Item List in order to see all questions that pertain to your machine tool. Note that each question you select offers an explanation about itself in the lower window. In many cases it also offers a suggested value that matches most machine requirements. Any edits to the Machine File immediately affect the code output. This simplifies the creation or debugging your Code Generators.

The following sections on this page cover topics that users often find confusing.

Numeric Formatting

Select View - Select Categories - Formats, Units, Tolerances and Machine Define will present a list of several questions about numeric formats.

Here are examples of possibilities. All of the examples use the value: 10.625

D3.4 = 10.625
T3.4 = 106250
L3.4 = 010625
F3.4 = 0106250
P3.4 = 10.6250
E3.4 = 010.6250

Note: for a more detailed explanation of Numeric Formatting, please see the About Numeric Formats Learning SmartCAM topic.

Canned Cycles

Questions 150 through 203 deal with outputting canned machine cycles, if desired. If your machine has the capability to use canned drill cycles, threading cycles or other similar cycles these should be used. They create smaller code files and are easier to read than individual moves.

Canned cycle code is output through @OP_(cycle) sections. See CGT Section Examples for examples of these sections.

Code Filtering for Mesh Polylines

Code filtering can significantly reduce the amount of G01 code output from mesh toolpath polylines to the machine tool. To initiate code filtering, set SMF question 86 to <1> and identify the deviation tolerance with question 87.

This establishes a tolerance bandwidth that controls when a point is output for a polyline.