Generate NC Code in Batch Mode

task target This task shows you how to generate NC code from the manufacturing program or part operation in batch mode.
 Post Processors are provided by Cenit, Intelligent Manufacturing Software (IMS), and ICAM Technologies Corporation.

For information about how to acquire Post Processor parameters files that provide machine specific NC code output, please contact your IBM representative. 

Select the type of Post Processor solution using Tools > Options > Machining > Output tab. If the output option is set to None, you will not be able to generate NC code.

Cenit Post-Processor Solution

Sample  Cenit Post Processor parameter files are delivered with the product in the folder
\Startup\Manufacturing\PPPar
which provides NC output for various machine types. To execute your own PP you must copy it into this folder.

You can use PPs that include external macros. In this case, you should define them in the PP in:

Modify postprocessor // Define NC-blocks // Index : MACRO APT WORDS

and then copy these macros in the same folder as the PP. 

IMS Post-Processor Solution

Sample IMS Post Processor parameter files are delivered with the product in the folder
\Startup\Manufacturing\IMSPar
which provides NC output for various machine types. To execute your own PP you must copy it into this folder.

The IMSPar folder must be accessible in Read/Write mode.

Note: The IMS PP solution is not available when working on a Windows XP 64-bits machine.

ICAM Post-Processor Solution

Sample  ICAM Post Processor parameter files are delivered with the product in the folder
\Startup\Manufacturing\ICAMPar
which provides NC output for various machine types. To execute your own PP you must copy it into this folder.

Always save your program modifications before generating NC code.

For best results, you should first verify the operations of your program by means of a replay or simulation. There should be no operations to be updated or in an undefined state.
scenario 1. Select Generate NC Code in Batch Mode . The following dialog box appears.
 

In the In/Out tab page...
2. Select the manufacturing document to be processed using the Input CATProcess [...] button. The current document is proposed by default.

Select the type of NC entity to be processed. This can be:

  • one part operation in the input CATProcess. In this case all the manufacturing programs of the selected part operation will be processed.
  • one or more manufacturing programs in the input CATProcess.
3. Select NC Code as the NC data type that you want to generate.
  4. Select the desired One file... option to generate a single NC code file:
  • for all the selected manufacturing programs
  • for each selected manufacturing program
  • or for each machining operation in the selected manufacturing programs.
    Please note that this option is not supported in programs containing Copy or Tracut Operators.
5. To store the resulting NC data file at the same location as the input CATProcess, select the Store at same location as the CATProcess check box.

Otherwise, specify the Output file where you want the NC data to be written using the [...] button.

A default name is proposed for the output file (for example,
Process1_Manufacturing_Program_1.CATNCCode). This name can be modified directly in the Output File text field.

On subsequent batch executions, the filename and the path of the last generated output are remembered if the Store at same location as the CATProcess check box is not selected. If this option is selected, only the filename of last generated output is remembered.
6. Select the Replace like-named file check box if you want to authorize overwriting an existing like-named NC code file.
7. If needed, you can choose to write the CATProcess document after processing. Select the Save Input CATProcess check box and specify where you want to save it using the [...] button.
  8. Select the Replace like-named CATProcess check box if you want to authorize overwriting an existing like-named CATProcess document.
9. You can attach the generated output file to the first selected manufacturing program by selecting the Associate output NC file to the program check box.

The output file can be accessed by right-clicking the manufacturing program and selecting Display NC File.

See Manufacturing Program with Associated NC File for additional information.
  10. You can select the Lock operations check box to lock all the machining operations after processing. Please refer to Locked Machining Operations for more information.
 

In the Tool Motions and Formatting tab pages...
  Certain option settings may have an influence on the generated NC code. Please refer to NC Data Options for more information.
 

In the NC Code tab page...
11. Use the list to select the desired Post Processor parameters file.
12. Click Execute to request computation of the NC code.

end of task