Posting

Introduction

This topic will explain the Posting page of the CAM Defaults Current Settings dialog, will explain how to access it, the options found in it, and will provide a link to a related topic.

Posting

The Posting page of the CAM Defaults Current Settings dialog box allows you to set the post settings for the machine selected on the Machine Parameters page. These post settings will be used when that machine is selected for a job unless otherwise specified in the Job Current Settings. Although this topic is grouped to model the Posting page of Milling machines, options for each machine can be found here.

To access the Posting page: 

 

  • In the CAM Tree Manager, right click CAM Defaults and select Current Settings.

    The Current Settings dialog appears.

  • In the tree on the left, select Posting.

Parameters

Post Processor

  • Select - displays the Open dialog box for you to locate and select a post processor to use for the selected machine.

 

 

NC File Path

  • Select - displays the Browse For Folder dialog box for you to locate or create a folder in which the posted NC program is stored.

  • NC File Extension - allows you to specify a file extension that is automatically added to the NC program file.

 

Important: By setting the NC File Extension value to APT, you can output the cutter location data rather than an NC file.

 

Program

  • Number - is the program number as it appears in the posted NC program.

 

 

Absolute/Incremental

  • Post Setting - uses the post processor settings to define absolute or incremental posting values.

  • Absolute - uses absolute values only for posting.

  • Incremental - uses incremental values only for posting.

 

 

Sequence Numbers

  • Start Number - designates the starting line number for events in the NC program if the machine is configured to output them.

  • Sequence # Increment - sets the number added to each subsequent line number for the next line.

 

 

Subprogram Numbers

  • Output Subprograms
    Select the check box to generate repetitive subprograms in the posted NC program, if the post processor is set up to do so.
    Clear the check box when not generating subprograms.

  • Subprogram for Operation
    Select the check box to generate repetitive subprograms for individual operations, if the post processor is set up to do so.
    Clear the check box when not generating subprograms.

 

The following two options are only available when the Output Subprograms check box is selected.

  • Subprogram Start # - sets the first subprogram number used in the NC program.

  • Subprogram # Increment - if more than one subprogram is generated, this value sets the number added to the previous subprogram number for the next.

 

 

Use Transform Planes

- With this option selected, the associated machine will, by default, output a Fanuc G68.2, or the equivalent of that code for index systems.

- With this option cleared, the associated machine will not, by default, output a Fanuc G68.2, or the equivalent of that code for index systems.

 

  • Use Index System Origin
    - With this option selected, the coordinates will be output from the index system origin.
    - With this option cleared, the coordinates will be output from the original location of the machine setup.

 

Machine Rapids Handling

  • Machine Does Dogleg Rapid Move - This option is for handling controllers that create dogleg rapids when moving more than one linear axis.

    - With this option selected, any rapid moves that are defined with more than one axis at a time (X,Y, and Z only) will be automatically converted to sloth-leg feed moves. The speed of these feed moves will be determined by the value used for the Maximum Cutting Feedrate listed in the Machine Parameters group of the Machine Parameters page in the Current Settings dialog.
    - With this options cleared, rapids will remain rapids, regardless of the number of axes utilized for the move.

 

 

Output Arcs in 4-Axis NC Program

Note: This option is only available when a mill machine is selected in Machine Parameters.

 

  • GCode 4 Axis Arcs OK

Select the check box to output arcs in the NC program for 4-axis machining.

Clear the check box to output only points and line segments in the NC program for 4-axis machining.

 

 

Lathe Toolpath Output

Note: This option is only available when a lathe machine is selected in Machine Parameters.

 

  • Theoretical Point - calculates the toolpath from the theoretical point of the tool (the intersection of two tangent lines extending from the extents of the cutting area of the tool).

  • Cutting Arc Center - calculates the toolpath from the arc center of the tool (inside the extents of the cutting portion of the tool by the size of the tool nose radius).

 

 

Output Automatic Comments

  • Output Automatic Comments

Select the check box to allow the automatic comments from the post to be output.

Clear the check box to not allow the automatic comments from the post to be output.

 

Next Topics

CAM Defaults Multiaxis Posting