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.

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.

Post Output

  • Type - determines the post output type as either G code or Command ISO format. Select the proper type for your machine. Most machines use the G code output, but some machine types, such as Agie, support the Command/ISO output format.

    • Post Info File - displays the Open dialog box for you to locate and select a post processor information file that is machine specific. This option only displays when Command ISO is selected as the Post Output Type.

  • Output Cutting Conditions - for EDM machines

Select the check box to allow the Cutting Conditions to be output.

Clear the check box to not allow Cutting Conditions to be output.

 

  • Output Cuts to Separate Files - for EDM machines

Select the check box to output each operation to a separate file. This must be configured in the post processor.

Clear the check box to output the entire program in one file.

 

  • Output File Breaks - for EDM machines

Select the check box to output markers in NC program that can be used to modify or reformat the code after it is post processed. When enabled, post block 75 is called to output new file header code in the NC program. This post block requires the post processor to be customized to function properly.

Clear the check box to output the NC program without file breaks.

 

  • Output Guide Positions - for EDM machines

Select the check box to output the guide positions of the program.

Clear the check box to not output guide positions.

Cutting Parameters

The Cutting Parameters only display when Sodick AQ325 or AQ537 machines are selected.

 

  • Cut Type - select from one of the available options to set the cut type.
  • Fluid Type - select from one of the available options to set the Fluid type.
  • Flushing Conditions - are usually applied for non-submerged machining and the options are based on the taper angle between the upper guide and lower guide. Good Flushing is used for parts with little to no taper. Medium Flushing is used for parts with around 10 to 18 degrees of taper. Poor Flushing is used for parts with greater than 18 degrees of taper.

Next Topics

CAM Defaults Multiaxis Posting