Posting APT Code
Introduction
This topic will explain how to post APT programs, how to save and edit code, and provide links to related topics.
How to set programs to post as APT
Before posting the program, you must first update your current settings in order to have the program post cutter location data rather than NC code.
Set a particular machine to output APT code as default:
-
In the CAM Tree, right-click CAM Defaults and select Current Settings.
The Current Settings dialog appears. -
In the Machine group of the Machine Parameters page, select the machine which should post APT code by default.
-
In the tree on the left, select Posting.
The Posting page opens. -
Set the NC File Path to the location the files should be saved to by default.
-
Set the NC File Extension value to .APT.
APT code will now be output when the program is posted.
Set a particular program to output APT code:
-
In the CAM Tree, right-click the job name (for example, Milling Job), and click Current Settings.
The Current Settings dialog appears. -
In the tree on the left, select Posting.
The Posting page opens. -
Set the NC File Path to the location the files should be saved to by default.
-
Set the NC File Extension value to .APT.
APT code will now be output when the program is posted.
APT Output Options
Optional parameters for controlling the APT output can be found in the BobCAD-Posting.xml file in the C:\BobCAD-CAM Data\*Current Version*\System Files\Posting folder.
-
IsSupportCannedCycle - boolean value of whether to output drilling cycles using the canned cycle format or long hand code
-
IsOutputCutterFirst - boolean value which determines the order in which to output the LOADTL or CUTTER command first in the APT output
-
IsBreakArc - boolean value to determine if all arcs should be converted to line segments using the ArcBreakTol value.
-
IsBreak3DArc - boolean value to determine all 3D arcs should be converted to line segments using the ArcBreakTol value.
-
The definition of a "3D Arc" is any arc that does NOT lie directly on the G17 / G18 / G19 plane with the tool orientation pointing perpendicular to the three main planes.
-
NOTE: At this time the tool vector will come from the end point of the arc and will be consistent along the entire arc.
-
-
ArcBreakTol - double value representing the chordal tolerance used for breaking the arc into line segments.
-
If this value is excluded a default of 0.0005 inches (0.0127 mm) will be used in the case of breaking arcs.
-
Note: Learn how to output APT using Lua here.
How to Post APT Programs
To post the code for every toolpath that has been computed and has not been set to Post No:
- In the CAM Tree, right-click the job name (for example, Milling Job), and click Post or click Post & Save As.
The posted APT code is displayed in the Posting Manager.
Note: You can also post the code for particular portions of the program by right-clicking that item and selecting Post.
Tip: After code is posted in the Posting Manager, you can click inside the Posting Manger to give it focus, and then use Ctrl+F to use the Find dialog. This allows you to search for particular codes/terms without the need to open the posted code in an editor.
The Posting Manager Shortcut Menu - How to Save and Edit Code
After posting a program, right-click anywhere in the Posting tab to display a shortcut menu with the following items. Use these options to save or edit the code that displays in the Posting Manager.
- Save As - opens the Save As dialog box for you to select a location, name, and save the code as an .apt file.
Note: The cutter location data (.apt) file is a text file that can be edited with any text editor. When you post a program, the file is automatically saved to the default location for .apt files: C:\BobCAD-CAM Data\*(Current Version)*\NC\...
- Predator Editor - opens the Predator CNC Editor with the posted code. Editing, back-plotting, and other actions can be performed with the editor.
- NC Editor - opens the NC Editor with the posted code. Editing, back-plotting, and other actions can be performed with the editor.
- Mach 3 - if you have purchased Mach 3, you can open the code in the Mach 3 software.
Note: BobCAM switched to the NC Editor for the Editor which comes standard with the software. The Predator Editor option was left as an option for users which previously owned, and still used Predator Editor. Please note that back-plotting the code in the editors require an upgraded license of the editor.
Related Topics
Machining (Posting) Order Dialog Box
Getting to Know the User Interface