Post Processing Error for tormach pcnc1100

[astover]

Warning: work offset has not  been specified using g54 as wcs.

Can anyone tell me why I continue to get this error.  I have a .25 plate to square up on end, drill and tap both sides.  Fairly simple.  

[Steinwerks]

Because in your Setup under the Post Processing tab you have left the Work Offset as zero. Zero defaults to 1. 2 = G55, 3 = G56, and so forth.

[Steinwerks]

A thought occurs: this will not keep the code from generating. Are you still getting a usable program or is it failing? If the latter, could you share the entire text of the log file?

[astover]

Information: Configuration: Generic Tormach PathPilot
Information: Vendor: Tormach
Information: Posting intermediate data to 'C:\Users\astover\AppData\Local\Fusion 360 CAM\nc\1001.TAP'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Code page changed to '1252 (ANSI - Latin I)'
Start time: Thursday, November 24, 2016 2:32:48 AM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41239
Configuration path: C:\Users\astover\AppData\Local\Autodesk\webdeploy\production\e94a84f42d31c56d0b570e5907b7d11677a71a5d\Applications\CAM360\Data\Posts\tormach.cps
Include paths: C:\Users\astover\AppData\Local\Autodesk\webdeploy\production\e94a84f42d31c56d0b570e5907b7d11677a71a5d\Applications\CAM360\Data\Posts
Configuration modification date: Tuesday, July 26, 2016 9:35:13 PM
Output path: C:\Users\astover\AppData\Local\Fusion 360 CAM\nc\1001.TAP
Checksum of intermediate NC data: 51f9898b21bb21910a377429f161ea9a
Checksum of configuration: b1c715ea143981993244579c12ab26b0
Vendor url: http://www.tormach.com
Legal: Copyright (C) 2012-2016 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2539
...
Warning: Work offset has not been specified. Using G54 as WCS.
Error: The depth is invalid.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to execute configuration.
Stop time: Thursday, November 24, 2016 2:32:48 AM
Post processing failed.

[daniel_lyall]

@Steinwerks It should still post's useable code, it just defaults to machine and work zero. these hobby programs are a bit loose.

[astover]

you were right, but when I entered 2, because i have two sides, it didn't change anything. Why?

[Steinwerks]

"The depth is invalid" is what is causing the post processing to fail. I would suggest going to File->Export and saving the file as a .F3D file and attaching it here. I suspect that one of the heights definitions in one of the toolpaths is awry and mucking things up for you.

[astover]

I've checked several times, I'm just stumped. Thanks for the help.
Andy Stover
Jackson High School
573-243-9517

[astover]

I've checked several times, I'm just stumped. Thanks for the help.
Andy Stover
Jackson High School
573-243-9517

[LibertyMachine]

If you attach your .f3d as @Steinwerks suggests, we can set you in the right direction

[astover]

here is the file. thanks

[LibertyMachine · Accepted solution]

The heights on #2 centerdrill were wrong. You had Top Height set to Top of Hole. That was fine. Your Bottom Height was set to Stock Top, with a negative offset of .03125. Setting it to Hole Top and leaving the negative value alone allowed it to post out.

[astover]

That worked, made sense too.  Thanks for the help.