Create Post Processor warning dialog for a particular toolpath

[iamcdn79]

There are times when I forget to set cutter comp. to LEFT in the NC Program settings when post processing for Corner Pencil toolpaths. I want to create a warning dialog to say something like cutter comp is not set for this toolpath.

I am wondering if it is possible and how.

I am thinking of creating an if statement like if the toolpath Corner pencil exists and if Cutter Comp is set to None then to pop up a warning when posting.

[evo80]

Ok, Figured it out.

[Jonathan.Artiss-DSI]

You call me, and I do it for you 😉 

Build a trap to filter the unwanted behavior, create a new user command, and at it to your trap, set the user command to Dissalow, this will cause the post to stop writing and throw a message. You can also set a custom message to the properties of the user command to display in the post information window. 

[evo80]

I'm trying to use the same for thread milling, but this fails every time.

I've tried all manner of different subtype names but nothing seems to fire.

[Jonathan.Artiss-DSI]

Your subtype is wrong. Use this - %p(Toolpath Strategy Subtype)%=="Thread_Mill"

[iamcdn79]

Are you getting all the subtype commands from the Powermill help parameters documentation? 

[evo80]

Wow, I'm sure I tried that configuration, anyhow I copied and pasted yours and it works, I must've been missing something. So Thanks for that!

Regards

[Jonathan.Artiss-DSI]

It's case-sensitive, and you had some training words that would also cause it to fail. 

[Sean571]

I get the sub type from debug view in the post 

[evo80]

@Sean571 

Hi Sean, How is this implemented into the Post Processor?

[iamcdn79]

I love the "Process as Debug" feature, it helps a lot. I never knew about the Debug View though.

[evo80]

I Agree!

That is proper handy.

[evo80]

Is this the correct syntax to check if an incorrect tool radius has been entered into the Tool Radius Comp Value?

[evo80]

 I also tried this, but doesn't seem to work either.

The disabled code does work, but i'd really like to check that the correct tool radius has been entered.

[evo80]

 I couldn't get the Tool Radius check to work so I decided on another route and have the post fill in the tool radius for the helical and threadmilling canned cycles at the tool load stage.

[Jonathan.Artiss-DSI]

I'm unsure of what you're trying to test for, but if you have it working, then it's correct 😉 

[Jonathan.Artiss-DSI]

I think I see what you're testing now. This is how I went about doing it. 

Do your math inside a user parameter, then test it in your logic. 

[evo80]

Ah, I see how you've done it. But anyhow by having the post automatically fill in the tool radius I don't need the check.

Still, learned a lot about checking conditions so thanks to all concerned.

Best Regards Jon K

[iamcdn79]

@Sean571 or @Jonathan.Artiss-DSI do you know what the if statement would be to check if the drilling canned cycle is turned on? I want to add that to my if toolpath strategy subtype = helical statement.

I tried looking in the option settings in the debug view but couldn't find anything drilling cycle or canned cycle

[Jonathan.Artiss-DSI · Accepted solution]

@iamcdn79 

You're looking for "Drilling Expanded Cycle Mode" On and Off are the checks. 

[iamcdn79]

I tried using that but in the debugger it is showing it as off when clicking on the first cycle def  when it should be on for a toolpath that was posted with drilling cycle output set to on