My Post processor generates abberrant moves not in simulation

[CEStanley]

Hi anyone,

I am getting my post processor under control. It presently generates aberrant moves that DO NOT show up in the simulation. Very frustrating as I am continually modifying my nc files to generate the correct code for my Grizzly Mini Mill which has been CNC'd for a while.

Any Idea how to get BobCAD to "See" the aberrant moves?

This morning I had one that moved the Y axis off the part by 3.75 inches and the table was not 3.5 inches larger than the part 0,0,0.

Thanks in advance,
CES

Similar Threads:

• Need Help!- Post processor for Fanuc Oi mate -TD post processor for lathe for NX or Edgecam
• Haas VF4 Rapid Moves vs. CAMWorks Rapid Moves and Post Processor Issues
• I need :Post Processor DMU-60T-MonoBlock and Machine Simulation DMU60_NEW
• post generates an F at the beginning of every program

[BurrMan]

Hi anyone,

I am getting my post processor under control. It presently generates aberrant moves that DO NOT show up in the simulation. Very frustrating as I am continually modifying my nc files to generate the correct code for my Grizzly Mini Mill which has been CNC'd for a while.

Any Idea how to get BobCAD to "See" the aberrant moves?

This morning I had one that moved the Y axis off the part by 3.75 inches and the table was not 3.5 inches larger than the part 0,0,0.

Thanks in advance,
CES

Your best bet will be to get a bbcd file that generates the moves you dont want and zip it, along with your post processor and attach it here.

Also, let us know which machine file is selected. If you have tried to customize or generate your own machine file, we "may" need that too, but may not.

Your post processor can be set in "debug mode_on" which will output WHERE in the post processor that any particular code is coming from... that can help you. Just search your post for debug to find the line to change the variable on and off.

[jrmach]

" my Grizzly Mini Mill which has been CNC'd for a while."

Does that mean you have set your machine up with a no-name system that did not come with your machine ?A Frankenstein ?

More details of your set-up please

[CEStanley]

" my Grizzly Mini Mill which has been CNC'd for a while."

Does that mean you have set your machine up with a no-name system that did not come with your machine ?A Frankenstein ?

More details of your set-up please

Hi jrmach,

G540 24V 3.1Nm motors on all axis connected to 5 to 1 ball screw controlled using Mach3 licensed. Motor movement is 1.8 degrees per step. Table is 15(X) 4.3(Y) and 9 to 2(Z) (depending on tool holder).

BobCADCAM is licensed V29. Design is done in Solidworks 2017 also licensed.

[CEStanley]

Hello BurrMan,

Sorry, it's 2AM and this website is not allowing me to upload my post or nc file.

Frustrated at this point and I can't give more information. Maybe the site will allow upload later or maybe my head will be clearer after a good nights sleep.

[CEStanley]

Well, can't sleep.
I was able to zip my files and attach them to this reply so my .nc file and my .pst file are attached. I took a picture of the Mach3 screen showing the two moves in question. They are off the part to the bottom of the picture by a lot and make no sense why they might be in the nc file.

[CEStanley]

I have located one of the aberrant moves generated by BobCADCAM V29 but not shown in the simulation of the part.
The moves, one to go way off part and one to move the head back to the part. Oops, the files "are too large to process".

Line 5 sends Y to -0.375 then line 10 brings Y back to -0.75 but Mach takes the head to -3.75 Then back to the part but I have crashed at that point. My table has been exceeded.

Oh, I just found the issue. Line 5 contains a G53 and can't. it is not valid to move my table to any positive value. X is only valid in minus, Y is only valid in minus and Z is only valid in minus.

Thanks everyone. Back to the post files...

[The Engine Guy]

CES

A very quick look at your code seems to indicate you have a G53 (Times 2) in your code where I would expect there should be a G54/55/56/57/58/59, that G53 will likely send your machine to the position set in the X and Y axis as shown on that line from your Home position, example on line N05 you have :-

N05 G00 G90 G53 X0.4661 Y0.375
I would have expected this line to be as :-
N05 G00 G90 G54 X0.4661 Y0.375
This would move the machine to the correct position for the start of the cutting moves and the X and Y positions would be whatever offset you used for the lead-in.

You also have the same in line N1542 :-
N1542 G90 G53 X2.0891 Y0.375
Again I would have expected there to be a G54 in there as :-
N1542 G90 G54 X2.0891 Y0.375

Looking at your Post Processor you have Block 900 set as :-

900. Work shift #1? "G53"
which is why it is generating the G53 for the Work Coordinate :-

When it should show as :-
900. Work shift #1? "G54"


That`s all I have time for at the moment, give that a try and see what happens

Usual Caveat applies, at your own risk and also make a copy of your PP before making any changes

Regards
Rob

:rainfro: :rainfro: :rainfro: :rainfro: :rainfro:

[BurrMan]

I have located one of the aberrant moves generated by BobCADCAM V29 but not shown in the simulation of the part.
The moves, one to go way off part and one to move the head back to the part. Oops, the files "are too large to process".

Line 5 sends Y to -0.375 then line 10 brings Y back to -0.75 but Mach takes the head to -3.75 Then back to the part but I have crashed at that point. My table has been exceeded.

Oh, I just found the issue. Line 5 contains a G53 and can't. it is not valid to move my table to any positive value. X is only valid in minus, Y is only valid in minus and Z is only valid in minus.

Thanks everyone. Back to the post files...

No bbcd file to check the setup. Be sure to place the stock origin correctly for your negative value outputs. The stock origin will affect the post processor's output also.

don't need nc files, as a bbcd file and the post processor will get us the same output. (Well, unless the machine file is configured differently)

Anyway, if you need to look at this further, zipping the bbcd file to go with the other attachments will help.