Incredible problem with the post process Mazak and Other

[usivar83]

Good morning all !

I allow myself to ask for your help because I find myself in a really complicated situation in production.

When I do my MILL TURN program, which I used to do, the movements are completely incoherent.

 

 

I let you look at the photos and give me your opinion ...
This occurs on all operations, pocket, contour, bore.

I specify that the part is not the one to manufacture but I created this small file in order to simplify the visibility.

Thank you in advance for your help. I have no idea why, while I had no problems before I find myself stuck at this point.

Good weekend to all.

[Anonymous]

I can't quite make out what square in second picture represents, are you trying to mill a pocket at part center ?

Can you upload the Fusion file ?, pictures are not very helpful.

[usivar83]

Hello and thank you for your return,

The square of the photo is precisely the problem it will have to resume the path tools viewed from the front and suddenly be perfectly round.

I voluntarily delete the lead in and lead out so that the visual is clearer.

On the second drawing (left side of the photo of my QTN 250 MY Mazak) we can see displacements on the Z axis which should not be done, the tools should simply return, bypassed in order to carry out the cylinder and come out straight.

There is a real disagreement with what fusion simulates me (which seems perfect) and the code it generates for me.

It's quite surprising because I never had this problem. Since I got the right post pro (thanks to you for that matter) everything is going perfectly, I have made very complex pieces easily.

Only, I probably made a mistake somewhere, and since then nothing is going right! However, I perfectly pilot my milling machining center ...

I do not have access to my file from home, but it is a Ø15 diameter pocket of the most standard, created only to simplify the visibility of the problem.

Thank you very much for your quick return, it's great!

[Anonymous]

Apparently there are two parts of getting something right, making Fusion tool paths and having post processor properly interpret them for particular machine in question. 

I don't recall when or how I helped you in the past as you are suggesting but my aim was to inspire you to upload actual Fusion file as pictures are far from being any source of usable material in detecting problems.

It seems though that your issue is with post processor and I am not the guy to talk to on that subject.

I did edit two posts I use daily with some editing of resulting G-code still being part of the deal but I am not familiar with Mazak religion beyond running some production work long time ago.

[billcainautodesk]

Hello usivar83

Which Post Processor are you using? and can you upload the .f3d files?

Are you using Polar or just XY?

Thanks

Bill Cain

[usivar83]

Hello,

Thank you for your help, here is the post processor used.

The second, does not work on my machine because it tells me that "options are not available". Yet I have exactly this machine. I will have to analyze the code to find the problem.

https://cam.autodesk.com/hsmposts?p=mazak_quickturn&_ga=2.119963592.1390310283.1594395091-785401708....

https://cam.autodesk.com/posts/post.php?name=mazak%20quick%20turn%20250-my

I do not have access to the file from home but I have reproduced something similar here.

 
What you see on the first photo of my machine screen and the result of a post process identical to this file.

It's really surprising, we can see on the left, completely crazy Z-shaped displacements and also a square instead of a circle on the XY plane.
It would seem however that the code generated from my home computer is much simpler. I will try it on Monday!

Thank you again for your help!

I will get back to you with the files at that time.

Thank you again for your responsiveness!

[Anonymous]

Actually, I am not in total dark on this one, I downloaded post you are using and came to realize it is not outputting polar mode.

Because I live in inch world, I changed units. In user parameters of post I switched to IJK for arcs and turned C axis optimizing on.

Without changing anything else in your Fusion file, I added manual NC command to force polar mode output.

Next, I divided X coordinates by 2 and changed C address to Y, doing so converts code to vertical mill format and when plotted there is correct circular output as you can see in screenshot.

I opened the post in Notepad++ and took a look at list of M and G codes, it seems that outputted G-code

activates C axis (M200), but I don't see it being deactivated at the end (M202)

Without being familiar with machine in question, it looks as if concept is same as on any other mill-turn I ran before.

It looks like post needs some refinement but that part is beyond my current "expertise".

[usivar83]

Hello,

Thanks again for your response.

Only the call of a polar interpolation creates an error.

- 936 Option not found

While I am sure that my machine is capable because it has already realized it before.

In order to reduce the number of tests to be carried out, already more than a hundred I think. Which of the two post pros would you advise me to use?

I find myself in a real pain. Machine stopped and impossible to produce. Surely because of a small detail ...

Thanks again for trying to help me

[Anonymous]

I only tried posting with first post you listed in your earlier post, mainly to see what the result would be and just pointed out that post in missing few things.

From practical point of view, there was nothing wrong with tool path, I am sure you have some documentation with your machine, including sample of basic functions in programming features machine is capable of.

You'll need G and M codes in order presented below, I have a hunch as to what they are but I don't have actual manual for your machine,  if you wanna  get things going, edit your tool path as shown.

So , you .....

call tool and offset

stop main spindle (M5)

engage C axis (M?)

zero reference C axis (G28 H0)

turn rotary tool on (M?)

rapid in position in front of the part

start polar mode (G12.1 or G112)

perform cutting

rapid away from part

cancel polar mode (G13.1 or G113)

stop rotary tool (M?)

disengage C axis (M?)

return to indexing position

M1

[billcainautodesk]

Hello usivar83

The first post you linked to we have deprecated so you should not use that one as it never had been out of beta testing. The second post was one we developed and tested with Mazak AE's so it would be the better choice.

I ran the code through a back plotter from both of the posts. The old post did not look correct while the newer post looked much better and looked like what the tool path looked like in Fusion.

Give the newer post a go and let us know how it works out. If there are any problems we can work through them.

[usivar83]

Hello,

Ok thank you very much, only when I use the official pro post, I end up with a G12.1 code and my machine tells me that this option is not available.

While, these are parts in tool paths that posed no problem to me!

Do you have a solution?
Can be done without polar interpolation?
Thank you !

[Anonymous]

It is highly unlikely that modern mill-turn having Y axis does not support polar mode, I have never encountered machine that had only C axis but did not support polar mode and I started  long time ago.

It could be matter of turning on parameter in software of control, in shop I work for, Fanuc tech had to come out to activate helical milling option on new Hyundai Wia mill-turn with Y axis, having Y axis also includes all options for C axis.

There was some chatter on this forum about doing face milling without polar mode, I am very skeptical of that idea because all machines I ever worked on had limited tool travel below center line and polar mode is there to rotate spindle so that tool always works on positive side of X axis.

I never heard back from you regarding list of G and M codes in machine's user manual, first place to look for clues.

[usivar83]

Indeed, I just had mazak and they confirmed to me that the option was present on the machine.

I do not understand why therefore, the machine gives me an error when the code appears "G12.1" I checked in the manual book and the codes from the post pro are all good.

I am relaunching a test series that the machine is available (currently in production)

I do not despair of finding the solution and I thank you very much for your support!

[billcainautodesk]

Hello usivar83

Error 939 looks to cover a few things so maybe it's not the G12.1 kicking it.

Can you provide the code your tested that gave the error?

Have you ever run ode with G12.1 before on this machine? If so can you provide the code that ran?

Thanks

Bill Cain

[Anonymous]

I haven't asked before, but ... are G12.1 / G13.1 on single blocks or in same block with another codes,......... each needs to be on single block, by itself.

Also, have you tried G112 / G113 instead?, it's a same thing but some controls don't like decimal point.