MAHO 432 post processor

[AchimN]

We have released a post processor for MAHO machines using Philips 432 control and would be happy to get some feedback from the community.

Please feel free to download and test it:

http://cam.autodesk.com/posts/?p=maho_philips_432

[Barbatoss]

Hi Achim!

I tested the post yesterday and have recognised these issues so far:

1) The control requires the following beginning of the programm

N1 %PM

N2 N9001

It stops transferring data to the machine by error on the original PP code

2) It seems like the comments for tools and the program are created regardless of the choosen option in the PP?

The control does not support displaying comments

3) Radius correction seems to work fine now but the PP creates the G41/G42 command one line too late so that the cutter runs into the material by half diameter before setting back for the right contour. In the programming manual which was posted in the former thread on comment 46 (https://forums.autodesk.com/t5/hsm-post-processor-forum/postprocessor-maho-or-changing-of-axes-in-di...) the coordinates are shown in the G43/G44 one line earlier instead of the G41/G42 command.

Same issure ocurres on the G40 command, the cutter runs into the material and then retracts again;

I´m not 100% sure if this will solve my issue but I´m willing to try it if you could provide the PP with changes included!

Regards,

Thomas

[AchimN]

@Barbatoss thanks for your feedback.

The updated post will be online in a few minutes. Let me know how it goes.

[Anonymous]

Hey Achim

Philips 432 is also interesting for me (remember me from the philips 3480 turning series)

My machine wants this hook-symbol in the last line, otherwhise there is an error an the last lines are not transfered.

It's the same sign like the 3480 control needs at the end of the code:

https://forums.autodesk.com/autodesk/attachments/autodesk/218/2614/2/12536_9977.nc

I dont know what sign that is in ASCII... so I call it "hook"

Could you add that for me ?

Greetings

Julian

[Barbatoss]

Hey Achim,

so the post seems to work fine! At least 99.95% of the time.

Or maybe even 100% and my machine shows strange behaviors.

The phenomenon I spoke about in my last post still occurs.

The mill runs into my workpiece and then sets back before following the correct contour.

But neither HSM nor the simulation in the NC Editor shows this movement.

Maybe I could send you the code for a professional glance at it?

Regards Thomas

[Anonymous]

Hi Thomas,

i think this is not a problem from the pp, but rather from the old Philips 432 Software with the radius correctur.

I can show you how to fix the Problem maybe today or tomorrow in the evening, it´s a little bit tricky.  

Greets Marc 

[AchimN]

@Barbatoss Although I don´t know your nc program, I could imagine that the reason is following:

By looking into the manual it is needed that the G43/G44 movement is perpendicular:

 So you have to enable "perpendicular" into your operation and make sure that the lead in sweep angle is set to 90deg:

 You will now see that the toolpath looks like this:

The "perpendicular" setting is not enabled by default in HSM, so I could imagine that you have X AND Z coordinates into your G43 line which causes the problem your are talking about.

Please test that and let me know if it worked on your machine.

Into the post processor I will add code to verify that the G43/G44 line has just one coordinate in it to make sure that the movement is perpendicular.

[Anonymous]

Hi AchimN,

you are right, i fixed the Problem like this. 🙂 

greets Marc 

[AchimN]

@Anonymous ok perfect, thanks for your feedback 🙂

[Barbatoss]

@AchimN, @Anonymous:

Guys, thanks for your support! This was exactly what made my issue disappear!

As so often... dullness is sitting behind the screen 🙂

I´ve done some milling meanwhile and until now everything works fine.

I´ll keep you updated!

Regards,

Thomas

[dudukovic_goran]

Hello Achim, thanks for the PP.
Is this PP can handle with 4 axis ?
On Maho machine this is B Axis ( turning table )

[dudukovic_goran]

Hello Achim, thanks for the PP.
Is this PP can handle with 4 axis ?
On Maho machine this is B Axis ( turning table around vertical axis)

[dudukovic_goran]

I just test the pp
Can you do boring ? I cud not, only do point by point, not with G3/G2 ( yes, I turn on helical)
And even with that, he do some wrong circle in last line
And why use G98/G99 in frst line ?

[AchimN]

@dudukovic_goran 4th axis table is not implementet, but you can switch between vertical and horizontal machining. What do you mean by boring? You mean the drill cycle or bore milling?

[dudukovic_goran]

I mean bore miling. And yes, I turn on helical 🙂

[AchimN]

So you would like to see G2/3 for bore milling? What is wrong with last circle? Do you have sample code to show the problem?

[dudukovic_goran]

Yes
I have pp that you relase about 2 year ago, for 532, and for now its olmost perfect, with cosmetic change I done
So I dont now why now that new pp, with that error 🙂
https://ibb.co/f2eafG new pp
https://ibb.co/jqVWLG my old pp, work fine
I hope that link with picture will work

[dudukovic_goran]

Mistake, code with G1 and strange circle on the end is yor new pp
Code with G3 is your old pp
And wath is G98 and G99 on the start in new pp
I can send you my pp

[Barbatoss]

Hi Achim!

In my opinion, the depth values for all drilling/tapping/... operations should be (cycle.bottom - cycle.stock) instead of (cycle.bottom) as the programming manual I have (on page 44) defines z-values as incremental.

I have had trouble in the past with my machine drilling holes deeper as I wanted them as soon as I changed the "start height" of my drilling operation from "stock" to "hole start plane". (sorry for my poor german-english translation).

Having changed the PP it seems to work for me now.

Regards, Thomas

cycle definition G81

[Anonymous]

Hi Barbatoss

Yes, that's a problem... i always change the values by hand cause i'm very bad with changing PP stuff...

Maybe Achim can change this in the official PP ?!'

There is a similar prob with the Heidenhain 155 PP, if there is a bore which is not in Z=0 but deeper, the machine drives down with the boring feed instead of FMAX...