What's new
What's new

Heidenhain Visi/Work NC Post Issues?

Heidenhain doesn't do options. IT aint fanuc, so, for instance, you don't pay heidenhain for rigid tapping, any control that is capable will do it.
I know nuthin bout no 5 axis, but the code after line 30 looks fine.
what does this mean?
28 CYCL DEF 32.2 HSC-MODE:1 TA5

Heidenhain service in Schaumberg is the best, give them a call
fanuc equivalent of G5.1, haas equivalent of p187 etc, smoothing control. 1 means its in roughing mode which should move freely.
 
Our Visi Post for 5 Axis Heidenhain works great.

Of course there are also machine specific things.

Depends on the dynamic of your machine, for me it looks like the tolerance cycle is limits your movement.

26 CYCL DEF 32.0 TOLERANCE
27 CYCL DEF 32.1 T0.0012
28 CYCL DEF 32.2 HSC-MODE:1 TA5

The machine needs to hit all axis below the tolerance of 0.0012 which will take a bit of adjustment at the end of the movement which could look like its standing still.

Have you tried it with a greater tolerance value?
Hi,

Yes we have tried opening up that tolerance. Another reply has me curious. Does your Visi post output 'M128' or 'FUNCTION TCPM' to activate live 5?

Here's the reply:
'Your line 20, try FUNCTION TCPM rather than M128'

Let me know please! It would be awesome if we could see the first 50 or so lines output from your Visi Live 5 post as well so we can compare to ours. Any random full 5 program would be helpful.
 
Its the tolerance in the round axis, -> A and C in this case.

1 means its activated and TA5 means it can differ up to 5° from the nominal value. Which seems alot, but for a ballnose it does not mater cause the control will adjust the XYZ axis to reach the right point (thanks to TCMP or M128).
But you have be carefull if you are milling 5X with a endmill, then you need a very low TA value (mine is at 0.1 at default, i even lower it for said application).

But a greater TA value means smoother 5X travels in most cases.
This actually answers another question of ours. Thankyou!
 
We use WorkNC to do simultaneous paths on our Promac with a 530 controller. I noticed your CYCL DEF 32 is set up for roughing. Is this what you want? HSC-MODE=1 is roughing. HSC-MODE=0 is finishing. If you do in fact want to set your controller tolerance for roughing, then I would relax that T value to something not so tight. Here is what our CYCL DEF 32 looks like (the T values are metric):

Roughing:
CYCL DEF 32.0
CYCL DEF 32.1 T0.1
CYCL DEF 32.2 HSC-MODE:1 TA1

Finishing:
CYCL DEF 32.0
CYCL DEF 32.1 T0.015
CYCL DEF 32.2 HSC-MODE:0 TA1

I would remove the PLANE RESET STAY and replace it with M129. The 530 controller might not support PLANE SPATIAL, depending on how old it is. We've got some that do and some that don't (I think our machines build before 1995 or 1996 don't support PLANE SPATIAL).

M128 does work on the 530 controllers. We use it for doing simu. I would remove the M126 as rotating the shortest distance isn't necessarily a good thing doing full simu. We use it for our Hermles doing 3+2 but not for simu.

I'm not saying these changes will solve your issue, but the code from line 30 on doesn't look problematic so I don't think that's where the issue is. If this was happening to us I would be taking a close look at your controller settings to make sure there isn't a setting to allow full simu that needs to be turned on. I'm not strong on the controller side, my expertise is on the post writing side of things.

Hope this helps,

Dan
 
We use WorkNC to do simultaneous paths on our Promac with a 530 controller. I noticed your CYCL DEF 32 is set up for roughing. Is this what you want? HSC-MODE=1 is roughing. HSC-MODE=0 is finishing. If you do in fact want to set your controller tolerance for roughing, then I would relax that T value to something not so tight. Here is what our CYCL DEF 32 looks like (the T values are metric):

Roughing:
CYCL DEF 32.0
CYCL DEF 32.1 T0.1
CYCL DEF 32.2 HSC-MODE:1 TA1

Finishing:
CYCL DEF 32.0
CYCL DEF 32.1 T0.015
CYCL DEF 32.2 HSC-MODE:0 TA1
Oh yeah true, i mixed that up in my post. HSC-Mode is not on or off, its for roughing and finishing!
 








 
Back
Top