Heidenhain Visi/Work NC Post Issues?

[BKuiphof]

Hi,

We have a large 5-Axis mill with a Heidenhain controller we are looking to run some live 5-Axis programs on. Currently, the machine will move line by line and stop at every line instead of feeding continuously throughout the program. For some reason, it seems Visi/Work NC have never had a live 5-axis post for a Heidenhain control before (same old BS).... lol

We're convinced it's an issue with the post. We may be wrong though and maybe there's a setting/parameter that needs to be changed to activate live-5 on the control?

Here's an example of the programs our posts are spitting out now:

0 BEGIN PGM VISI TEST 5AX CODE INCH
1 M129
2 ;
3 * ;-
4 ; BALL NOSE
PLANE RESET STAY
5 ;
6 ; SAFETY POSITION
7 L Z-3. FMAX M91 ;Z-SAFETY
8 ;
9 L C0 A0 R0 FMAX
10 CYCL DEF 247 DATUM SETTING ~
11 Q339=+1 ;Datum Number
12 ;BALLNOSE DIAMETER +0.25 LENGTH 2.437
13 TOOL CALL 125 Z S2000
14 L M3
PLANE RESET STAY
15 CYCL DEF 7.0 DATUM SHIFT
16 CYCL DEF 7.1 X+0.
17 CYCL DEF 7.2 Y+0.
18 CYCL DEF 7.3 Z+0.
19 ;
20 M128 ; TCPM ON
21 M126 ; SHORTEST PATH TRAVEL
22 M11 ; UNLOCK AXIS
23 L X+1.74998 Y+2.30159 C-0.013 FMAX
24 L Z+6.4 FMAX
25 L A+10. FMAX
26 CYCL DEF 32.0 TOLERANCE
27 CYCL DEF 32.1 T0.0012
28 CYCL DEF 32.2 HSC-MODE:1 TA5
29 L R0 FMAX
30 L Y+2.32484 Z+6.26812 FMAX
31 L X+1.75001 Y+2.3943 Z+5.8742 A+10. C-0.013 F100
32 L X-1.74959 Y+2.3943 Z+5.8742 A+10. C+0.136
33 L X-1.76448 Y+2.39411 Z+5.8742 A+10. C+1.086
34 L X-1.79334 Y+2.39284 Z+5.87419 A+10. C+3.926
35 L X-1.82209 Y+2.39026 Z+5.8742 A+10. C+6.408
36 L X-1.85133 Y+2.38628 Z+5.87419 A+10. C+9.072
37 L X-1.87359 Y+2.38234 Z+5.87421 A+10. C+11.456
38 L X-1.89553 Y+2.37766 Z+5.87424 A+10. C+13.419
39 L X-1.91845 Y+2.3719 Z+5.87424 A+10.001 C+14.668
40 L X-1.94241 Y+2.3649 Z+5.8742 A+10. C+17.383
41 L X-1.96596 Y+2.35703 Z+5.8742 A+10. C+19.554
42 L X-1.98933 Y+2.3482 Z+5.8742 A+10. C+22.104
43 L X-2.01217 Y+2.33855 Z+5.87423 A+10. C+23.79
44 L X-2.03538 Y+2.32765 Z+5.8742 A+10. C+26.315
45 L X-2.05805 Y+2.31589 Z+5.8742 A+10. C+28.597
46 L X-2.08023 Y+2.30324 Z+5.87421 A+10. C+30.855
47 L X-2.10207 Y+2.2896 Z+5.87421 A+10. C+33.122
48 L X-2.12355 Y+2.27497 Z+5.87421 A+10. C+35.405
49 L X-2.14439 Y+2.25949 Z+5.8742 A+10. C+37.703
50 L X-2.16462 Y+2.24316 Z+5.8742 A+10. C+40.024

Every move after line 30 the machine makes the move and then stops instead of moving smoothly through those moves.

What would be greatly appreciated would be if any of you have a live-5 post for Visi/Work NC and wouldn't mind outputting some random program for us. Then we can compare programs and change the post accordingly.

Any help with this would be greatly appreciated!

Thanks,
Brandon

 

[Houdini]

Interesting, I'm not a 5 axis guy, wonder if this is what happens when you run a simultaneous program on a positional machine

 

[empower]

can you tell if the a/c brakes are being turned on/off?

 

[empower]

Interesting, I'm not a 5 axis guy, wonder if this is what happens when you run a simultaneous program on a positional machine

wont let you.

 

[BKuiphof]

can you tell if the a/c brakes are being turned on/off?

I believe the '22 M11 ; UNLOCK AXIS' turns the breaks off. Maybe that needs to be in every line? We've also tried adding feed rates to every line with no change. The operator doesn't believe the breaks are locking and unlocking but I'll get eyeballs on the machine while it's making it's moves to verify that.

 

[empower]

I believe the '22 M11 ; UNLOCK AXIS' turns the breaks off. Maybe that needs to be in every line? We've also tried adding feed rates to every line with no change. The operator doesn't believe the breaks are locking and unlocking but I'll get eyeballs on the machine while it's making it's moves to verify that.

ah, didnt notice.
what tolerances are being used in CAM? can you show a video of the motion?

 

[BKuiphof]

what tolerances are being used in CAM? can you show a video of the motion?

Unfortunately I can't get a video of the motion at the moment. The best way I can describe it is that it looks like a 3+2 program getting to position then stopping, moving to the next 3+2 position, then stopping, etc.

Tolerances in the program are set to what we would normally use (.002 or less?). We have a few other 5-axis mills around here with Fanuc controls and live-5 seems to work fine in those machines. Of course the code will look completely different from a Gcode file vs. Heidenhain's conversational format.

 

[empower]

Unfortunately I can't get a video of the motion at the moment. The best way I can describe it is that it looks like a 3+2 program getting to position then stopping, moving to the next 3+2 position, then stopping, etc.

Tolerances in the program are set to what we would normally use (.002 or less?). We have a few other 5-axis mills around here with Fanuc controls and live-5 seems to work fine in those machines. Of course the code will look completely different from a Gcode file vs. Heidenhain's conversational format.

what machine is this, how old, which HH control? i'd look into what options were purchased with that control. have you tried reaching out to the builder?

 

[BKuiphof]

what machine is this, how old, which HH control? i'd look into what options were purchased with that control. have you tried reaching out to the builder?

This is an old ProMac mill. No support for the machine because no one makes them anymore (We're great at getting our hands on machines with no support lol...). Control is the iTNC530. I've thought about getting ahold of HH themselves too. Is there a way we can quick check the options purchased on the control itself?

 

[empower]

This is an old ProMac mill. No support for the machine because no one makes them anymore (We're great at getting our hands on machines with no support lol...). Control is the iTNC530. I've thought about getting ahold of HH themselves too. Is there a way we can quick check the options purchased on the control itself?

there is, i think from the edit screen, hit the mod key, and dig around in those menus, should be somewhere there, i forget which option it is exactly.

but yea, you should be able to call HH usa and talk to their apps guys, they're very helpful.

 

[JtM90]

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?

 

[5 axis Fidia guy]

Your line 20, try FUNCTION TCPM rather than M128

 

[empower]

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?

thats pretty open tolerance for HH, shouldnt be an issue.

 

[JtM90]

thats pretty open tolerance for HH, shouldnt be an issue.

Well the OP said that its an old Promac mill and for such a thing i dont consider this open.

But it also depends on you HH version, do we know about that?
Cause if its 426/430 5X is not really usabe imo.

 

[empower]

Well the OP said that its an old Promac mill and for such a thing i dont consider this open.

But it also depends on you HH version, do we know about that?
Cause if its 426/430 5X is not really usabe imo.

he said its a 530 control, which is quite modern. if it has the correct options installed, that tolerance should NOT be an issue. it would slow down to hit it, but not stutter. again, need to check what options are installed in that control first.

 

[JtM90]

he said its a 530 control, which is quite modern. if it has the correct options installed, that tolerance should NOT be an issue. it would slow down to hit it, but not stutter. again, need to check what options are installed in that control first.

overlooked that, yeah you are right, for a 530 it should be fine

 

[gustafson]

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

 

[JtM90]

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

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.

 

[gustafson]

THere used to be on older controls either an m function or parameter for 'positive stop' I have never used it but I remember seeing it

 

[gustafson]

Again dunno 5 axis, but in 3 axis the tolerance parameter is optional. If it is moving in space[IOW no risk of crashing anything] try deleting that. In 3 axis that just returns it to whatever the default is.
Look up M109/M110 constant contouring speed, reset with 111