What's new
What's new

5 axis part alignment in B and C axis using Heidenhain 530 control

Redwineracing

Plastic
Joined
Mar 16, 2018
Does anyone know how to align a part using both B and C axis. (Mikron HPM450 with a Heidenhain 530i)
We have aligned the part to both B and C axis but when running the program it gets lost when it comes to machining a hole at a compound angle.
If we align the part to the bed of the machine the program works fine. But as these are casting this can take a long time. So align the part and re setting both B and C axis to Zero would seem to be the way to go.
Any advice would be appreciated.
 
On my DMG I can tilt the head and apply plane axis move (or cycle 19 or several others) and the plane of the probe will then have changed.
Then probe the surface.

If you need to compute the angle from the part, I would think you would probe it with B=0 C=0, compute the angle you want, rotate the part AND apply a coordinate system rotation, then probe holes or other pickup features.

Or do I misunderstand your question?
 
Does anyone know how to align a part using both B and C axis. (Mikron HPM450 with a Heidenhain 530i)
We have aligned the part to both B and C axis but when running the program it gets lost when it comes to machining a hole at a compound angle.
If we align the part to the bed of the machine the program works fine. But as these are casting this can take a long time. So align the part and re setting both B and C axis to Zero would seem to be the way to go.
Any advice would be appreciated.

@Redwineracing That's a beautiful machine... VERY nice...


The thing that's odd about your machine as I'm sure you know...

https://www.gfms.com/content/dam/gf...performance_machine/en/mikron-hpm-450u_en.pdf

Is that is says " Cartesian (rectangular) alignment of the axes - results in coherent tool/workpiece movement during the milling process "

Which is an odd thing to say, but basically the knuckle style rotary MOVES in X axis as you face the machine, but the Spindle moves in Y (to and fro) and up and down in Z.



__________________________________________________ _________________________________


I'm kinda interested in this as I'm having to dig deep on the Heidenhain (or Heiden-pain (as some call it TNC 640 or go Smooth X / Mazak from now until I kick the bucket).

I'll put my thinking cap on about the transformations you are doing + probing versus aligned to the "bed" of the machine... Are you using a DTI / indicator to do that or are you probing also in some way (dumb question) ?

Not sure about dynamic work offsets (G54.4) setting + Tool CenterPoint control on the 530i + (Start up modes and what you have reset/ clear on your program too … ).


Are there special cuts and tolerances you need for the first set up you are using ?

_________________________________________________________________________________________


On a regular trunnion machine the Spindle moves in XY and Z, on your machine the knuckle moves in the opposite direction for X … So I'm wondering + or - sign in your post might need to be flipped + order of rotations vs probing ? Kinda hard to visualize without the set up / more detail. [Don't mess about with my rubbish and crash your machine until there is a smidge more clarity].

Also wondering about the intersection point of your B and C axes how far above the table that comes relative to your part ?

Do you do any type of Axi-set (Kinematic option) calibration on a tooling ball kind of thing?

When you say it gets "lost" how far / how bad... do you have to hit the E-stop or does it just "Machine it's hole" in the wrong place by a few thousandths. Is it wrong angle / tool poise or correct angles but wrong position "On face" ?

Things to cancel (in more generic G code / fanuc at the start of program)

G54.4 cancel any active WSEC "workpiece setting error compensation".
G80
G40 <-- (cancel) - any tool radius comp.
G49 <-- cancel TCP tool center point control.
G69 <-- Cancel previous or any tilted workplane or coordinate rotation.
G54
G90 <-- Absolute positioning
G20 ?
G94
G17.... (XY plane)

etc.

@Redwineracing was the program or code originally run on a different machine / layout ?

I'm wondering if the probing cycle messes with the "State" / modes of the machine/ program ? G54.4 P1

Does your program automatically turn off/clear TCP (Tool center point control) G49 at the end of your program... Weird things can happen there...

Are you using G54.4 or Tilted work plane G68.2 ?
 
Does anyone know how to align a part using both B and C axis. (Mikron HPM450 with a Heidenhain 530i)
We have aligned the part to both B and C axis but when running the program it gets lost when it comes to machining a hole at a compound angle.
If we align the part to the bed of the machine the program works fine. But as these are casting this can take a long time. So align the part and re setting both B and C axis to Zero would seem to be the way to go.
Any advice would be appreciated.

I used to be an applications guy at GFMS US for their Mikron Mills. What you are trying to do is not possible with the 530. As you've found, the tilting axis (B on your HPM450u) must be zero for the PLANE FUNCTIONS/M128/FUNCTION TCPM to work properly.

Depending on what you'd like to do there maybe a (involved) workaround, Have you called GF?
 
I used to be an applications guy at GFMS US for their Mikron Mills. What you are trying to do is not possible with the 530. As you've found, the tilting axis (B on your HPM450u) must be zero for the PLANE FUNCTIONS/M128/FUNCTION TCPM to work properly.

Depending on what you'd like to do there maybe a (involved) workaround, Have you called GF?

Hi Jeffers88 so you are saying you can't probe a rotated work piece to refine accuracy on the 530 ?

There probably is away to input direct values into a transformation matrix (maybe that is part of one work around (that you are suggesting) , but some sort of macro would need to be written for that? They can do that for him at GF ?)).


Is that the same on the TNC 640 ?


When GF in their literature says " Cartesian (rectangular) alignment of the axes - results in coherent tool/workpiece movement during the milling process " for HPM450u ? What does that mean.. ?


They enforce the above condition as they assume "rigid body" of the work piece rather than a workpiece that moves about and changes shape as a result of stress relief (for example various Titanium alloys ? … That you might mill out a cavity on first set up and then rotate partially completed work piece at a compound angle the "rigid body" condition is no more ?). Same for example if you have a fixture that had tooling balls that could be accessed from different positions and orientations to act as a spatial reference that can be compared to a stress relieving distorting work piece (that has to be further milled bored etc from different positions and orientations ?).

Maybe I completely mis-understand what's going on here ?

Maybe the machine is really for 5 axis mold work ?



:cheers:

_____________________________________________________________________________________________

@Jeffers88 do you still work with / on Heidenhain controls with another manufacturer / brand / outfit etc. ?
 
Does anyone know how to align a part using both B and C axis. (Mikron HPM450 with a Heidenhain 530i)
We have aligned the part to both B and C axis but when running the program it gets lost when it comes to machining a hole at a compound angle.
If we align the part to the bed of the machine the program works fine. But as these are casting this can take a long time. So align the part and re setting both B and C axis to Zero would seem to be the way to go.
Any advice would be appreciated.

Don't have any Heidenhain 5axis experience, so just spit balling here...

Sounds like you're using an offset in both B and C for work? Perhaps if it is anything like on my Haas control (which says to NOT use any B offsets) you can cheat this for some applications by finding the angular offset you'd need, then adding it to any b-values in the program. Eg. B[90.+#500]
 
I used to be an applications guy at GFMS US for their Mikron Mills. What you are trying to do is not possible with the 530. As you've found, the tilting axis (B on your HPM450u) must be zero for the PLANE FUNCTIONS/M128/FUNCTION TCPM to work properly.

Depending on what you'd like to do there maybe a (involved) workaround, Have you called GF?


Seems like a ton of on line resources with


Heidenhain Programming Manuals and Operator Documentation Free Download - Helman CNC

and other

I put "PLANE FUNCTIONS/M128/FUNCTION TCPM" into my gooople search string..


And got a lot of direct pages and PDF's to that but curiously I can down load them and read them but can't link to them ?

But also drawing "blanks" too.

______________________________________________________

Heidenhain ISO G Codes - Helman CNC

Heidenhain M Codes - Helman CNC

______________________________________________________

This is one rabbit hole that is worth jumping down just to follow what's going on...

https://www.gfms.com/content/dam/gf...performance_machine/en/mikron-hpm-450u_en.pdf


^^^ On page 4 and 5 they show a mini tomb stone fitted to the knuckle table tilted over 90 degree with multiple and different workpieces fixtured into a three sided tomb stone and it is said that the machine can only probe work pieces with an untitled knuckle ? (How can that be ? ) No comprendo ?


Is there a custom 5 axis mold mode (written by GF) and a separate working mode for 5 axis positional (type work) where you can probe and refine position (actual in process probing for 5 axis ? (specifically for this machine so that the best intended results/design intent for the machine are upheld ?)).
 
Hi Jeffers88 so you are saying you can't probe a rotated work piece to refine accuracy on the 530 ?

There probably is away to input direct values into a transformation matrix (maybe that is part of one work around (that you are suggesting) , but some sort of macro would need to be written for that? They can do that for him at GF ?)).


Is that the same on the TNC 640 ?


When GF in their literature says " Cartesian (rectangular) alignment of the axes - results in coherent tool/workpiece movement during the milling process " for HPM450u ? What does that mean.. ?


They enforce the above condition as they assume "rigid body" of the work piece rather than a workpiece that moves about and changes shape as a result of stress relief (for example various Titanium alloys ? … That you might mill out a cavity on first set up and then rotate partially completed work piece at a compound angle the "rigid body" condition is no more ?). Same for example if you have a fixture that had tooling balls that could be accessed from different positions and orientations to act as a spatial reference that can be compared to a stress relieving distorting work piece (that has to be further milled bored etc from different positions and orientations ?).

Maybe I completely mis-understand what's going on here ?

Maybe the machine is really for 5 axis mold work ?



:cheers:

_____________________________________________________________________________________________

@Jeffers88 do you still work with / on Heidenhain controls with another manufacturer / brand / outfit etc. ?

You can absolutely probe a rotated work piece, that wasn't part of the OP's question. If I understand correctly OP wants B zero to be physically not zero, but some other angle. On the 530, you can not do this and use the TWP (PLANE FUNCTIONS/CYCLE 19), or TCP (M128/ FUNCTION TCPM). This is not a limitation on the 640.

I believe the literature is saying that the rotary axes are non-nutating.
 
Seems like a ton of on line resources with


Heidenhain Programming Manuals and Operator Documentation Free Download - Helman CNC

and other

I put "PLANE FUNCTIONS/M128/FUNCTION TCPM" into my gooople search string..


And got a lot of direct pages and PDF's to that but curiously I can down load them and read them but can't link to them ?

But also drawing "blanks" too.

______________________________________________________

Heidenhain ISO G Codes - Helman CNC

Heidenhain M Codes - Helman CNC

______________________________________________________

This is one rabbit hole that is worth jumping down just to follow what's going on...

https://www.gfms.com/content/dam/gf...performance_machine/en/mikron-hpm-450u_en.pdf


^^^ On page 4 and 5 they show a mini tomb stone fitted to the knuckle table tilted over 90 degree with multiple and different workpieces fixtured into a three sided tomb stone and it is said that the machine can only probe work pieces with an untitled knuckle ? (How can that be ? ) No comprendo ?

You are misunderstanding. You can work on a tilted plane, but you cannot set the tilting axis zero to 90 in your preset table.
 
You are misunderstanding. You can work on a tilted plane, but you cannot set the tilting axis zero to 90 in your preset table.

Ok thanks for making that clear.

That kinda makes sense to me … (If I was writing code for that I wouldn't let people do that either lol! :D ).

Not being able to do that what would you consider as the biggest obstruction to what you really want to do is ?

And are GF being helpful to you ? (Just wondering).

Cheers,

E
 
The correct procedure on a 530 would be to use touch probe cycle 431 to probe 3 points in Z, the results are the spatial angles around XYZ (output to Q170 - Q172). You can then use these values in your plane spatial function and it should make the part flat. After this you still need to probe an edge to set rotation around Z as this will probably not be correct. You must also set XYZ locations after this. Then you can use the PLANE RELATIVE function for your tilted planes... unfortunately you can only tilt over one axis at a time using this function, so it can get tricky to get where you want to go.

In TNC640 this is a standard probing cycle in the manual probe routines (the results are stored in the SPA,SPB,SPC fields of the preset table) Then you use your PLANE functions as you normally would.

Aaron
 
After this you still need to probe an edge to set rotation around Z as this will probably not be correct. You must also set XYZ locations after this. Then you can use the PLANE RELATIVE function for your tilted planes... unfortunately you can only tilt over one axis at a time using this function, so it can get tricky to get where you want to go.

In TNC640 this is a standard probing cycle in the manual probe routines (the results are stored in the SPA,SPB,SPC fields of the preset table) Then you use your PLANE functions as you normally would.

Aaron
great post.

i'll just say that the plane relative only working in on axis for this solution is perfect. Plane spatial gets you flat while plane relative rotating about C gets the system aligned with the edge of the part.
Once there i like to do a system read:
FN 18: SYSREAD QR170 = ID210 NR5 IDX1
.
.
followed by calling a final plane spatial

PLANE SPATIAL SPA+QR170 SPB+QR171 SPC+QR172 MOVE FMAX SEQ-
 
Last edited:








 
Back
Top