Understanding G68.2

[al.whatmough]

In the last few weeks the topic of multi-sided programming has come up serval times.
Many users program many diffent ways.  One of thoes ways is the use of 68.2

So, I decided to describe how to use G68.2 with HSMWorks.

G68.2 Allows the operator to see Gcode positions that are relative to a given point on the model with out the need of creating a new Work Offset.



To keep this explanation simple we are going to machine 3 lines on perpendicular faces of a  3” square block.



The Feed plane, Retract plane and Clearance plane will all be 1" from each other.  To keep the code easy to follow.



In our example, we are setting G54 on the face of the part.



Let’s first post this program using G68.2 with just a rotary transformation.



(Above) Notice the J90. So, the Z value is now relative the 90 Deg face.  However, X & Y are still referencing the G54 location. (Below) As such, when the we reach full depth we are a Z 1.5 and the center of the part is @ X 1.5.
(The machine control to taking into account all the offsets relative to the center of rotation)



Now, Let’s post the same program but using a outputting a transformation for XYZ as well.



68.2 Has now also captured the X Y Z Transformation so the operator now sees numbers relative to that face and orientation.
So, how did we handle this in HSMWorks?  It was simple.
I simply activated tool orientation and selected my SolidWorks coordinate system for that orientation.
(I could have also uses Point and orientation and simply selected a face for z to be perpendicular too and a point for my origin point)



I then used Posted the program with a post that supports G68.2 with X Y Z transformations.

So, what do you need to do?

Just check and see if your machine supports g68.2.

[al.whatmough]

More pics

[Rob.Lockwood]

I hate to admit this, as i'm usually pretty good at this stuff..

But I have no idea what you're talking about.

😕

[al.whatmough]

It makes more sense when the images line up with the text...


Let me try to get it formatted better.

[Ales_Prochaska]

A. Whatmough wrote:

There is command G68.2 with non-zero XYZ values in your example. Is it generated by HSMWorks? I always obtain G68.2 with X0 Y0 Z0, used only for new plane orientation, not for XYZ origin. XYZ offset is added to following moving commands values.

[cj.abraham]

Ales,

HSMWorks sees the distance between the Job WCS and a coordinate system selected for tool orientation, which will then be applied to G68.2 (assuming the post was set up for G68.2) If the two match, XYZ will all be zero.

Rob,

It's like using multiple offsets to get around a part (G54, G55, G56). However, instead of using up those offsets, you use one offset (G54) and then move the coordinate system incrementally in the program. (If your machine supports G68.2)

[Rob.Lockwood]

CJ wrote:

Ales, HSMWorks sees the distance between the Job WCS and a coordinate system selected for tool orientation, which will then be applied to G68.2 (assuming the post was set up for G68.2) If the two match, XYZ will all be zero. Rob, It's like using multiple offsets to get around a part (G54, G55, G56). However, instead of using up those offsets, you use one offset (G54) and then move the coordinate system incrementally in the program. (If your machine supports G68.2)

Huh.. So somewhat like using g52? I'll look into whether anything we have has g68.2 support..

[cj.abraham]

Yep. It just works in conjunction with a stored center of rotation on the machine.

G68.2 wouldn't be my first choice though. It's an option available in HSMWorks to those who want it.

[mcarney_12]

Is there a command that returns to the original orientation?  Or how might I do that? My post processor seems to handle 3+2 operations, but when I try to do a basic 3axis on the original coordinate system it never returns.

I was thinking something along the lines of:

G69
G53 G0 Z0
G68.2 X0. Y0. Z0. I0. J0. K0. U0. V0. W0.
G54

any other suggestions?

[Laurens-3DTechDraw · Accepted solution]

CJ wrote:
Yep. It just works in conjunction with a stored center of rotation on the machine. G68.2 wouldn't be my first choice though. It's an option available in HSMWorks to those who want it.

Why would it not be your first choice?
You rather program from dead center on a 5-Axis machine?

G52 and G68.2 in fact are totally different. G52 is just to move the wcs without using another set wcs in the machine. So you just move the G54 for example.

G68.2 has as main point that your axis always stay like they are in real life. So if you turn your machine table(4/5-Axis) 90 degrees normally you would program from dead center and if you program a Z-move actually your Y-axis will start to move. With G68.2 you can put you wcs anywhere you like and when the table or head is rotated it it moves this wcs point to stay on that place on the part. Due to the machine kinematics being in the machine. It's like Cycle 19/Plane Spatial on Heidenhain controls.



So let me try to explain it's use better. It's mostly called TCPM or RTCP (Although those moslty also include other features). With TCPM you program a 5-axis part just like you do a 3-axis part. You place your zeropoint where you can probe easily(That may be on the vice or the part/stock piece). While you program you don't take into account where this zero-point is going to be in the machine it's self. Without the TCPM you must set the zero point in your CAM system to the true centerpoint of your machine, so the workflow would be to place the part in the machine, probe it's offset to the center point and adjust your coordinate systems place. If the next piece is a little of this location you need to do the whole thin again, change WCS location in your CAM system post processes again and look carefully everything goes alright.
The G68.2(Fanuc) and Plane Spatial(Heidenhain) take this compensation a step further. They also rotate the coordinate system that you put on the WCS so to speak. This meand that you can just keep programming Z as the movement of the machine up and down, and not in the way it was originally before you started to turn your 4th-/5th-/6th-Axis.

[Greg_Haisley]

I'm with Rob on this one. Maybe I'm a bit too old to understand. I know my machines don't support G68.2.

I program from the center of rotation for the WCS whether 4 axis or 5 axis. The numbers are all over the place relative the the WCS but the parts come out fine. I have also added additional WCS's for different 4th and 5th rotations for allowing the operator to make small adjustments at the machine verses moving the model in the CAD and reposting.

Everybody has there preferred way of getting the job done.

[Rob.Lockwood]

While I didnt follow the purpose when this thread initially came about, ive come to understand it much better recently; I'm just not sure why one would want to use it as demonstrated in this thread, though I probably should give the OP a second pass, I'm sure it would make more sense.

If you want to program a 5x part that's relatively agnostic to the machine you want to run it on.. And/or if your workflow requires blocks to be placed somewhat uncontrolled on the table.. Or if you want to do 5x features, for instance on castings, where features need to be accurate relative a physical location on the part which can't be easily accounted for in CAD. I THINK this last instance is what the OP had in mind? Ramble ramble ramble..

[Laurens-3DTechDraw]

Rob Lockwood wrote:

While I didnt follow the purpose when this thread initially came about, ive come to understand it much better recently; I'm just not sure why one would want to use it as demonstrated in this thread, though I probably should give the OP a second pass, I'm sure it would make more sense. If you want to program a 5x part that's relatively agnostic to the machine you want to run it on.. And/or if your workflow requires blocks to be placed somewhat uncontrolled on the table.. Or if you want to do 5x features, for instance on castings, where features need to be accurate relative a physical location on the part which can't be easily accounted for in CAD. I THINK this last instance is what the OP had in mind? Ramble ramble ramble..

Yes its like the video CJ showed no harder to program 5-axis than 3-axis if your machine supports this. If you pay the flights I'll explain it all when the 5-axis comes in 😛
Part of the point is that it doesn't matter what the machine is you are going to run it on where with the "old" option it does matter what the layout of the machine is.

You definitely need this on machines that have a milling head that rotates.

[Laurens-3DTechDraw]

Greg Haisley wrote:

I'm with Rob on this one. Maybe I'm a bit too old to understand. I know my machines don't support G68.2. I program from the center of rotation for the WCS whether 4 axis or 5 axis. The numbers are all over the place relative the the WCS but the parts come out fine. I have also added additional WCS's for different 4th and 5th rotations for allowing the operator to make small adjustments at the machine verses moving the model in the CAD and reposting. Everybody has there preferred way of getting the job done.

I think indeed Greg this to someone that is used to the old way doesn't seem much easier without seeing it in action.

[nick]

Greg Haisley wrote:

I'm with Rob on this one. Maybe I'm a bit too old to understand. I know my machines don't support G68.2. I program from the center of rotation for the WCS whether 4 axis or 5 axis. The numbers are all over the place relative the the WCS but the parts come out fine. I have also added additional WCS's for different 4th and 5th rotations for allowing the operator to make small adjustments at the machine verses moving the model in the CAD and reposting. Everybody has there preferred way of getting the job done.

Greg, I have a horizontal tombstone on my vertical VMC and program it as you do with WCS at the center of rotation. Question; how are you adding the additional WCS points and adjusting at the machine? I'm having to resort to running back to adjust in CAD... your method would be ideal and really help.

[Greg_Haisley]

nickglobal101 wrote:

Greg Haisley wrote: I'm with Rob on this one. Maybe I'm a bit too old to understand. I know my machines don't support G68.2. I program from the center of rotation for the WCS whether 4 axis or 5 axis. The numbers are all over the place relative the the WCS but the parts come out fine. I have also added additional WCS's for different 4th and 5th rotations for allowing the operator to make small adjustments at the machine verses moving the model in the CAD and reposting. Everybody has there preferred way of getting the job done. Greg, I have a horizontal tombstone on my vertical VMC and program it as you do with WCS at the center of rotation. Question; how are you adding the additional WCS points and adjusting at the machine? I'm having to resort to running back to adjust in CAD... your method would be ideal and really help.

Nick, you can break up the operations in different jobs with additional unique work offsets for each side that are in the same location as the original but rotated to a different angles for features used on that angle. Posting all these jobs at once the operator will be able to make adjustments for the additional work offsets to move features on those sides relative to features on the original side. I have done this on tight tolerance parts. I too sometimes move the model in CAD, regen and repost. Both ways will work. The additional work offset is user friendly once you understand how it affects the part. Getting to know where the features move relative the the other side is the learning curve. When you look at the model with all jobs highlighted you should see all the work offsets turned in the different directions.

Hope this helps. Good luck.

[nick]

Greg Haisley wrote:

Nick, you can break up the operations in different jobs with additional unique work offsets for each side that are in the same location as the original but rotated to a different angles for features used on that angle. Posting all these jobs at once the operator will be able to make adjustments for the additional work offsets to move features on those sides relative to features on the original side. I have done this on tight tolerance parts. I too sometimes move the model in CAD, regen and repost. Both ways will work. The additional work offset is user friendly once you understand how it affects the part. Getting to know where the features move relative the the other side is the learning curve. When you look at the model with all jobs highlighted you should see all the work offsets turned in the different directions. Hope this helps. Good luck.

Thanks, Greg. That's along the lines what I thought--but was not sure if there was a special technique involved where the offsets adjust in conjunction with the center of rotation.  It sounds like the G68.2 would be pretty slick to use (if I understand it correctly).  Thanks!

[nick]

A. Whatmough wrote:
So, how did we handle this in HSMWorks?  It was simple. I simply activated tool orientation and selected my SolidWorks coordinate system for that orientation. (I could have also uses Point and orientation and simply selected a face for z to be perpendicular too and a point for my origin point)

@A. Whatmough, I'm trying to be clear on how to use this in Inventor HSM.  Couple questions if you could please help clarify:

1. Aside from G54, do I need to set a coordinate for the center of rotation of the tombstone? In one of your images, it states "Machine Center of Rotation (Stored in Machine Control)" -- I'm not sure how that works exactly on a VMC with a 4th axis tombstone (maybe this is specific only to Horizontals?)--how is this stored on a VMC 4th>?

2. In the above quote from your post, you show how this is done in Solidworks--however, Inventor HSM has it a little different; what would I set? (image attached).

This sounds like it would be a great way of programming--if I can fully understand and implement it. Thanks!

[scottmoyse]

---

@al.whatmough wrote:
....

To keep this explanation simple we are going to machine 3 lines on perpendicular faces of a  3” square block.



The Feed plane, Retract plane and Clearance plane will all be 1" from each other.  To keep the code easy to follow.



.....

---

@al.whatmough any chance of fixing up the image links in your OP please? It's a valuable post, but all the image links are broken since the migration.