4 th axis rapid height Problem (V24)

[woffler]

My forth axis wants to rapid in the material , i have set the rapid height to .2 in the software .
There are three .5 pockets .1 deep .05 per pass wrapped around the stock .
I have included a zip folder with G code file BBC. file and POST. file if more is needed please let me know.
I can not figure out what is causing this could some one please look at it and see if i am missing something.

Thanks Woffler

[BurrMan]

Hi woffler,
You have a hard coded "Z 0" in the end of file portion of your post processor...



On your 4th axis, the Z 0 will be the center of the stock...

What version and build are you using? I circled in green an area that needs to be changed for later builds of V23 and also V24.. If you have 1812 or later, then you want to remove the "R" from anywhere that reads like those lines circled in green...

I didnt do anything but look at the post processor.. If you need/want to get into anything further, or want me to make the changes to the post, or run the file and the output, then respond back here...

[BurrMan]

Oooop's. I see you posted you have V24! You will want those lines to read like this:

rotary_xy_angle

Instead of "xyr"

[BurrMan]

Hi Woffler,
So here is your post processor back with the changes, "EXCEPT" for the G53 Z0 value that is causing your stock gouge...

Line 5 in your post has this:

5. End of file for non-zero tool
   n,coolant_off
   n,spindle_off
   n,"G53","Z0."
   n,"G53","Y4."
   n,end_of_file

For us, we put a G54 X0 and Y0" in the place of the 2 G53's.. The program itself will output the set rapid up as it's last command, then the machine will zero to X and Y 0 at that height...

If you know what other value you want to put there, that is the change you need to make. But if you are not using work AND machine coord systems, then you need to be careful about putting in a hard coded Z value in there.

Let me know if you want to get into it any further.

[woffler]

Thank's Burrman ,i am working with offsets and work cord's . I kind of thought it was in the post but i did not know what needed to be changed.
I can remove the (G53 Z-0), can i replace it with some thing else to move the head to the top of the coloum to get it out of my way ,that's the reason for the g53 Z0.

[BurrMan]

Thank's Burrman ,i am working with offsets and work cord's . I kind of thought it was in the post but i did not know what needed to be changed.
I can remove the (G53 Z-0), can i replace it with some thing else to move the head to the top of the coloum to get it out of my way ,that's the reason for the g53 Z0.

Yes, you know your machine and where it should go..... But Z zero on cylindrical stock, is not a good place to go! (I know you know this...)

I dont use "BOTH" the work and machine coords, so am not totally proficient in what needs to go there to move it correctly... Like, does it need to now see a G54 BEFORE the G53 or something, so it doesnt plunge to the center of the work coords...???? You may know this better than I...

At the very least as a hack, you could create a "rotary only" post processor that has a hard coded Z "uppper limits" move to get it out of the way, but I think you can get it going without doing things that way....

[woffler]

I thought about this a little bit, and we may on the wrong page here, the problem comes into play when moving from one pocket to the next.

Not at the end of the program when the spindle retracts. Or can this be caused by the xyr problem?
Or am i missing your point here ? i changed the post and put in the G54 X0,Y0 as you suggested .

[woffler]

I just read your post , a g53 will move in absolute machine coord's no matter what , it can not move to a g54 location say (Z-0 )unless you changed the g 53 to the same location and then homed to it.

[BurrMan]

I thought about this a little bit, and we may on the wrong page here, the problem comes into play when moving from one pocket to the next.

Not at the end of the program when the spindle retracts. Or can this be caused by the xyr problem?
Or am i missing your point here ? i changed the post and put in the G54 X0,Y0 as you suggested .

Yeah, try the output with the new post processor i uploaded.. If your toolpath was gouging on the op feeds, then this could/would be from the lines that needed changing that I had changed...

Your file backplots correctly for me with your post that I had changed (I just had to remove the Z0.

You are correct that the G53 should be machine home, and if that is way up somewhere, it shouldnt be going to the center of the cylinder..

Since I was working from your file with your post processor that works, I figured the issue was the ending thing. If you still experience something going wrong between the pockets with the new post I uploaded, then post back with some more details, because at this point, it backplots the code for me ok. If it is something different at your actual machine, I may need help.

[1234567]

Try g28 g91 z0.0

[woffler]

It was the (xyr) that caused the problem ,it works fine now i guess we need to update the post's for V24 to remove the R from them.
A good lesson in posts for the 4 th axis .

Thank You Burrman and to all that helped and read along