gangtool setup / backtools

More
05 Oct 2012 12:49 #24985 by BigJohnT
gmouer wrote:

Thanks, BigJohnT

WIsh you had some of those suggestions earlier in this thread. Using axis coordinate system rotation for handling front/rear lathe tools was never suggested. Once known, using remap and the command formats are pretty obvious. I try not to ask things with obvious answers that can be found with a bit of research.


Hind sight is always 20-20... I was once asked how long will it take to design this machine? My answer was how long does it take to find an unknown solution to a problem?

John

Please Log in or Create an account to join the conversation.

More
05 Oct 2012 15:24 #24990 by ArcEye
Andy Pugh wrote:

Someone with a lathe config in front of them needs to experiment before we go too far down this route.

Looks good to me, the Z symbol is reversed, but other than that X and Z axes both move in the correct direction with positive and negative values and the tool plot is now on the top where it should be, with a slant bed / back tool lathe.

Well done, I shall just implement it with a preamble setting for ngcgui, as that is what I use almost exclusively.

regards

Please Log in or Create an account to join the conversation.

More
05 Oct 2012 20:47 #25023 by gmouer
ArcEye wrote:

Andy Pugh wrote:

Someone with a lathe config in front of them needs to experiment before we go too far down this route.

Looks good to me, the Z symbol is reversed, but other than that X and Z axes both move in the correct direction with positive and negative values and the tool plot is now on the top where it should be, with a slant bed / back tool lathe.

Well done, I shall just implement it with a preamble setting for ngcgui, as that is what I use almost exclusively.

regards


I agree with all of ArcEye's findings. The Z symbol is reversed but shows on the backside of the Z axis, setting up back tools as type 8 would maybe fix that. Of course there is no onscreen indication that you are operating in a rotated coordinate system (except the tool indicator is behind the Z line) so you have to pay attention if you are rotated or not otherwise you could get into trouble of course.

All in all it works extremely well. A remap of G68 and G69 to turn off and on the rotation puts the icing on the cake.

How can we get this into the lathe section of the docs for others in the future?

Thanks all !!!

Please Log in or Create an account to join the conversation.

More
05 Oct 2012 21:07 #25027 by BigJohnT
gmouer wrote:

All in all it works extremely well. A remap of G68 and G69 to turn off and on the rotation puts the icing on the cake.

How can we get this into the lathe section of the docs for others in the future?

Thanks all !!!


You could add a GladeVCP panel and using the python interface to LinuxCNC show the rotation angle of G54.

Write me something up about what you want to include in the lathe docs. When you get something send me an email and I'll respond so you can send the text file. We use asciidoc so plain text is the format.

John

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 01:40 #25046 by gmouer
Well, I spent many hours attempting to remap G68 and G69 to the appropriate G10 rotation commands with total failure. I got a g68 and g69 subroutine to work but no luck remapping to it.


According to the docs for remap, only modal group 1 G codes can be remapped AND remapping G68 to the G10 makes it a modalgroup 0 ,, so no-can-do. If G68 and G69 are going to be implemented for this purpose it will have to be done by some of the developer boys it looks like.

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 10:51 - 06 Oct 2012 10:52 #25058 by BigJohnT
I don't think that is the problem as I could not get a simple msg to remap... I think there is a missing clue yet to be found.

John
Last edit: 06 Oct 2012 10:52 by BigJohnT.

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 11:39 #25059 by BigJohnT
I got the G68 remap to work somewhat using the simple remap example.

REMAP=G68.0 modalgroup=1 ngc=g680

put g680.ngc in the nc_files directory of the RIP
o<g680> sub

(msg, g680)

; signal success be returning a value > 0:
o<g680> endsub [1]

m2

make sure you run . ./scripts/rip-environment of course if you install master you don't need to do this.

At this point g68 wants and axis or it complains about missing axis so there is still a missing clue.

John

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 11:46 #25060 by BigJohnT
I did figure out that modal group 1 is a motion group and requires an axis word, so until motion group 0 is supported your much better off just using G10.

John

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 14:36 - 06 Oct 2012 14:37 #25062 by gmouer
I got a g68 subroutine setup and called by a G68 remap. If I put the G10 code line in that subroutine it errors out. SImply substituting M3 for the G10 line of code and it works nicely. If I type G68 on the MDI line, the spindle turns on. Put the G10 line back in, replacing the M3, and it is back to faulting.

If I call the G68 sub directly from the mdi line, with the G10 code in the sub, it works nicely. The G68 remap faults in that case.

It also worked nicely with a MSG line in the subroutine, a G68 in the MDI produced the message onscreen.

Success or failute seems to be determined by the code line executed in the subroutine. G10 (modalgroup 0) faults, M3 or a MSG command executes nicely on the remap.

The only difference I can see in the above tests was the G10 line in the subroutine file. G10 is a modalgroup 0 command AND in the remap doc it clearly states that only modalgroup 1 remaps are supported. Apparently, they mean it.

In all tests, no axis words were used.

I learned a lot last night experimenting and researching further.
Last edit: 06 Oct 2012 14:37 by gmouer.

Please Log in or Create an account to join the conversation.

More
06 Oct 2012 14:45 #25064 by gmouer
BigJohnT wrote:

I did figure out that modal group 1 is a motion group and requires an axis word, so until motion group 0 is supported your much better off just using G10.

John


I don't see any choice at the present other than using G10. Its not that bad, at least the axis coordinate system can be rotated which makes handling rear tooling much simpler.

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.089 seconds
Powered by Kunena Forum