Rotary tool path output is wrong.

This forum is for general discussion regarding VCarve Pro

Rotary tool path output is wrong.

Postby PhilJohnson » Sat Jan 19, 2019 12:51 am

I hope someone from vectric.com is seeing this. I'm so excited for the rotary ability. But I found a huge glitch. It is a glitch. I just spent 4 hours digging into it. It's all explained in this video.

https://youtu.be/RtTKuqkpGdM

I can't wait to use my new rotary cnc machine. Just need proper g code.
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby martin54 » Sat Jan 19, 2019 1:49 am

Are you using the correct post processor? there are 2 pp one for wrapping x & one for wrapping y, sounds like you have selected the wrong one :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 4692
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Rotary tool path output is wrong.

Postby Rcnewcomb » Sat Jan 19, 2019 1:59 am

If your rotary is parallel to the X then you need to wrap the Y values. The X movements stay the same. It is the Y movements that need to be translated into rotary movements. Change the post processor to wrap Y.
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3659
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Rotary tool path output is wrong.

Postby PhilJohnson » Sat Jan 19, 2019 4:01 pm

Rcnewcomb wrote:If your rotary is parallel to the X then you need to wrap the Y values. The X movements stay the same. It is the Y movements that need to be translated into rotary movements. Change the post processor to wrap Y.


Correct

What I'm saying is that there IS a glitch that is not allowing you to use the correct post processor.

Along X axis job setup should = wrap Y
Along Y axis job setup should = wrap X

The glitch is it not allowing you to use the correct wrap post processor. If it's not correct, the rotary output box doesn't pop up.

This was a job set up along X. It will currently not pop up this box unless you select a wrap x, which is wrong.

This glitch may be in desktop only.

If you notice also, its saying wrapped around the cylinder 5xx degrees. Which even says that for just a blank cylinder. It should be 360°
Attachments
20190118_202531.jpg
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby PhilJohnson » Sat Jan 19, 2019 4:09 pm

martin54 wrote:Are you using the correct post processor? there are 2 pp one for wrapping x & one for wrapping y, sounds like you have selected the wrong one :lol: :lol:


Nope. I spent 4 hours on this straight. This is a glitch in vcarve desktop.
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby PhilJohnson » Sat Jan 19, 2019 4:50 pm

I just tried every single wrap y-axis post processor there was with all the same results. It is not allowing you to use the correct direction rap post processor in V carve desktop 9.5. I will be upgrading to pro and hopefully the glitch is not there.

I am uploading a better video showing exactly the issue or explaining it better. I will post the link when it's Uploaded.
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby PhilJohnson » Sat Jan 19, 2019 4:59 pm

Heres the better video

https://youtu.be/seWeywTkS-8
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby Rcnewcomb » Sat Jan 19, 2019 8:53 pm

You want to use the Wrap Y values post processor. If you could Zip and upload your rotary post processors that would be helpful

If things are working correctly you should NOT see the Wrapped Output dialog box. That dialog box is a holdover from older versions.

If you want the Y values to be changed to A axis moves then your post processor file should have:
ROTARY_WRAP_Y = "A"
or more likely
ROTARY_WRAP_Y = "-A"
depending on your machine setup. A partial example of machine moves would be"
Code: Select all
N220 G00 X1.0000 A-36.7606 Z1.2000
N230 G1 X1.0000 A-36.7606 Z0.9000 F120.0
N240 G1 X1.0000 A-323.2394 Z0.9000
N250 G1 X11.0000 A-323.2394 Z0.9000
N260 G1 X11.0000 A-36.7606 Z0.9000
N270 G1 X1.0000 A-36.7606 Z0.9000
N280 G00 X1.0000 A-36.7606 Z1.2000



Likewise if you want the Y moves translated to the B axis you would have
ROTARY_WRAP_Y = "B"

Some people disconnect the Y axis and connect it to the rotary motor because their control box only has support for 3 axes. If this is the case then you would use:
ROTARY_WRAP_Y = "yes"

Example output is:
Code: Select all
N220 G00 X1.0000 Y36.7606 Z1.2000
N230 G1 X1.0000 Y36.7606 Z0.9000 F120.0
N240 G1 X1.0000 Y323.2394 Z0.9000
N250 G1 X11.0000 Y323.2394 Z0.9000
N260 G1 X11.0000 Y36.7606 Z0.9000
N270 G1 X1.0000 Y36.7606 Z0.9000
N280 G00 X1.0000 Y36.7606 Z1.2000


Notice how the Y moves are all in degrees.


I've always written my own rotary post-processor, but I did look at some that were in the Post P/05 Wrapped folders and frankly, some of those post processors are wrong.
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3659
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Rotary tool path output is wrong.

Postby PhilJohnson » Sun Jan 20, 2019 9:29 pm

I figured it all out.
PhilJohnson
 
Posts: 25
Joined: Wed Nov 16, 2016 4:48 pm
Model of CNC Machine: X-carve

Re: Rotary tool path output is wrong.

Postby mtylerfl » Sun Jan 20, 2019 10:25 pm

PhilJohnson wrote:I figured it all out.


Did you have to do anything special or was the software correct after all?
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 4283
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Rotary tool path output is wrong.

Postby gregk » Mon Jan 21, 2019 10:47 am

In version 9.5 we have introduced direct support for rotary jobs. If correct post-processor is selected in rotary job (i.e. matching the orientation) the "Wrapped Output" dialog is not displayed anymore.
This is intended since the necessary information was provided when setting up the job.

If the orientation of the post-processor does not match that of a rotary job, or when rotary post-processor is selected for single-sided job, "Wrapped Output" will be shown to confirm the user's choice.

Greg K
gregk
Vectric Staff
 
Posts: 78
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None


Return to VCarve - General

Who is online

Users browsing this forum: hooby, jstur23 and 27 guests