UC300ETH skipping G-code (G3 - full circles)

If you think you've found a bug post it here.

Re: UC300ETH skipping G-code (G3 - full circles)

Postby Robertspark » Fri Sep 28, 2018 5:17 pm

Balazs, thanks for taking the time to reply.

Ok, I understand that, but if I round all my gcode off to two decimal places with the post processor there will never be a situation where the start point does not correspond with a whole step value if my settings are 100 steps per unit.

G1 x0.01 f500
G4 P1
G2 x0.01 Y0 i10 y-10

If I feed the machine 2 decimal place information and it is set to 2 decimal place precision then it will never have a problem.

When would the last move ever land on 0.005? For example

I understand the problem with imperial machines is if lets say you have a 4 turns per inch ball screw, direct drive, so potentially your steps per unit (maximum {no microstepping mutiple}) are 4*200 = 800 steps per unit, so the smallest step is 0.00125.... now I have a rounding error if I send the machine to

G1 x0.001 F100
G4 P1
G2 X0.001Y0 I5 J-5

Because X0.001 does not exist for the machine
Only X0, and X.00125

One simple way to fix this is use 10uStep setting on the drive.... So now the smallest step is 0.000125..... now X0.001 exists... because there are now 8 steps from
X0 to X0.001..... so to fix this problem make sure your machine only exports gcode from the post processor with 3 decimal point precision
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby cncdrive » Fri Sep 28, 2018 9:25 pm

Yes, but what if in your drawing the circle is a littlebit off from e.g. X0.01, it is drawn to for example 0.01001, then the same issue can happen.
Noone can guarantee that the drawings which you will use to generate the g-code are always drawn perfectly.
Ofcourse with hand coding it is different, but most people do not code with hand nowadays, but using somekind of CAM software and CAD drawings.

And if you make the CAM software to output only 2 decimal places will make some error on the toolpath. If it is a problem or not I don't know, depends on the job tolerance requirements...

So, the proper solutions for this issue are what I told in my previous post.
cncdrive
Site Admin
 
Posts: 4695
Joined: Tue Aug 12, 2014 11:17 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby Robertspark » Sat Sep 29, 2018 9:13 am

I've asked a question on the sheetcam forum here
https://forum.sheetcam.com/viewtopic.ph ... 092#p25092

I am not aware of a simple setting in sheetcam which can split circles in half / quadrants. I can see a way to do it in the post processor for sheet am, but that is a little more complex in my opinion and I thought I'd ask to see if I missed a simple setting.

I am aware that vectric aspire apparently by default outputs arc motion in quadrants so there will be no skipped circles there.

I can see this being a problem with imperial setup machines that use non round number steps per unit settings.

I know I've had the problem a couple of times with mach3 (when I used it) but thought it was just a missfire or mach3 quirk.

Would the original poster mind posting the gcode file (or part of) and your machine setup (steps per unit for the axis) please, thanks
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby cncdrive » Sat Sep 29, 2018 11:22 am

Hmm, I thought it can split the arcs, but maybe it was really vectric and I remember incorrectly, I'm not 100% sure now.

Yes, it is not a Mach3 issue, but it is a mathematical/g-code representation issue which issue appears when the controller have to syncronise the coordinates to the real values which is not a mach3 specific things, but no controller can work without doing that.

Yes, seeing the g-code of the poster would be useful to see if the issue is really what I described, but I'm 99% sure it is.
cncdrive
Site Admin
 
Posts: 4695
Joined: Tue Aug 12, 2014 11:17 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby Robertspark » Sun Sep 30, 2018 7:27 am

For sheetca, the solution may be (not tried it yet) to edit the post processor
Code: Select all
 Options->machine->post processor. Click on the 'edit post' button.
Add this as the first line of the post:
post.SetOptions(post.ARC_SEGMENTS)


As given in the sheetcam forum question i posted with a link in one of my earlier posts
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby jawneelogik » Tue Oct 02, 2018 9:08 pm

Sorry for the delay in responding, but as I indicted in one of my previous posts, I was out on the road at the time. I am now back home and have access to the machine and the files.

First off, the steps per unit (inches) is: 1016.67
My microsteps per step is fixed at 10 by the G540 (this allows for only about 15% of the total torque/holding power.)

I also had a look at the gcode and now see that, yes indeed, there is a call to M205 inserted right between the initial G3 call and the XYIJ coordinates for the remainder of the circle. If that is a problem then I can resolve it because I have also determined that I don't want THC on for any part of the hole anyway. I will be revisiting my Sheetcam path rules to make some adjustments.

However, having said that, I was under the impression that this whole issue had been resolved with the advent of UCCNC. In fact, you make reference to it twice in the previous thread. http://www.forum.cncdrive.com/viewtopic.php?t=1195
where you say:
cncdrive wrote:We have checked this problem today.
The issue is the same what was also a problem in the UCCNC for some time, but we managed to correct this issue recently in the UCCNC.
The problem is that with Mach3 we have no access to the source code and the issue is so complicated that so far we could not figure out a way to fix this problem, however we know about this problem for some time now and have tried to fix it already.

Then further down:
cncdrive wrote:..... As I said the same issue was already fixed in the UCCNC, but in Mach3 it is much harder, because we have no access to the source code and we can only work with it's public interface which is complex and also is limited in many ways.


The two different code files are attached. One of them is a multi-part nested job where holes were skipped in a consistent pattern. The other is a single part, but cut multiple times where I changed the angle of the Lead-in to be on a diagonal instead of perpendicular after which, the hole was not skipped. ???

Any ideas?
John
Attachments
p1 times 30.tap
(77.06 KiB) Downloaded 782 times
M520 modified lead-in.tap
(1.69 KiB) Downloaded 801 times
John L.

UC300ETH, UCCNC 1.2106, Gecko G540
Hypertherm Powermax85
jawneelogik
 
Posts: 5
Joined: Tue Sep 25, 2018 6:57 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby cncdrive » Tue Oct 02, 2018 9:14 pm

However, having said that, I was under the impression that this whole issue had been resolved with the advent of UCCNC. In fact, you make reference to it twice in the previous thread. viewtopic.php?t=1195
where you say:


That was a different problem.
The issue you talking about or at least what I'm think and was talking about is unresolvable.
But I will test your code tomorrow to see if I'm right about the reason for the issue or if it is something different.
cncdrive
Site Admin
 
Posts: 4695
Joined: Tue Aug 12, 2014 11:17 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby cncdrive » Tue Oct 02, 2018 9:16 pm

Please post your profile file too, because it will help me to reproduce the issue here.
cncdrive
Site Admin
 
Posts: 4695
Joined: Tue Aug 12, 2014 11:17 pm

Re: UC300ETH skipping G-code (G3 - full circles)

Postby jawneelogik » Fri Oct 05, 2018 10:03 pm

Again, I apologize for the delay. Here is my profile as requested.

John
Attachments
Plasma.pro
(34.25 KiB) Downloaded 814 times
John L.

UC300ETH, UCCNC 1.2106, Gecko G540
Hypertherm Powermax85
jawneelogik
 
Posts: 5
Joined: Tue Sep 25, 2018 6:57 pm

Previous

Return to Report a bug

Who is online

Users browsing this forum: No registered users and 10 guests

cron