forum.cncdrive.com

Hello All,

I find myself having a problem with UCCNC, runnin a program in Mach3, all is fine and smooth, but runnin the same file in UCCNC, the machine behave's jerky or better with hesitations.

I tested out different settings in the constant velocity, but that seems no solution at all.

https://youtu.be/mJHfGOqpOSk


https://youtu.be/qA6mF9IGf2Q

Anyone got an idea? i'm out of it.

Regards Simon

http://www.cncdrive.com/UCCNC/UCCNC_usersmanual.pdf

read + reread pdf pages 33-35

corner error max

The main issue here is that Mach3 has no error tolerance setting. So it will happily run as fast as you want, with no regard at all for how close it follows the commanded path.

With UCCNC, it will follow the path as close as you tell it to. In order to get it to run like Mach3, you likely need to increase the error tolerance settings much more than you think.

Hello, Ger21,

When i set these valeu's to high, the software makes itself a whole new path, which is way of the drawing line, i other words it produces a whole new drawing, thats the way i see it.

Maybe i see it wrong, or read it wrong (english is not my native)

I will try out the corner error setting

Simon

I'm sorry to hear you are having issues with UCCNC.
I moved from Mach 3 because of the jerky movements and UCCNC has been fantastic for me. One thing to be aware of is the GCODE that was produced for Mach 3 from your CAM software, one needs to make sure the CAM software outputs the GCODE for UCCNC ie the POST PROCESSOR needs to match. I made that mistake and thought that the GCODE was compatible exactly and it is not. I was using Inventor at the time but now have switched to Fusion 360 and my machine just runs better with Fusion 360. Again it is all in the post processor.
I recently did a job that had 585,000 lines of code and it ran flawlessly.

Yes, the CV tolerance parameters tells the software how far it can go off the path to possibly run faster.
You should only set the tolerances as high as what your application/workpiece allows.
But if you setting the CV tolerance too low then the machine has to follow the toolpath too stricktly and so then it will have no room to save time and the lots of sharp accelerations/deccelerations can cause jerky movements.

You can also try to higher the acceleration parameter of the axes. The UCCNC can run the machine safely with higher accelerations than mach3.

Well in my opinion, i've tried about everything in settings, and i cant get t anywhere near smooth. I did attach an NC file, maybe some of you could find a fault in there. (in mach it runs OK)

Machine runs with a 300eth controller, windows 10, leadshine motors and drivers.
Did try all different settings on cv mode, with various accelerations form 50 to 500 (500 feeling like a bullet start) and also different kernel speeds. total speed of the machine is at 2500 U/pmin (that is metric units)

I do like this program, this is the only thing i dislike about it, and still maybe its just me...

Regards,
Simon

I tried your file in simulation mode in my default UCCNC install, and I got the same issue.

I thought maybe your file was bad so I converted your gcode to DXF and took a look at it in Coreldraw. Quite a few lines instead of arcs, and nodes close together causing very small zig zags in the path.

So changed all lines to curves and greatly reduced the number of nodes. Got all the paths looking smooth and curvy, no straight lines.

Exported to DXF and generated new gcode with Sheetcam. Tried a new run in UCCNC and lo and behold still the same problem with apparent pauses in motion. I remember having an issue like this before and it was my acceleration settings.
Upped my axis acceleration settings to the max my steppers can handle without losing steps and the motion become smooth and fluid.

Could that be your issue.

I even tried your original gcode with the less than ideal path and the zig zags and it also seemed to run fine.