[Fyresparxx]

We have an EZCutCNC 8000 series plasma table, and we've been very happy with it for over a year. https://www.ezcutcnc.com/plasma-table-photo-gallery/

All of a sudden a couple months ago I started getting really bad jitter in my cuts. I've cleaned everything thoroughly, I've squared the gantry, I've verified that it has nothing to do with the torch (happens with a sharpie too). Every cut made with a G01 Command jitters when it changes direction even slightly, leaving chewed out edges when moving at 200ipm and above (14gauge and thinner). It isn't noticeable at 95ipm (11 gauge). I can make nice smooth cuts with G02 and G03, but if I recreate the arc with G01 commands, even with high segmentation, I get jitter, as if it's pausing for a moment at each corner.

Like I said, it's a new problem, and the table has been behaving properly for over a year before this, so I want to say it isn't user error.


I couldn't edit my original thread title to reflect my continued issue.
Originally we were told that my problem could be caused by the machine being out of square. We have since squared the machine exactly, but the problem persists.
Previous thread: http://www.cnczone.com/forums/genera...ne-square.html

[Jim Dawson]

Is it possible that a setting has been changed in the G-code in the CAM software, maybe G61 (Exact Stop), vs. G64 (Constant Velocity) ? Or maybe an equivalent setting in the controller?

[Fyresparxx]

Just letting CAM generate a shape:

G20
M106
G00 X Y
G603
G03 X Y I J F
G01 X Y (many lines worth)
G00 X Y
G603
G01 X Y repeat

I only started learning G-Code recently, I've mostly just let the CAM program do the work. We bought this machine and I ended up being the one to learn to use it. I don't know what G603 means. All the charts I have end at G99. The manual that EZCutCNC gave me mentions a "Programming Reference Manual" But it doesn't seem to exist. Manually inputting a G61 or G64 command results in "An unrecognized command was encountered" error.

I don't know how it could have changed overnight though. I didn't do any upgrades, updates, or settings changes and, as far as I know, everyone else is too afraid of computers to even think about messing with settings or code.

[Jim Dawson]

I have never seen a G603 either. The only reference to G603 I can find is on page 13 of the following document, not sure exactly what it does, but it seems to control Exact Stop mode.

http://www.m3.tuc.gr/EQUIPMENT/CTX310/840D%20G-CODE.pdf

Maybe try changing the G603 to G600, or some other combination and see what happens.

[Fyresparxx]

Apparently, I'm missing about 5 different documents from the manufacturer that might help clear this up. In the mean time, I found a setting in the software that says it always runs in "Continuous Contouring Mode" where it seemingly decides line by line whether to use G61 or G64 based on the current speed vs the change in motor speed required to execute the movement? I turned this tolerance up until I was worried about losing steps, and then turned it back down about 30% for safe measure. It seems to have improved the cut quality a lot, so your suggestion may have hit the nail on the head. I still don't know how anything could have changed overnight, but I'll be happy with having a useable machine.

[Jim Dawson]

I hope it works out for you.

[Torchhead]

The biggest problem you have is the artwork is segmented and all the arcs are being output as G01 moves (straight lines) . If CV is not turned on and/or you have the wrong settings in the CV settings then the toolpath will not be blended and you get herky jerky motion. I don't know what CAM you are using so I can't comment on how it handlers things like DXF imports but typically bad drawings end up with bad motion. I don't think its a setting in MACH although you can mess around and get it to do different things but its trying to cover up the base problem. If the settings have not changed then its not logical they suddenly need to be changed at some magic point in time. Of course MACH can be dinked with . You might check the xmlBackups folder under MACH2 and see how many numbered profiles of that same name are shown. Anytime you make a change in MACH it saves a copy of the XML and numbers it progressively. That would show you a trail if someone made changes tot he factory settings. The XML has 99% of all the settings for MACH and you can change its whole behaviour by picking a different Profile.

Its interesting that the code shows one G03 (arc) and the rest are all G01 (straight lines) .That looks like maybe the leadin is a true arc and the other curves are all segmented lines. That should still run pretty smooth if the beginning and end points of each line is lined up with the next but it takes CV being turned on to blend those lines together.

Have you tried cutting something that cut fine before?

Does it cut angled lines ragged?

Its Really hard to make a machine cut those scallops unless there is something mechanical or dramatically wrong with the cut file.