Jerky movement with UCCNC

[Heiko]

Hi,
I own a UC300ETH and recently switched from Mach3 to UCCNC. First of all, I like UCCNC very much. It is very user friendly and I want to continue using it.
A few days ago I made the first attempts with UCCNC and some basic settings. The movement is very jerky and the processing takes a long time.
I never had such problems with Mach3 and the UB1 profile from CNC-Room.
In the manual I found the general settings and tried some values but it did not get much better.
I found this thread and converted Gerry's values to millimeters:

https://www.forum.cncdrive.com/viewtopic.php?t=356

Linear Error max – 0.125
Linear Addition Length – 1,25
Linear Unify Length – 2,5
Corner Error Max – 0,125

Because I have not received any improvement, I tested the values in the range of 0.01; 0.1; 1 in different combinations. So far I have not found a good solution.

Here is a short low quality video of the parameters(from 30 seconds):
https://youtu.be/y2ygF4qbpVw

On the video that looks very unspectacular. But you can clearly see and feel the accelerations and vibrations when standing next to the machine
Could someone please give me some more tips on how to optimize the movement? I think that the parameters are not machine dependent?

One more thing, sometimes the text box with the NC code jumps back to Line 1 during the cycle. The movement will continue but it looks scary. Is that OK?
https://youtu.be/SsfZcq99lso

I also tried to use Mach3. It tells me that the firmware is different. Can I update the firmware via Mach3 and still use UCCNC later again?

Thanks. I hope these are not too many stupid questions.

best regards

[cncdrive]

You can make the tolerance parameters higher.
You can also make your accelerations higher.

Mach3 can execute those type of motions fast, because:

1.) It has no path deviation control and so it erases as much details from the path as it thinks is fine. This means that you can only guess about your tolerances, but in exchange the movements will be fast, because it cuts off paths.
2.) Mach3 overrides your acceleration settings, we have measured up to 8x the set value. This means that you likely down-tuned your axes acceleration parameters to not loose steps with Mach3 and so if you using the same acceleration settings with the UCCNC then it will finish slower and it will make movements more jerky, because the UCCNC will obey your acceleration settings.
This also means that with the UCCNC you can use higher acceleration than you could with Mach3 and you will still not loose steps and so the overal performance will be higher, you just have to higher the acceleration parameter.

Yes, that jumping of the line ID to the first line in version 1.2049 is a known issue, it is a visual glitch.
The issue does not exist in later versions. Try version 1.2109, it is proven to be pretty stabile by now.

Our mach3 plugin and the UCCNC updates the firmware when and if needed automatically, you can connect to any of the softwares any time, the firmware update will happen automatically when it is required, the softwares check that and update when needed...

[mgt]

Is that a fusion 360 toolpath? I've had similar issues using the smoothing option when doing adaptive clearing. Even if i'm very generous with my acceleration and CV settings it runs jerky.

[Derek]

I've found that the trick to smoothing out the movement is to keep reducing your feed rate until the motion smooths. UCCNC likes a lot of acceleration in order to blend the moves. The feed rate that you end up with is the maximum you machine can cut with continuous motion. I can cut an arc with smooth movement at 80 IPM. Break that arc into line segments and I have to reduce the feed to about 55 IPM. I have yet to find a combination of tolerance settings that will provide smooth motion. 3D files are just brutal. It is accurate though:)

[Heiko]

Hi,

Thanks for the answer. I will continue to work on the parameters. The acceleration is currently set very low. Certainly I can increase this a bit.

I now understand why Mach3 runs so smoothly. In fact, the corners were a bit round with Mach3. Since I use UCCNC these are totally sharp with the tested parameters. But round corners were not a problem for me.
I use Solidcam iMachining. I think it's very similar to Fusion adaptive clearing. The NC code contains many short segments with varying feed rates. But I would like to continue using this strategy because I can work very effectively with it. I hope to find a suitable setup for UCCNC.
Reducing the feed rate is certainly a possibility. But I would like to keep my settings.

Of course I am open to any suggestions to optimize the Motion. If I find good settings, I will post it here.

[ger21]

The acceleration is currently set very low

That's likely the biggest problem. The higher the accel, the smoother it'll run.

[Heiko]

Today I made a few more attempts. I have increased the acceleration from 400 mm/s ^2 to 1000 mm/s^2. The program was faster but the movement was still very jerky.

Then I told the CAM to use lines instead of arcs. It seems like the problem is solved. The movement was much smoother and a change in the general settings had a direct effect on the movement. Honestly, I could hardly achieve any change with the settings before.

Certainly I can still optimize the parameters. Now I can do a fine-tuning.


Are these findings plausible or already known? I hope I have not bored you with it.
I thought it would be better to use arcs instead of lines. But maybe UCCNC can not work with those very small arcs?

Thanks to all.

[cncdrive]

Small arcs are more troublesome than small lines, because with lines the software can basically even skip the line with optimising it out in the CV panner, but it can't do that with arcs, because in an arc the movement vector direction is not constant, so it can't just skip an arc to make the path smoother like how it can with a line if it is very small, unless if it is smaller than the tolerance. So, with codes like that it is better to use lines.
We have plans how to further optimise the path planner to make this to work better, but ofcourse it will be never perfect, it can't work perfect unfortunately, the world is not perfect. Compromises have to be done.

[mgt]

Heiko. Removing arcs, turning off smoothing, in fusion 360 did the trick for me as well.

Per

[Beardie7]

Heiko. Removing arcs, turning off smoothing, in fusion 360 did the trick for me as well.

Per

Where are you actually turning off the smoothing feature? In Fusion 360 or in UCCNC? Same with Removing arcs?

I'm just getting started and trying to get a reasonable starting point for my velocity and acceleration. I have 637 oz/in Nema 34's with a 2.2kw spindle in a "Joe's design EVO"

I just did my first real cut of a project with 180 IPM with 1/4" bit 3 flute bit and the sweeps have noticeable flat spots. It was cutting pine and went trough it like butter with .25" depth of cut. All of the general settings were left alone (angle stop 89, L 300, LE .03, LALM 1, LULM 2, CEM .03, and ART .1)

My axis' are running with 400 inches/s, and 40 "/s/s (comp accel at 60- I don't know what comp. Accel is though)

The plan is cut out of walnut so I know that I need to slow it down some. I was using the Vortex Tool app to get the feedrate. I know that feeds and speeds it dependent on so many variables so I was using the app as a guide. Again it cut well but had a more segmented look than I was expecting.