CV Settings OK?

[sngatlanta]

We're having an issue with repeatability and are also noticing cater or jerky during arc motions. We have tried many setting adjustments and have improved some but just cant get over the hurdle here.
I have installed the latest release 1.2101
We use Ger21's Screenset 2017.
Our CV settings which are in inch setting as that is what we use.
CV is checked
Exact Stop at Angles: 89
Maximum Corner Error: 0.001
Maximum Linear Error: 0.001
Maximum Linear Addition Length: 0.03
Maximum Linear Unify Length: 0.05


Anyone see something wrong or have advice?

Thanks,
Greg

[cncdrive]

Repetability has nothing to do with CV settings, but your machine may have a mechanical or electrical problem that it looses steps or it has a backlash or both.

[sngatlanta]

I didn't mean to mix the two issues as one. Sorry. My question here is only about the CV settings and the jittering in the arcs. Do the numbers I posted look correct or do you see something that may improve smootness in arcs?

[cncdrive]

It's hard to tell if the values are OK for your job or not without knowing what are the requirements of the job.
What I can tell you is what those settings mean, however they are probably better documented in the UCCNC manual:

1.) Stop at angle means that the machine will deccelerate and stop and accelerate up again on any connection points on the path where the connection angle is greater 89°,
so basicly anything which connects a bit less of a square will make the machine to deccelerate.

2.) The Maximum corner error means that the machine can make a maximum of 0.001 error off the connection corners.

3.) The linear error means that when lines are unified then they get unified if the error between the new path is lower than the 0.001 value. So, the unification of the looking ahead stops when the error becomes larger and the machine deccelerates to that point.

4.) Maximum addition length means that the software can add a maximum of this line length to the unification when it is looking ahead. If the line is longer then the software is not allowed to unify it and so it has to deccelerate to that point.

5.) Maximum unify length means that lines upto this total length can be added (unified) together in one look ahead round. If the total is longer then the machine deccelerates to that point.

Generally speaking the larger the error parameters the less smooth the workpiece will be in most cases, especially if talking about arcs and paths which have lots of direction changes. However the same time the faster the execution will go especially with paths where there are lots of direction changes, because the lower tolerance means that the software has to follow the path closer and the higher tolerance means it has more freedom to optimise the path for speedy execution.

And the larger the addition and unify lengths are the motion will be less jerky, because the software is allowed to unify longer lines and longer total length of lines together.

[ger21]

Are they really arcs, or arcs made up of straight segments?

Try setting the maximum corner and linear errors a bit higher, between .003-.005.

And the linear Addition and Unify to 0.25.


It'll take some trial and error to find out what works best for your machine.

[sngatlanta]

We have a test file produced in Vcarve Pro we're using to try and get things better, it contains 2 circles, one about 10" in dia and another about 25". as you know the circles produced in vcarve are divided into 4 arcs. The biggest issue with those is as it gets to the 12,3,6,9 o'clock position there is a jump. On that same file an ellipses with a square leg on one side. Not sure how that is handled by vcarve. I assume its much smaller segments.

I'll try the suggestions and see if it improves.

Thanks,
Greg

[sngatlanta]

Gerry,
Thanks for the tips. I think we have improved the smoothness somewhat but still need to fine tune it.

I see on your screenset requirements you don't recommend the test version of uccnc over 1.21. I had installed it just the other day before reading that. Is there anything in particular I might watch for? How far out is your next update?


Greg

[ger21]

I see on your screenset requirements you don't recommend the test version of uccnc over 1.21.

There are quite a few checkboxes and buttons in the 1.21 version that are not in the 2017 screenset. There's a possibility that this could cause some issues. I don't think that you'll have any issues with it, but I don't know for sure.
You should be OK to use it. If you run across anything that appears to be not working correctly, shoot me an email and I'll look into it.

The one issue I know of, is that if you change the color of the toolpath boundaries, it will turn them off, with no way to turn them back on.

Some time this week I'll be sending out new probing macros, as there's an issue with number formatting which can cause a crash in some cases. It's only been reported by one person, though.

The updates screen will be completely new, and will probably take me a few months to get finished. I have to redo the graphics on almost every page, to accommodate all of the new features in UCCNC.

[sngatlanta]

We are still having issues with arcs connected to linier items. For lack of a better definition lets call it a hard slamming when coming to these turns. I am far from an expert and must turn to those that are. I have read a lot of info on this forum and find similar issues but no definitive answer. I have read the manual. I must be missing something in my settings or my machine is just no good. No one here can judge the machine I understand and belive me I digging deep into that.

So let me reach out again for answers.

Does the acceleration setting also apply to deceleration rate when coming up to these problem areas?

If someone can explain how I would attach a sample file.

NOTE: We use V Carve Pro for toolpaths and generating our cutting files.

[cncdrive]

Acceleration value is the same as decceleration value is why there is no separate decceleration parameter.
The UCCNC will never accelerate or deccelerate faster than what you have setup the acceleration parameter to.
The acceleration is always the limit for how fast the machine will accelerate up the axes and deccelerate them down,
except when safety events happen (e-stop/reset/limit switch triggers) then the axes are instantly stopped.

If the machine is with steppers then the only way the axis can accelerate or deccelerate faster than you want it to is if the acceleration parameter is too high for the machine to handle.
The acceleration is then still correct, it's maximum value is always what you have setup as the acceleration parameter, but your machine might not be able to mechanically handle it.

One more thing is if you have backlash setup then when the backlash is compensated then the comp.accel parameter is used which can be set higher than the normal acceleration parameter.
So, if you have the backlash enabled then you should check that parameter also.

You can attach files to forum posts with certain file extensions only. You can for example attach .txt files, just rename the file extension to .txt and upload it.