Tuning CV Settings - my amateur findings - to discuss!

[AvB]

Hi people - I have already posted this but mistakenly put it in the ToolBox section, so I'm reposting it here where it belongs. When I first installed UCCNC, after changing from Mach3, the Constant Velocity settings I initially set were too tight, and the machine operated as if in Exact Stop. I had problems and got some basic advice but felt like I really had no idea what I was doing.

After writing all this stuff (below) I found that there's a recent thread where Matej had similar problems discussed, and it contains some very good info from Balazs and Robert which is helping me to understand it better.

I'm going to repost my "report" and then below I'm going to ask some questions that relate to the info in Matej's thread. Thanks for reading and I really appreciate any information ... remembering that I'm not any expert at CNC, machine setup or programming. So aim your feedback at learner level!

My machine is a fairly heavy solid rigid mill with servos and ball screws/ linear rails. I run maximum velocities of around 3500 mm/min on X and Y axis and around 2000 on Z. My accelerations are currently 200 mm/sec/sec on X and Y (more on this below).

I mostly make model aircraft moulds which involve a lot of 3D work (and various bits of 2 1/2D) and I am after very high accuracy but also smooth and reasonably fast cutting. I want the mould surface finishes (wing foil shapes) to be very smooth and accurate, and the edges and curves to be accurate and the corners sharp.

The CV settings available are:
Stop at Angle Degrees (I use 75°)
Look ahead Lines Count (I use 300)
Maximum Corner Error (MCE)
Maximum Linear Error = (MLE)
Max Linear Addition Length = (MLAL)
Max Linear Unify Length = (MLUL)

I found it difficult (and still do) to work out what the best settings are for the last 4 parameters. The manual is very comprehensive and explains the system well, but it doesn’t help you to work out how to tune the settings. It would be good to have some more information such as:
1) A guide to starting points for each of the 4 parameters, and
2) Tips on the effects of increasing or tightening each of the parameters.

To get straight to the point, I have settled on using the following with good results:
MCE 0.1
MLE 0.05
MLAL 10
MLUL 25

The following settings were way too tight and caused the machine to run very jerkily, almost like Exact Stop at times:
MCE 0.01
MLE 0.01
MLAL 5
MLUL 10

The following settings were reasonable, but made the machine run too slowly on long cuts as it tended to hesitate at various points.
MCE 0.05
MLE 0.02
MLAL 3
MLUL 5

This was way too loose and caused really major rounding of corners - I used a 1mm cutter following a zigzag line and it turned it into curves!
MCE 1.0
MLE 1.0
MLAL 10
MLUL 25

A couple of months ago I did quite a lot of tests, running a custom made 3D test cut into acrylic material. It contained features my typical shaped cuts, like a "leading edge step onto flange" in both directions as well as squarer steps that were inside the CV angle so CV was active. I ran about 20 of these test cuts varying each of the CV settings up and down and taking notes on the results, until I was happy with the speed as well as the smoothness of the 3D face and the sharpness of the corner edges. So I was able to objectively choose settings that seemed to give the desired results without being too tight.

After that, doing a couple of small 2D jobs for a while, I kept getting concerned about getting maximum accuracy and I progressively tightened up the settings again bit by bit. But just the other day, cutting another set of 3D wing moulds it was clear that the cuts were much slower than usual with lots of hesitation along the path. The machine travelled much slower than the velocity specified in the feed rate. I finished the job with those settings but I didn't like the hesitation and mild jerkiness and the cuts took too long. So I created another test cut section (a small section of the wing I had been cutting), and ended up putting the settings back to the previously selected numbers in bold above.

These are just some observations, mostly subjective, that I made when playing with the settings:

Increasing MCE as high as 1.0 didn’t have a lot of effect, but increasing MLE to 1.0 caused some rounding of sharp corners (on Z based steps) and it seemed to be necessary to have MLE at or below 0.05 to get sharpness.

Reducing MCE and MLE didn’t seem to slow the cuts badly, but reducing MLAL and MLUL too much did cause slower more hesitant cutting.

When the settings were a bit too tight and the cuts slower and hesitant, at the following settings:
MCE 0.05
MLE 0.02
MLAL 3
MLUL 5
... I found that doubling MCE made no difference to speed and smoothness. Doubling MLE made no difference. Increasing MLAL from 3 to 10 made the cutting clearly smoother (smoothing out the hesitations), but not faster overall. Tripling MLUL still resulted in the hesitations, but the cutter moved faster in between each slow-down, and the overall speed was higher. Increasing MLAL and MLUL together to 10 and 25 respectively was both smoother and faster. But my final current settings were even faster and smoother again. Note: in the above tests, only one parameter was changed, then returned to original before the next parameter was changed. I also timed the cuts from start to finish to measure the overall speed. That test cut involved a period of parallel finish cutting in a 3D shape for nearly 2 minutes so time differences were quite clear.

ACCELERATION is another factor to consider in the overall CV equation. My accels were all at 180mm/sec/sec and I was advised that this was very slow, and back when I was doing my first tests, Gerry advised that I should increase my acceleration a lot to get better sharper results. Yes, this was true - when increasing accel from 180 to 300, settings which previously had minor rounding were clearly sharper. But unfortunately my gantry jolts quite hard at a Y accel of 300 and I wasn’t comfortable with how hard it was working the machine, so I have reduced the accels back to around 200 - 220, which is definitely smoother.

[AvB]

So now having read Matej's thread, I have got some answers but also some questions.

Robert gave this advice:

Stepping back a bit to understand the Corner Error max.

What you are telling the machine to do is if you have a feedrate of 3000mm/min and a corner error max of say 4.2mm, the machine is allowed to round the junction of two linear moves with a radius of 4.2mm without slowing down

So if you have a tool with say a diameter of 8.4mm then this setting will do nothing to reduce the accuracy of the component finish because the radius is equal to / smaller than the corner error max setting. So the motion should be offset 4.2mm from the intended finishing cut line anyway.

OK, that's great info and I can use that to tune the CV corner error setting to suit the cutter size for its XY moves. But how does this work in 3D stuff where a small square end mill is following a shape and has to lift and drop over angles? I'm assuming that the same corner error setting will apply to ZX and ZY paths? In those cases, the square end mill doesn't use a radius to make a corner. If I set a corner error low enough to get the Z corners sharp, won't that then make all the XY moves slow?

[AvB]

Also Robert, you said:

What you are telling the machine to do is if you have a feedrate of 3000mm/min and a corner error max of say 4.2mm, the machine is allowed to round the junction of two linear moves with a radius of 4.2mm without slowing down

Is this correct? I thought that the machine still slows down to some extent, but the CV function means that the fastest, shortest path which is within the corner error parameter is chosen.

[AvB]

Also I have not considered arc radius tolerance in the above discussion. I am using Gerry's screenset and the parameter is on a different page to the CV settings so I've been ignoring it.

I have read the manual carefully about arc radius tolerance and although I can understand the words, I can't work out the practical application of how I would choose a setting to suit my needs. Can someone give a basic explanation of how to decide on arc radius tolerance, and what effects will occur if it's too loose or too tight?

Thanks,
Andrew

[rmat]

Hi, looks like Im not the only one fighting CV.
I can not understand it anymore, it behaves so strange. I have found some spot that im comfortable with now, but I really cannot understand CV logic in UCCNC.
I have some job that I have mill some 200 different plastic pieces, and is actualy getting funny, some code just runs trough and other is jerking. I use arc and in fact force them so the controller runs smooth. If you use points its no matter what you do, you cannot combine smooth motion and accuracy with UCCNC.
I really dont even know why the hell is the CV angle there, and also the look ahead lines, as software is clearly not obeying it. I have just cutted something, and the arc was very small, like 5 degree angle. So guess what the machine did. Exact stop at start of the arc and another one at the end of the arc. Just ridicolous.
So Ive abanded trying to figure this out for the sake of my sanity and will wait for new motion planner. I have bought also eding controller, just in case I dont get too old waiting on the new planner, but in the mean time at least I can work now, its nowere near what I like, but it does the job.

Just to clarify my specific problem, I have somewhat fast machine and very rigid machine and want&can cut very fast, with right paths and approach I can mill with 12000mm/min in 3d and even faster in 2D and accelerations of 1500mm/s2. But for this I need smooth motion, witch I cannot get at the moment, so im not utilizing machine fully. Many of the machines out there running UCCNC, like stepcraft machines ect will never ever have problems like that becaose they would dismantle themselves if run on souch speeds.

[cncdrive]

We run fast machines like plasmacutters with light weight axes and not too rigid frame and they run pretty well upto about their maximum possible 40m/min feedrates.
I think it is not too complicated to understand how the planner works, I mean I do not understand what is so complicated about it?
It is described well in the UCCNC manual, I don't know how to explain it better.

[cncdrive]

The arc radius tolerance is not a CV parameter, it is a tolerance for the arcs when they are coded with radius (R) instead of I and J.
Then it is possible that CAM softwares make the R too short compared to the start and R point which would mathematically defines an impossible to make circle.
For example the start point for an arc is 0,0 and the end point is 10,0 and lets say you want a half circle, now CAM software might generate R4.999 due to rounding errors in it's calculations,
and you see that it is not a circle anymore, because the 2*4.999 = 9.998 and the distance between the start and endpoint for this example is 10. And so it is impossible to define the center point of the arc for that R4.999 code.
This happens with CAM software which could then cause a problem for executing the code. The arc tolerance setting adds a tolerance distance and corrects the radius value if it is shorter than the half of the distance of the start and endpoints, then it calculates the arc center point exactly in the middle between the start and endpoints and executes the arc with those values.
Or if the R is more short than the tolerance then the UCCNC throws an error for that arc into the status field...

[AvB]

Thanks - a problem here is that I don't know much about G-code postprocessing, so I am not sure whether my code uses IJ or R. I will have to have a look. I use Madcam some of the time, and it generates point code rather than arcs. I also use Rhinocam (MecSoft) some of the time, and it generates arcs - much smaller G-code files. I suspect that the Madcam toolpaths are more of a problem for UCCNC.

Could you address the questions above, particularly the question about sharp corners required in 3D moves using Z?

[AvB]

This is the sort of cut I've been concerned about - getting a sharp corner on the leading edge.We can't use a ball nose cutter here because we want the airfoil shape to be very faithful to the original, and the radius right in close to the tip becomes less than 1mm for most foils. So I use 4mm end mill doing parallel cuts at approx 90 deg to the leading edge line, and each pass, it lifts exactly around that corner after cutting tightly into the leading edge tip curve. (see photo of aerofoil tip curve). I was concerned that if I had the CV settings loose enough for general movement to be smooth, it would then round off that LE corner.

This is where I guess you experienced guys would straight away know what to do without thinking but for a 50+ yr old newbie like me with a slow brain, it's not so obvious. I have a test cut that I've used to tune the CV settings previously so I used that to do a similar test today (see photo of test cut toolpaths, and cuts in material). The step-up plateau in the middle of the dished area is not square edged - it has 88 degrees angle sides

1) I loosened up my CV numbers a bit to exaggerate any problems, to:
MCE 0.3
MLE 0.1
MLAL 15
MLUL 35
... and then I did the cut with the CV angle at 90 degrees. It was very smooth and fast, but the corners were all a bit "soft". They looked fine, but I can feel that they are smooth from slight rounding.

2) I then did the same cut with the CV angle set at 45 deg, and although it was a bit slower from pausing at each corner, it was not jerky, and the corner angles were really sharp. Interestingly, the surfaces were smoother - I don't understand why that would be.

3) I repeated the same cut with CV angle staying at 45 deg, but with the CV settings tighter at my "normal" settings:
MCE 0.1
MLE 0.05
MLAL 10
MLUL 25
... and it was still pretty fast and smooth. It wasn't any sharper or better than with the looser settings, but it would have been hard to improve on it.

So in summary, for the wing finishing cuts I've been worried about, I can make sure that the Z lift corners are sharp by keeping the CV angle lower.

[rmat]

This is the sort of cut I've been concerned about - getting a sharp corner on the leading edge.We can't use a ball nose cutter here because we want the airfoil shape to be very faithful to the original, and the radius right in close to the tip becomes less than 1mm for most foils. So I use 4mm end mill doing parallel cuts at approx 90 deg to the leading edge line, and each pass, it lifts exactly around that corner after cutting tightly into the leading edge tip curve. (see photo of aerofoil tip curve). I was concerned that if I had the CV settings loose enough for general movement to be smooth, it would then round off that LE corner.

This is where I guess you experienced guys would straight away know what to do without thinking but for a 50+ yr old newbie like me with a slow brain, it's not so obvious. I have a test cut that I've used to tune the CV settings previously so I used that to do a similar test today (see photo of test cut toolpaths, and cuts in material). The step-up plateau in the middle of the dished area is not square edged - it has 88 degrees angle sides

1) I loosened up my CV numbers a bit to exaggerate any problems, to:
MCE 0.3
MLE 0.1
MLAL 15
MLUL 35
... and then I did the cut with the CV angle at 90 degrees. It was very smooth and fast, but the corners were all a bit "soft". They looked fine, but I can feel that they are smooth from slight rounding.

2) I then did the same cut with the CV angle set at 45 deg, and although it was a bit slower from pausing at each corner, it was not jerky, and the corner angles were really sharp. Interestingly, the surfaces were smoother - I don't understand why that would be.

3) I repeated the same cut with CV angle staying at 45 deg, but with the CV settings tighter at my "normal" settings:
MCE 0.1
MLE 0.05
MLAL 10
MLUL 25
... and it was still pretty fast and smooth. It wasn't any sharper or better than with the looser settings, but it would have been hard to improve on it.

So in summary, for the wing finishing cuts I've been worried about, I can make sure that the Z lift corners are sharp by keeping the CV angle lower.

Thank you for doing this!

Just a suggestion, I am also a plane builder, so we use to cut the moulds with bull nose cutter (for leading edge). Those have 0.5 or 1mm radius so you can just go waterline this radius, will be a mile quicker.
Also, its beter to do those flats with a flat, or you can just use bull nose for flats also.
And it would be more accurate and both more efficient to do two operations, one for airfoil surface finish and other for flat finish. If you want to have true edge, machine has to stop, and the more you stop the looonger the machining takes. Like you already observed, the smoother the motion, the smoother the surface, so make your toolpaths flow.
Also, dont loose your head on accuracy of airfoil ect., big workpieces tend to do miracles when you mill it. I mean especially bending, twisting ect. If you get total accuracy of 0.1mm on 1000mm its already a small miracle.

Best regards, Matej