Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Davek0974 on September 12, 2015, 02:51:28 PM
-
Been trying to improve my plasma cut quality on internal corners, using the "Stop CV on angles >89" appears to help but I seem to get a visible jerk in the cut upon each transition from a straight line to an arc or radius, is that normal??
Is there any improvement to be had or is it just the way it is?
-
What are you trying to improve about your cuts ?? Rounding ??
(;-) TP
-
Pretty much, yes, its a plasma PITA :)
With CV on i get a bit of a radius on the top of the cut, (the bottom is always rounded due the the flame lag) and with CV off the tops are much improved but there is this jerk when going from straight to curve every time, not much, just a judder in motion.
I'm just tuning up my new table so looking at ways to get the best, I have tried pushing acceleration into the shudder zone but the stop-CV is still the best for a sharp corner. Acceleration is currently around 0.3G and speeds are around 4000-5000mm/min on my test parts.
As i say, I'm just looking for improvements really, Mach is doing what it does best as usual :)
-
Bit confused here Dave. TP asked if you were talking about (corner) rounding and you said yes but then described the problem as top edge bevelling. Which is it you're concerned about?
-
Its a confusing thing plasma, the bottom of an internal corner is always rounded because the bottom of the flame or arc lags the top by about 15degrees or so, so as the top has passed the corner the bottom has no option but to round it leaving a bevel..
I think the main crux of my question was is there way to stop the jerks when transitioning from a straight to an arc when using stop-cv???
-
I think the main crux of my question was is there way to stop the jerks when transitioning from a straight to an arc when using stop-cv???
The problem here is that if you have a line tangentially joining an arc then it is essentially pointless using stop-cv on angles > because there IS NO angle.
The fact you've asked the question would suggest that you do indeed see a difference. That is baffling because it makes no sense.
-
Yes the line joins as you say - no angle.
Yes, It's pointless using stop cv on that part BUT lets say the part has internal corners AND arcs etc, the corners are improved BUT the arcs are degraded by the blip.
-
but here should NEVER be a "blip" with CV - anywhere - period. If there is then CV would be pointless - and it isn't.
maybe time to post some code and a description that demonstrates your problem(s).
-
but here should NEVER be a "blip" with CV - anywhere - period.
I've cut parts on my router where CV would stop when it shouldn't.
An oval, two straight sections with tangent round ends. On one side it would stop before making the turn, and the other side it would transition smoothly.
-
Ok, g-code and a picture attached.
You can clearly see the hiccup in the cut on the last two parts in the picture, the only difference was turning stop-cv on angles>89 deg on for these two.
The reason for wanting the exact-stop is because there is a 3mm slot in the parts which i wanted as square as possible.
-
take a look at line N0360 and N0490 and tell me what you see.
-
take a look at line N0360 and N0490 and tell me what you see.
N0360 G01 X8.171 Y25.365
N0490 X33.009 Y48.108
G01 is missing?
Thats all i can see, i'm way down the learning chain though...
-
No that's perfectly fine.
Sorry Dave - it's actually N0370 etc. and it's not quite what I thought now I've looked closer.
However, I'm guessing it (and possibly some others) are still the cause of your ills. The thing is your toolpath has loads of REALLY short lines joining your "intended" lines to arcs. The one on line 370 is 0.07mm long (where I think ONE of your "blips" is). I'm thinking this is what's tripping up CV with angles >.
NOW - it shouldn't - but I seem to recall REALLY short lines having bad effects sometimes in CV so I'd get rid of them and see what happens.
What CAD/CAM do you use?
Are the 2 "blips" in your photo the only two?
-
Dave, (;-) It would seem you have an accel issue IF you are getting corner rounding. Plasma depends on a constant as possible cutting rate . Turning OFF CV anywhere defeats the purpose of CV. I plasma cut just about everyday from 28ga up to 3/4",steel and aluminum.
A lot of what you are talking about in corners is a THC problem where it is NOT holding the height as it slows down. THAT is a setting you need to play with. Start adjusting the anti dive/corner dive in Mach3. IF it is to much reduction in vel before it locks then you get a arc that is to low and THAT will angle the kerf . You want the anti dive to lock out before it effects cut quality.
Another issue is using the correct combination of Nozzle, Sheild. air pressure, amp settings, DRY AIR. This are very important to cut quality as well. Get one part off and the quality goes down the tube.
with Plasma a LOT can be said out the quality of the Cut file. You are much better of with radiused corners where ever possible. A sharp intentional corner makes it HARDER for the machine to maintain a constant cutting speed(almost impossible) without rounding. Accel is king with Plasma cutting and well as a very lightweight rigid gantry. Motros are calculated for max acell properties (low inertia High torque) THEN comes speed. Most times steppers have limited RANGE of operational speed where as Servos have a much wider RPM band they can work in.
THCs are another can of worms for most DIY users . BUT that is a different chapter in the " So you want to be a plasma cutter book ". (;-)
NOW IF your control cannot do transitional changes in Gcode without a HESITATION then you have a Controller problem. There ARE controllers that do not have that problem. Another chapter in the book. The trajectory planner has to be top notch and very much in control without hesitations in execution.
I use the STANDARD Mach3 CV with NO adjustments at all. JUST like it comes out of the box and it cuts fine detail very well here. I do a LOT of artsy stuff where DETAIL is an issue. NOW that siad I also use an alternative cutting speed settings for the very thin stuf <18ga . I am not interested in trying to cut above 200 IPM . There is ALWAYS an alternative cutting solutions to high speed cutting, you just have to find it
You are trying to solve a mechanical issue through software control (;-).
-
Terry
Generally I agree with everything you've said.
However - look at WHERE the gouging is happening on the picture. That should have NOTHING to do with slowdown because at that point there shouldn't BE any slowdown.
Of course there obviously IS, which is why I've suggested what I have.
-
Hmm, ok here we go ;D
That file is not my general standard, it's downloaded from the 'net and yes it's pretty ugly when loaded in CAD, thousands of little lines. However, with normal CV on, it cuts perfectly fine - no issues at all, its only when stop-cv is on that the blips show up and there is one every point where it goes form straight to a curve - no slowdown so should not blip.
It's a minor point and i was just playing about looking for improvements.
Yes, I have not fine-tuned the THC yet, it could well be diving unseen, I will have a play with the dive% settings.
So far I only have the 45A consumables for my PM45, I will be getting some 30A ones to try though. The air is passed through a refrigerated dryer so should be pretty good.
Any chance of a pic or two of some examples of your cuts for comparison, some settings maybe ;)
-
OK are ALL the plates the same way ?? I can not see enough kerf detail to tell IF it was coming into the arc or just coming out of the arc ? Which was it. I see 2 defects.
Both appear to be a stall of motion ?? . Does it do the same thing if you set the CV back to box stock settings ?. never see that here so it appears to be a local event. are you using the LPT version or other ?? What THC ?? Have you tried with the THC off ??
Have you reversed the motion to see IF it is an arc direction problem ?
(;-) TP
-
I've only cut this one part, using it as a test to check the slot width etc. The whole lot are drawn just as badly though.
No, with CV back on the blips disappear.
This is the LPT version, the THC is a CandCNC Mp3000 DTHC2, not tried this part with THC off yet or reversed directions.
I've attached the whole file incase someone wants a play.
-
Dave what version of Mach3 are you running ??? IF the problem goes away when you put the CV back to normal then there is your answer , leave teh CV alone and work on other areas for improvement. IF you are having rounding problems at those speeds then you need to rethink your settings or motors/drives or gantry design. (;-)
(;-) TP
-
Hi
can't remember which version, its at home, will check tonight but i do know that the CandCNC plugins and THC only works with one version of Mach.
Yes i can leave it on of course.
The main issue is i think that i done even know what a PM45 is capable of when it comes to internal corner quality, i know it can't be tighter than the radius of the flame but its difficult to know when you can't see what other users are happy with ;) I may be chasing the impossible.
Anyway, thanks all for the info, I will leave CV on as normal and revisit my table settings etc.
-
Well I had a vague recollection that actually I'd seen this before. It was raised here (http://www.machsupport.com/forum/index.php/topic,4113.0.html) in 2007 and fixed in R2.56. I guess it was broken again later. The latest version I've just tried is R3.043.62 and it's still busted in there.
It's actually nothing to do with short lines, it's simply when you have any arc following any line where "stop cv on angles >" is ticked.
So Dave, if you absolutely must turn CV off selectively, here's "A" solution for you. Just stick a G61 and a G64 in your code at the appropriate places. There are other ways but this seems as easy as any.
-
Ohh, nice, found a bug ;)
Ok thanks for the fix, very useful.
Dave
-
Dave it is NOT an issue with the PM45 it is a Machine design issue. You accel is too slow . Have you tried raising the acell rate until you get skipping of steps then back it up untill it stops skippinging steps. THAT is the only way to know the upper limit of the setting.
AND it that is still not enougt THEN you redesign the drives/motors /power supply to a better combination that WILL let you get to where you need to be.
-
Dave it is NOT an issue with the PM45 it is a Machine design issue. You accel is too slow . Have you tried raising the acell rate until you get skipping of steps then back it up untill it stops skippinging steps. THAT is the only way to know the upper limit of the setting.
AND it that is still not enougt THEN you redesign the drives/motors /power supply to a better combination that WILL let you get to where you need to be.
Not sure i ever hinted it was an issue with the PM45?? I will retune the drives as soon as i can, this is a pretty small issue really, i know plasma can never cut a square corner and i have seen some samples of others work which shows i am not that far away from a typical cut.
I will push it to the limit though just to find the limit ;)
-
Reply #19
"" The main issue is i think that i done even know what a PM45 is capable of when it comes to internal corner quality, i know it can't be tighter than the radius of the flame but its difficult to know when you can't see what other users are happy with Wink I may be chasing the impossible. ""
You can cut as tight an inside corner as the width of the kerf. That leaves the radius of the kerf as the squarest corner you can cut. It is NO different than with a router or mill.
(;-) TP
(;-) TP