Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Davek0974 on April 24, 2014, 07:16:54 AM
-
I drew up a part this morning and run it on my plasma table in thin sheet as a trial part.
It contains arcs and straight lines plus one circle, I have attached the dxf file plus a picture.
On the picture I have marked four points where the action goes from straight motion to an arc and there is a visible divot at each point.
However there is no divot at the exit from each arc - it transitions perfectly. The other bigger arrows indicate cut direction.
I can not see anything wrong in the dxf and likewise in sheetcam so it has me guessing now, any ideas???
-
I've got a feeling I've seen this before - but my memory's shot. I seem to remember it was only happening on straight line to clockwise arcs - which looks like what you're seeing. I think this was YEARS ago though. What version are you using?
-
This one - Mach3Version3.043.066.exe
-
Never used 3.043.066 but I believe Hood advises not to use it.
-
Damn ::)
Is there a "recommended" plasma version?
Also, is it an easy install or do i have to follow a winding path to get it all working again?
-
Someone woke up Mr. Grumpy this morning then...
re-install is easy - but of course you should always backup first. I do it all the time on my test PC to try different things and have never lost any settings. I do it by un-ticking everything except for the parallel port driver. That way it installs Mach and the PP but no xml, no screensets, etc.
Just a hunch but read this thread - I think it may be related. http://www.machsupport.com/forum/index.php/topic,24350.0.html
-
Not sure it was related but interesting anyway.
I have a copy of 062 here, I'll try that.
-
062 made no difference.
Something I have just noticed is that on a dumbell shape cut - a bar with a circle on each end, I get a sharp entry into the arc from the straight but on exit from the arc to the straight Mach is cutting the corner and giving some sort of fillet - the two sides do not match.
Picture attached.
the drawing looks like the sharp transitions not the rounded ones.
Is this a mach issue or a settings issue?
Clearly it could not be used like this.
It is better at low speed but still the entry/exit do not match
-
Could be a lookahead/CV problem.
How are the arcs being created in the G-code?
Probably worth uploading the G-code you used for that, so people can see if the G-code is good.
-
This is the code, I know there is an issue with the odd THC on/off codes but that's not the issue here and is being dealt with elsewhere.
I have learnt that it seems to be connected with CV and acceleration settings so I'm going to retune next week and see if that makes a change.
N0010 (Filename: Test 1.tap)
N0020 (Post processor: Mach3 THC with scriber 2.scpost)
N0030 (Date: 25/04/2014)
N0040 G21 (Units: Metric)
N0050 F1
N0060 G53 G90 G40 G64
N0070 (Part: Test 1)
N0080 (Operation: Outside Offset, 0, T2: 1.5mm Steel, 30A, Std Tip, 103v)
N0090 G00 X41.3478 Y30.1053
N0100 G28.1 Z3.00 F800.0
N0110 G92 Z0.0
N0120 G00 Z3.9000
N0130 G92 Z0.0
N0140 G00 Z3.5000
N0150 M03
N0160 G01 Z1.0000
N0170 M101 (THC Off) (On arcs)
N0180 G03 X50.9478 Y20.5053 I9.6000 J0.0000 F2310.0
N0190 M102 (THC On) (On arcs)
N0200 G01 X72.6444 F3300.0
N0210 M101 (THC Off) (On arcs)
N0220 G02 Y9.4947 I14.3556 J-5.5053 F2310.0
N0230 M102 (THC On) (On arcs)
N0240 G01 X29.3556 F3300.0
N0250 M101 (THC Off) (On arcs)
N0260 G02 X0.5522 Y9.7414 I-14.3556 J5.5053 F2310.0
N0270 M102 (THC On) (On arcs)
N0280 M101 (THC Off) (On arcs)
N0290 X9.7414 Y29.4478 I14.4478 J5.2586
N0300 M102 (THC On) (On arcs)
N0310 M101 (THC Off) (On arcs)
N0320 X29.3556 Y20.5053 I5.2586 J-14.4478
N0330 M102 (THC On) (On arcs)
N0340 G01 X50.9478 F3300.0
N0350 X52.4478
N0360 M05
N0370 G00 Z10.0000
N0380 X0.0000 Y0.0000
N0390 M05 M30
-
Could it be related to the different feedrates for G1 and G3s?
Going into the arc, lookahead will see the lower feedrate so will be able to corner sharper, whereas coming out the arc into the straight with the higher feedrate, it has to corner less to maintain/accelerate to the higher feedrate.
-
It seems to get very confused between line 260 and 340?
The first arc is a lead-in mid way on the top straight
-
That code is exactly the same as in your other thread but the two pictures show entirely different results and problems. Have you changed something else or is this (or the other) the wrong code for the image.
-
I upped the speed, the 6000 marked is 6000mm/min, the other would have been at 3300mm/min.
The different entry/exit angle is still there just not so visible at the lower speed.
From what I have been told and read, this is related to CV being choked by poor acceleration and if this correct, hopefully I will be able to fix it this week when I redo my acceleration settings.
Does that sound correct?
-
I upped the speed, the 6000 marked is 6000mm/min, the other would have been at 3300mm/min.
The different entry/exit angle is still there just not so visible at the lower speed.
From what I have been told and read, this is related to CV being choked by poor acceleration and if this correct, hopefully I will be able to fix it this week when I redo my acceleration settings.
Does that sound correct?
It's impossible to say unless you post the ACTUAL code you used - sorry Dave but something similar to what you used is no use - I can't simulate here without THE file.
However IF the code you used has M codes in the same places then it is absolutely 100% nothing to do with CV. Mach's CV planner can NOT cross M codes. You already know this remember, because it's in my post (#6) in your other thread.
-
Pasted wrong code, my apologies. It should be this one, it's the same but I killed the THC stuff in sheetcam then wound the speed up.
N0010 (Filename: Test 1.tap)
N0020 (Post processor: Mach3 THC with scriber 2.scpost)
N0030 (Date: 25/04/2014)
N0040 G21 (Units: Metric)
N0050 F1
N0060 G53 G90 G40 G64
N0070 (Part: Test 1)
N0080 (Operation: Outside Offset, 0, T2: 1.5mm Steel, 30A, Std Tip, 103v)
N0090 G00 X41.3478 Y30.1053
N0100 G28.1 Z3.00 F800.0
N0110 G92 Z0.0
N0120 G00 Z3.9000
N0130 G92 Z0.0
N0140 G00 Z3.5000
N0150 M03
N0160 G01 Z1.0000
N0170 G03 X50.9478 Y20.5053 I9.6000 J0.0000 F6000.0
N0180 G01 X72.6444 F6000.0
N0190 G02 Y9.4947 I14.3556 J-5.5053 F6000.0
N0200 G01 X29.3556 F6000.0
N0210 G02 X0.5522 Y9.7414 I-14.3556 J5.5053 F6000.0
N0220 X9.7414 Y29.4478 I14.4478 J5.2586
N0230 X29.3556 Y20.5053 I5.2586 J-14.4478
N0240 G01 X50.9478 F6000.0
N0250 X52.4478
N0260 M05
N0270 G00 Z10.0000
N0280 X0.0000 Y0.0000
N0290 M05 M30
It might be better if I retune my settings before you invest any time on this one, if it is connected with poor acceleration then it could resolve itself, thanks anyway.
-
What are your axis setup parameters VEL, ACCEL ?
If you are getting rounding with THIS file your are either cutting TOO fast OR accel setting too slow for the feedrate.
It looks as thought you are cutting at about 240IPM which is way to fast for the most part for the material you are cutting and AT that feedrate your accel should be about 30 ips/s .
Remember the settings you see for the cutting in the manuals are for very rigid servo driven industrial cutting machines. They can run at very fast speeds and cut square inside corners AT that speed with very fast accelleration rates on the drives.
I am guessing that you are NOT using one of those machines (;-) so your setup and cutting parameters should be VERY different .
For that file and material here I would be cutting at about 130IPM Cut height .080 with a fine cut tip and nozzle, 40 amp power setting AND I get very sharp inside corners HERE. Fine tune the Feedrate to TUNE the cut quality. It may be a touch faster or slower just depends on conditions and material.
Just a thought, (;-) TP
PS, IAN sorry for taking over your post(;-) but I cut that type material every day on a DIY type machine.
-
Many thanks for that help, you see this is where lack of knowledge really bites me.
As I know not what is right or wrong, I can only follow stuff given to me here and there on the 'net. So far this advice has been to cut at silly fast speed with full-on acceleration and as much power as I have. That is what I was testing when I spotted this effect. Obviously I had pushed my parameters too far and not realised.
My previous cuts were exactly where you just said - around 3300mm.min!
I was going faster to see if it reduced dross (easily tapped off) as I had been advised. In the end the dross got less but harder so counter productive effect. This was with standard consumables.
Even at that 236ipm rate, the little table still managed to make that cut without losing a step which I feel is a good thing, I will retune it this week and reduce the speeds again a fair bit back into the real world.
BTW the book recommends 10,000mm/min which just seems stupid fast and there is no way that could be attained on a table that is only 700mm square without some serious G force effects, it would probably tip over on each corner :)
Thanks again, it is real-world figures I am searching for, but bear in mind I only have 30A to play with.
-
PS, IAN sorry for taking over your post(;-) but I cut that type material every day on a DIY type machine.
Hey Terry - not my post - be my guest - Like I've said, you've probably forgotten more about plasma than I'll ever know.
Turns out though that with specific regard to the question about the firedoor and dumbbell I've found this:
It would appear it's caused by a bug in Mach's CV when using Angles >. It only affects G1/G2 blends and not G1/G3. So that's why you're seeing your notches where they are in the firedoor and why you have asymetric blends on the dumbbell. It goes from the present version back through to the dawn of time so looks like we're stuck with it.
However, as Terry and I have both said you shouldn't be needing CV options anyway so it shouldn't be an issue here. Note that this doesn't solve your rounding - it will just make it consistent - your rounding is still down to speed/accel. At least though, now ALL your joins should be rounding you shouldn't get the notching.
Cheers
Ian
-
Brilliant, thanks Stirling.
As I said, I will be clearing that cv angles box this week and then retuning.
From what I've read, it seems I need to set my max speed (pretty much where it is) and then push acceleration until it fails through lost steps or gets too violent and then back it off maybe to 70% of that value?
Does that seem correct?
What are your views on speed? I have currently set my max at 9000mm.min as I could not see any point in setting it higher, but is that still too high for such a small table?? The reason I ask is that speed and acceleration seem interdependent so I don't want to waste time on one if the other is wrong, I think that's logical :)
-
HIGH speeds are only good for LARGE tables were you have to jog a long distance sometimes. It is a waste on small tables and will bite you one day jogging at high speed on a small table.
Here I limit the table to 200IPM at 30IPS/s accel. That does a great jog on 99.99% of all cutting we do. That would be from 28 guage up to 3/4" Steel and 28ga to 3/8" alum plate AND we cut a lot of each.
YOUR parameters will be dependant on your table design , rigidity, drives and motor and Feed mechanics ( screw,rack/pinion,belt) type.
(;-) TP
-
Brilliant, thanks
Looks like I'm shooting too high on the speed and too low in acceleration.
Does my tuning strategy seem correct?
-
IF you go with a lower Vel then your acel is not as sensitive to lost steps.
Your sweet spot will be based on YOUR machines ability to Acell under load.
TEST,Tune,Test,Tune
(;-) TP
-
Just out of curiosity, and I know it's machine specific, but what sort of figure do you have for relative G force on your setup??
-
OK, educational half hour for me...
Speed was set at 3300mm/min in the file, THC codes removed, all CV config boxes cleared, THC turned on and ignored by me ;)
In the first picture we have, from the back, acceleration values of 2000, 1500, 1000 & 900mm/s/s
As you can see, the higher the acceleration, the worse is the ripple effect caused by my belt drive system or machine design being taxed too hard.
Once I hit 1000mm/s/s I dropped to the smaller increment to see what happens and the 900 seems to be pretty acceptable i think?
The second picture shows the 900mm/s/s cut face-on and the nasty exit slope seems to be all but gone now which is good.
A question..
Is it worth going any lower on acceleration as the quality likely will not improve much as it seems pretty good bearing in mind this is the thinnest/fastest material I have (1mm)?
-
CV rounding < accel > Jerk.
i.e. accels right there somewhere between CV rounding and Jerk. What's the best accel for your machine? Looks like your close on finding it. To me those cuts look pretty darn good. Good work.
Ian
-
Well at least I'm getting somewhere now thanks to all the help :)
I might try and se what happens if I knock it back another 50 maybe, just for reference purposes but as it is, I think it's a 100% better.
Question - as it is I now know it will work at 3300mm.min on 1mm sheet very nicely. If I then go for thicker metal, say cutting at 700mm.min, will the acceleration have less 'bite' than it does at this higher speed.?
My guess is it will be gentler as there is less speed to reach but I'm still a bit foggy on how it affects the process.
:)
-
The question remains is the chatter in the cut related to the belt drive rebounding OR is it THC osillation due to the THC coming back online after the arc ?? I would lower the THC SPEED a bit and go back up on acell just to see IF it is any better.
Here that cut would be a nice sharp corner about as sharp as it it drawn .BUT that is this machine not yours. Here the settings are Vel 200 Acell 30IPS/S. It would depend on the drives/motors here everything runs from nema 34 high torque motors and gecko drives and the CLong axis has 2 slaved nema 34's.
Looking better though, (;-) TP
-
I could run the same speed and part with THC off to prove the point, but I'm fairly certain it's belt flex. I have the THC rate very low, 8 or 10% i think! I don't think it would react fast enough to oscillate that rapidly. Plus the sheet is pretty flat so I doubt THC is doing much at all in this instance.
Will try tomorrow though just for confirmation.
It's more likely because I have under specified my belts, they are only 10mm wide, Y has two and Z has one. To make matters worse, they are full loops too so are about 2m long each. I could have halved that by mounting the motor on the gantry and using the belt as a rack but that would make the gantry far heavier which I thought would be a worse situation.
Live and learn, it's almost pretty damn good and that will be good enough for my uses I think, little bit more fiddling and learning should have it nailed.
Just thinking on, my settings for vel and acc are higher than yours, would I not get exactly the same results as you by setting them the same?
Just wondering.
-
Question - as it is I now know it will work at 3300mm.min on 1mm sheet very nicely. If I then go for thicker metal, say cutting at 700mm.min, will the acceleration have less 'bite' than it does at this higher speed.?
Not sure what you mean by "bite" but if you mean "jerk" then...
(Jerk is not just an arbitrary term btw - it's the pukka name for the rate of change of acceleration).
As acceleration is constant in Mach - so is Jerk. (There used to be a planner that used S-curve accel to reduce jerk - but that's another story).
Or to put it another way - any lack of rigidity presents the same issues at any speed.
Not sure if that answers your question.
-
Yes, i think so ;)
Anyway, I just squeezed in a little play time and ran the dumbell with THC off and no change so as I suspected, my ripple effects are all machine related, at least i know now.
I tried dropping the acc to 850, no change so i will leave it there for now.
Then I tried the file for the picture attached, this is the most detailed I have tried yet and was met with total success, the shape matches the file, it has some surprisingly fine detail in it and apart from the metal being some galvanised crap, is just about perfect.
There is some dross but look at it and falls off so i'm not worried about trying to get rid of that, looking at the way the machine was whipping around it, I really dont think more speed is possible so dross is a thing that I live with I guess?