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