Need Help!- Slow G02 / G3 moves

[ronateah]

I am using Mach 3 on my plasma table and I am cutting 8 inch character O in this case. I am using sheetcam tng. I have CV paramenters set and I am generally have with my set up. However the machine slows right down and seems drop the CV functionality when it hits these G02 G03 moves. I am not sure why there are so many G03 moves in the code as it only happens in a relatively small portion of the cut. I am not clear as to why my velocities slow down and become jerky as well.

Any help would be much appreciated - Ron

N16930 M03
N16940 G04 P0.6
N16950 G01 Z0.0650 F80
N16960 G02 X7.9508 Y13.8441 I-0.0073 J0.1118 F45.0
N16970 G01 X7.9396 Y15.7516
N16980 X9.4879 Y15.7607
N16990 G03 X9.4985 Y15.7608 I-0.0086 J2.0695
N17000 X9.5188 Y15.7621 I-0.0035 J0.2056
N17010 X9.5395 Y15.7655 I-0.0273 J0.2330
N17020 X9.5608 Y15.7708 I-0.0560 J0.2683
N17030 X9.5825 Y15.7781 I-0.0912 J0.3106
N17040 X9.6049 Y15.7872 I-0.1342 J0.3603
N17050 X9.6278 Y15.7982 I-0.1863 J0.4182
N17060 X9.6514 Y15.8110 I-0.2491 J0.4847
N17070 X9.6756 Y15.8257 I-0.3237 J0.5604
N17080 X9.7005 Y15.8423 I-0.4118 J0.6459
N17090 X9.7260 Y15.8606 I-0.5145 J0.7417
N17100 X9.7522 Y15.8809 I-0.6334 J0.8484
N17110 X9.7791 Y15.9029 I-0.7697 J0.9666
N17120 X9.8067 Y15.9268 I-0.9249 J1.0968
N17130 X9.8350 Y15.9525 I-1.1003 J1.2395
N17140 X9.8640 Y15.9801 I-1.2974 J1.3953
N17150 X9.8938 Y16.0095 I-1.5174 J1.5647
N17160 X9.9242 Y16.0407 I-1.7618 J1.7484
N17170 X9.9554 Y16.0738 I-2.0319 J1.9468
N17180 X9.9874 Y16.1087 I-2.3290 J2.1605
N17190 X10.0200 Y16.1455 I-2.6547 J2.3900
N17200 X10.0530 Y16.1837 I-3.1376 J2.7469
N17210 X10.0847 Y16.2212 I-3.0223 J2.5829
N17220 X10.1147 Y16.2577 I-2.7307 J2.2761
N17230 X10.1431 Y16.2933 I-2.4593 J1.9951

[ger21]

Mach3's CV can not maintain constant velocity in all situations. The problem is that a lot of those arcs are only .01 to .02 long.

Do you have CV distance or CV feedrate turned on? Try turning them off. Also, turn off CV angle greater than as well and see if it helps.

[ronateah]

I need my cv settings. They are necessary for the rest of the part. This code is only representive of a small parts of the cut that are problematic.l

[Torchhead]

You don't turn off CV. He meant turn off the CV Feedrate and the CV accleration CV options. They are on the settings tab. Also do not try to use Backlash compensation with CV...they play poorly together. Also there is an F45 command on the G02 and it's modal so the G03 will use it as well. Do you really want to cut at 45 IPM? Must be thick metal.

TOM Caudle
www.CandCNC.com

[ronateah]

Thanks Tom I will have to check this tomorrow. In the mean time I got a reply from sheetcam suggesting I alter the way I am bringing drawings into sheetcam and as well as editing the post to ignore arcs less than 1.5 inches and use small moves instead. Seems to have mad a big diference. To be clear though I do know now that I have a bit of an issue with the computer I am using which could also be a contributor to the problem. I thought I was fine with the on video but it looks like it is a problem. I have an external video card on order.

I was cutting 1/4 inch with a fine tip on a hypertherm 1000 at 45ipm. Is out of line?