Hey guys,

Im a new SheetCam user and I have a few issues.

I have Version 1 Flashcut CNC and I only have a X and Y axis so I use the FlashCut no Z post processor and export as G code.

When I load up the G code my circles are not showing, the simulator shows them with no isses…

I have the most recent release of SheetCam and have tried uploading and reimporting the code, I even ran it in a different post processor and then back to FlashCut no Z… Still no circles.

I also see in the simulator that my torch is not firing at the beginning of my lead in, it goes along the path of the lead in and then stops and fires the torch on the edge of the circle.

I dont really want to edit every single string of G code to correct these circles…

Any help will be greatly appreciated.

So, in the previous post I said that I didnt want to edit the G code to fix these circles… well honestly after getting back into the program again I can’t seem to figure out how to correct the G code.

searching all over this forum I cannot find anything that will correct this…

Could you post a copy of the code here so I can see what is going on. Is this on a plasma cutter?

Yes, Plasma Cutter and I sure will.

Tonight when I get home. Thanks so much.

Here is the .DXF and the G Code that Sheet Cam generates.

N0000 (Filename: Final Double Wine Holder)

N0010 (Post processor: Flashcut plasma no Z.scpost)

N0020 (Date: 4/3/2013)

N0030 G20 (Units: Inches)

N0040 G90 G40

N0050 (Part: Final Double Wine Holder)

N0060 (Process: Outside Offset, 1, T1: Jet tool)

N0070 M06 T1 (Jet tool)

N0080 G00

N0090 X1.4425 Y10.1725

N0100 M50

N0110 G04 X3

N0120 G01 Y9.9225 F60

N0130 G03 I0.0000 J0.7137 F60.0

N0140 M51

N0150 G00

N0160 X10.8714 Y10.1093

N0170 M50

N0180 G04 X3

N0190 G01 Y9.8593 F60

N0200 G03 I0.0000 J0.7137 F60.0

N0210 M51

N0220 G00

N0230 X12.3083 Y6.3156

N0240 M50

N0250 G04 X3

N0260 G01 X12.0583 F60

N0270 G02 X10.0288 Y4.2861 I-2.0295 J0.0000 F60.0

N0280 G01 X2.0288 F60

N0290 G02 Y8.3451 I-0.0000 J2.0295 F60.0

N0300 G01 X10.0288 F60

N0310 G02 X12.0583 Y6.3156 I-0.0000 J-2.0295 F60.0

N0320 M51

N0330 G00

N0340 X6.0952 Y8.4098

N0350 M50

N0360 G04 X3

N0370 G01 X6.2720 Y8.5866 F60

N0380 Y8.6161

N0390 Y12.5798

N0400 G02 X6.3015 Y12.6094 I0.0295 J0.0000 F60.0

N0410 G01 X10.2652 F60

N0420 G02 Y8.5866 I-0.0000 J-2.0114 F60.0

N0430 G01 X6.3015 F60

N0440 X6.2720

N0450 M51

N0460 G00

N0470 X2.0486 Y12.8725

N0480 M50

N0490 G04 X3

N0500 G01 Y12.6225

N0510 X6.0124

N0520 G02 X6.0419 Y12.5930 I0.0000 J-0.0295 F60.0

N0530 G01 Y8.6293 F60

N0540 G02 X6.0124 Y8.5998 I-0.0295 J0.0000 F60.0

N0550 G01 X2.0486 F60

N0560 G02 Y12.6225 I0.0000 J2.0114 F60.0

N0570 M51

N0580 G00

N0590 X-0.2795 Y2.0000

N0600 M50

N0610 G04 X3

N0620 G01 X-0.0295 F60

N0630 G02 X2.0000 Y4.0295 I2.0295 J-0.0000 F60.0

N0640 G01 X10.0000 F60

N0650 G02 Y-0.0295 I-0.0000 J-2.0295 F60.0

N0660 G01 X2.0000 F60

N0670 G02 X-0.0295 Y2.0000 I-0.0000 J2.0295 F60.0

N0680 M51

N0690 G00

N0700 X0.2500 Y0.2500

N0710 M51 M30

I tried a few other post processes related to FlashCut and nothing would work with circles.

I found a similar post/problem on the forum that had me delete 4 lines under the edit post area… no change in the circles, it still is working fine for other projects that dont have full circles.

Actually it is making my life so much easier, I love Sheetcam! Money well spent.

I sure hope this can be fixed…

Try this version. Does it work?

```
N0000 (Filename: Final Double Wine Holder)
N0010 (Post processor: Flashcut plasma no Z.scpost)
N0020 (Date: 4/3/2013)
N0030 G20 (Units: Inches)
N0040 G90 G40
N0050 (Part: Final Double Wine Holder)
N0060 (Process: Outside Offset, 1, T1: Jet tool)
N0070 M06 T1 (Jet tool)
N0080 G00
N0090 X1.4425 Y10.1725
N0100 M50
N0110 G04 X3
N0120 G01 Y9.9225 F60
N0130 G03 X1.4425 Y9.9225 I0.0000 J0.7137 F60.0
N0140 M51
N0150 G00
N0160 X10.8714 Y10.1093
N0170 M50
N0180 G04 X3
N0190 G01 Y9.8593 F60
N0200 G03 X10.8714 Y9.8593 I0.0000 J0.7137 F60.0
N0210 M51
N0220 G00
N0230 X12.3083 Y6.3156
N0240 M50
N0250 G04 X3
N0260 G01 X12.0583 F60
N0270 G02 X10.0288 Y4.2861 I-2.0295 J0.0000 F60.0
N0280 G01 X2.0288 F60
N0290 G02 Y8.3451 I-0.0000 J2.0295 F60.0
N0300 G01 X10.0288 F60
N0310 G02 X12.0583 Y6.3156 I-0.0000 J-2.0295 F60.0
N0320 M51
N0330 G00
N0340 X6.0952 Y8.4098
N0350 M50
N0360 G04 X3
N0370 G01 X6.2720 Y8.5866 F60
N0380 Y8.6161
N0390 Y12.5798
N0400 G02 X6.3015 Y12.6094 I0.0295 J0.0000 F60.0
N0410 G01 X10.2652 F60
N0420 G02 Y8.5866 I-0.0000 J-2.0114 F60.0
N0430 G01 X6.3015 F60
N0440 X6.2720
N0450 M51
N0460 G00
N0470 X2.0486 Y12.8725
N0480 M50
N0490 G04 X3
N0500 G01 Y12.6225
N0510 X6.0124
N0520 G02 X6.0419 Y12.5930 I0.0000 J-0.0295 F60.0
N0530 G01 Y8.6293 F60
N0540 G02 X6.0124 Y8.5998 I-0.0295 J0.0000 F60.0
N0550 G01 X2.0486 F60
N0560 G02 Y12.6225 I0.0000 J2.0114 F60.0
N0570 M51
N0580 G00
N0590 X-0.2795 Y2.0000
N0600 M50
N0610 G04 X3
N0620 G01 X-0.0295 F60
N0630 G02 X2.0000 Y4.0295 I2.0295 J-0.0000 F60.0
N0640 G01 X10.0000 F60
N0650 G02 Y-0.0295 I-0.0000 J-2.0295 F60.0
N0660 G01 X2.0000 F60
N0670 G02 X-0.0295 Y2.0000 I-0.0000 J2.0295 F60.0
N0680 M51
N0690 G00
N0700 X0.2500 Y0.2500
N0710 M51 M30
```

So, that G-Code worked like a charm!

I can see that you changed this line for both circles:

N0130 G03 X1.4425 Y9.9225 I0.0000 J0.7137 F60.0

It was showing this before:

N0130 G03 I0.0000 J0.7137 F60.0

So my question is… Did you have a different post processor that generated this or did you rely on your awesomeness and technical prowess in G-Code?

Very much appreciated.

Sorry it took me so long to get back to you. I have been out of the office a lot recently. I have come across this issue before on another controller. While the code generated by the post is valid, it looks like earlier versions of Flashcut get confused by the missing X and Y coordinates. The attached post should fix it.

Save the post to any convenient folder the run SheetCam and go to Options->machine->post processor. Click on the ‘import post’ button and open the post. Go back to Options->machine->post processor and make sure you have the edited version of the post selected.

Looking good to me!

Ill run it past the machine since clearly it is the boss of this entire operation… Ill ask it for a raise for you also!

Thanks for the superior support!