Cut speed decreases after second pierce.

[Ribbedgiraffe]

Hello all, I've discovered a new problem (actually it's not new, it was never that important before this point).
For some reason when I'm cutting an item that has multiple start points (like most projects) my Mach 3 slows down after the second cut, i.e., for a specific item I'm cutting now, my speed is 60ipm, after the second pierce I'm dropping to 20ipm, I'm assuming it is something sheetcam is producing in the Gcode, anyone else have these types of issues? It doesn't always do it, that's the weird part.

[sphurley]

What version of SheetCam? What post processor are you using to create the G-code?

[acourtjester]

For the second cut is there any "cut rules" used that may have been accidently placed in the G-code.
Attaching a section of the G-code for the starting of the second cut may help to see.

[Ribbedgiraffe]

Sorry Guys - Its been a busy week at work.

The version of SheetCam im using is 6.0.15 - honestly I know its silly, but I'm a little worried to update until I get all the bugs worked out.

Here is the Gcode from the end of the first cut.
N1310 M05
N1320 G00 Z0.5000
N1330 X3.8300 Y2.4855
N1340 Z0.2200
N1350 G90F100
N1360 G31 Z-3 F20
N1370 G92 z0
N1380 G0 z0.16
N1390 Z0.2200
N1400 M03
N1410 G04 P0.06
N1420 G01 Z0.1800
N1430 G02 X3.7500 Y2.4055 I-0.0800 J0.0000

[Les Newell]

That looks like a post processor issue to me. What post processor are you using?

[Ribbedgiraffe]

That looks like a post processor issue to me. What post processor are you using?

Ill have to double check, I believe it is a Mach3 one that I had to modify . Is there a line of code that jumps out to you as being wrong?

[Les Newell]

line N1350 looks odd. I wouldn't have expected a G90 there.

[WyoGreen]

I see a speed rate change to 20 in line 1360 (N1360 G31 Z-3 F20), but no feed changes after that.

Steve

[Ribbedgiraffe]

ok - I see the problem...

Looking at the initial Pierce;
N0110 G00 Z0.5000
N0120 X2.9116 Y1.3529
N0130 Z0.2200
N0140 G90F100
N0150 G31 Z-3 F20
N0160 G92 z0
N0170 G0 z0.16
N0180 Z0.2200
N0190 M03
N0200 G04 P0.06
N0210 G01 Z0.1800 F60.0 < - Feed rate is set in the Post processor from speed input in sheetcam

VS

The second Pierce
N1320 G00 Z0.5000
N1330 X3.8300 Y2.4855
N1340 Z0.2200
N1350 G90F100
N1360 G31 Z-3 F20
N1370 G92 z0
N1380 G0 z0.16
N1390 Z0.2200
N1400 M03
N1410 G04 P0.06
N1420 G01 Z0.1800 < - Feed rate is not being transferred, its still running the speed set back on Line N1360?

I'm not sure what I'm missing in the Post Processor to get the same feed rate I achieve after the initial pierce.

function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G31 Z-3 F20\n")
post.ModalText (" G92 z0\n")
post.ModalText (" G0 z0.16\n")
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end


Thoughts on a solution?