forum.cncdrive.com

In the video below I have a plasma drill op (see code snippet). Looking at the video the dwell time starts before the arc ok signal (you can watch the LED's in the video). Is there a setting to have it wait for ARC ok before Dwell starts? (THC is ON)

Code: Select all

N0130 (Operation: Drill, DRILL, T103: finecut 16g steel, 0 in Deep)
N0140 G00 X1.1675 Y1.4567 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G04 P0.600
N0190 G01 X1.1675 Y1.4567 Z0.0600 F150.0
N0200 M05 (Torch Off)

https://www.youtube.com/watch?v=GjEhSnAXxm8

If your phone or camera can do slow motion recording, zoom in on the dwell DRO, and the arc OK and dwell LEDs.

You will see the dwell LED come on but the dwell DRO does not start counting until the arc ok LED comes on.

So it appears the dwell LED is only an indication that a G04 command is now in progress, but the actual dwell timing does not start until the arc OK signal has arrived.

I'm a plasma user too so was very interested to check that out.

I will have to try that.... The reason I posted this was because of the behavior below. It is the same 4 plasma drill operations as above but with a 400ms delay instead of 600ms. The torch only fires on the first of the 4 drills. You can see the torch on button turn on for the 3 non torch firing drill attempts. The dwell proceeds without an ARC OK. If it was waiting for the ARC OK and the torch did not fire the gcode should not proceed. Something funny is going on here. I am running the latest dev version of UCCNC from Feb 2020. Controller is AXBB-E.

https://www.youtube.com/watch?v=3ME4QUhiNPk

Code: Select all

N0010 (Filename: stepper mount - rob edit 16g v8 DRILLS.tap)
N0020 (Post processor: UCCNC_M1031.scpost)
N0030 (Date: 13/08/2020)
N0040 G20 (Units: Inches)
N0050 G17 G40 G49 G50 G64 G69
N0060 G80 G90 G94
N0070 M205 (THCON)
N0080 F1
N0090 S1
N0100 (Part: stepper mount beefy v5)
N0110 M06 T103  (finecut 16g steel)
N0120 G64 Q0.023
N0130 (Operation: Drill, DRILL, T103: finecut 16g steel, 0 in Deep)
N0140 G00 X1.1675 Y1.4567 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G04 P0.400
N0190 G01 X1.1675 Y1.4567 Z0.0600 F150.0
N0200 M05 (Torch Off)
N0210 G04 P0.200
N0220 G00 Z1.5000
N0230 X2.3880
N0240 M1031 (TouchOff)
N0250 G00 Z0.1500
N0260 M03 (Torch Fire)
N0270 G04 P0.400
N0280 G01 X2.3880 Y1.4567 Z0.0600 F150.0
N0290 M05 (Torch Off)
N0300 G04 P0.200
N0310 G00 Z1.5000
N0320 X1.1675 Y0.2362
N0330 M1031 (TouchOff)
N0340 G00 Z0.1500
N0350 M03 (Torch Fire)
N0360 G04 P0.400
N0370 G01 X1.1675 Y0.2362 Z0.0600 F150.0
N0380 M05 (Torch Off)
N0390 G04 P0.200
N0400 G00 Z1.5000
N0410 X2.3880
N0420 M1031 (TouchOff)
N0430 G00 Z0.1500
N0440 M03 (Torch Fire)
N0450 G04 P0.400
N0460 G01 X2.3880 Y0.2362 Z0.0600 F150.0
N0470 M05 (Torch Off)
N0480 G04 P0.200
N0490 G00 Z1.5000
N0500 G0 X0.0 Y0.0
N0510 M05 M30


I did 2 more test videos

In this video I run the drill code above with the ARC OK set to pin to a non used pin. The drill ops do not pause to wait for the ARC OK that does not come.

https://www.youtube.com/watch?v=JYTGtgu4Xp8


In this second video I do a line test to show that with longer duration cuts the ARC OK functionality does work. I cut a line with ARC OK set to the right pin. With it set to the wrong pin the torch fires an waits over the hole for the ARC OK signal that does not arrive. I need to stop it manually with the estop switch.

Their seems to be an issue with really short operations where ARC OK is not honored. Maybe I have something configured wrong?

https://www.youtube.com/watch?v=kAf_hoPSqek

Config screens

When drilling holes with plasma, in fact there is no movement of the machine (along the x or y axis), so the lack of ARC OK signal has nothing to stop.
Try inserting a little movement for the x or y axis in the G code after M3.

For example instead of:
N0130 (Operation: Drill, DRILL, T103: finecut 16g steel, 0 in Deep)
N0140 G00 X1.1675 Y1.4567 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G04 P0.400
N0190 G01 X1.1675 Y1.4567 Z0.0600 F150.0
N0200 M05 (Torch Off)

Try this:
N0130 (Operation: Drill, DRILL, T103: finecut 16g steel, 0 in Deep)
N0140 G00 X1.1675 Y1.4567 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G01 X1.1676 Y1.4567 // x moved by 0.0001
N0190 G04 P0.400
N0200 G01 Z0.0600 F150.0
N0210 M05 (Torch Off)

Here is the code for a line that does work (waits for ARC OK). It does not have any code after the M03 and before the dwell like you propose. I get what you are saying though.

Code: Select all

N0130 (Operation: No Offset, LAYER_1, T103: finecut 16g steel)
N0140 G00 X0.0000 Y0.0000 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G04 P0.400
N0190 G01 X0.0000 Y0.0000 Z0.0600 F150.0
N0200 X2.7165
N0210 M05 (Torch Off)


I could do this to make it more inline with the code above. Moving your 0.0001" move below the pause.

Code: Select all

Try this:
N0130 (Operation: Drill, DRILL, T103: finecut 16g steel, 0 in Deep)
N0140 G00 X1.1675 Y1.4567 Z1.5000
N0150 M1031 (TouchOff)
N0160 G00 Z0.1500
N0170 M03 (Torch Fire)
N0180 G04 P0.400
N0190 G01 X1.1676 Y1.4567 // x moved by 0.0001
N0200 G01 Z0.0600 F150.0
N0210 M05 (Torch Off)

This dimple test program is a perfect example of the issue. See in the video with THC on with the increasing pierce delay you can see that the dwell timer starts with ARC OK. The ARC OK never lights (the plasma cutter is off for this test).

https://www.youtube.com/watch?v=SyR8VoHnUBw

Code: Select all

(PIERCE / DIMPLE SETTING TEST)
(distances in mm as shown)
(time in mSec as shown)

#1 = 0.6 (x spacing between pierces mm)
#2 = 0 (y spacing between pierces mm)
#3 = 100 (pierce time increment mSec)
#4 = 0 (start pierce time delay mSec)
#5 = 1000 (end pierce time delay mSec)
#6 = 1031 (touchoff macro number)
#7 = 0.150 (pierce / dimple height mm)
#8 = 205 (THC ON macro number)



#10 = [#5 - #4]
#10 = [#10 / #3]
#10 = [#10 + 1]

#11 = #1
#12 = #2

G90 G64
G92 X0 Y0  (set temp offset X&Y)
M#8 (THC ON)

M98 P2000 L#10

G0 X0 Y0
G92.1

M30



O2000 (sub-program to repeat)
M#6 (touchoff)
G0 Z#7 (retract to pierce height)
M3 (fire torch)
G4 P#4
M5 (torch off)
G0 Z1 (Z safe retract)

#4 = [#4 + #3]

G0 X#11 Y#12 (move to next pierce point)
#11 = [#11 + #1]
#12 = [#12 + #2]
M99



It is true that there is no movement immediately after M3, but it still exists before M5.

laki wrote:It is true that there is no movement immediately after M3, but it still exists before M5.

2.png

Yes I agree, although it does move in the Z plane but not the X/Y. That is why I suggested trying it right after the delay pause. I think your suggestion is valid and I will test.