PDA

View Full Version : Need Help! Question obout code within my Gcode



bigdipper
09-22-2014, 03:24 PM
I believe this is the best place to start trying to find out what is going on. My problem is that I have a file that I cannot get to cut on my plasma cnc. It has in the past worked but something has been changed and I cannot find it. I have another file that cuts perfectly so I printed both of the Gcodes and began to compare them. What I am seeing is there are added code at the first of the progams or maybe they just have different numbers on the code. For example, the one that works has an s3115 and the one that doesn't has a s3116. There is an additional code of s445 on the one that doesn't. The GO1 on the working file is GO1 Z0.0600 F30.0 and the nonworking is GO1 Z0.0600 F1.9685. I have looked for the definitions of s and F but have been unable to find anything. This is probably simple to some of you but yes,, I am a newby. One last thing is that when it gets to the first pierce and the pierce is made the torch will go out but machine continues to operate. It is very puzzling to me that right after having this problem I can load the other program and it cuts perfectly. Would appreciate any help you might give. I am stumped. Thanks in advance.

Bill in Arkansas

awerby
09-22-2014, 03:48 PM
On a mill, the "s" word is the spindle speed in RPMs, while the "f" word is the feedrate in units per minute. I'm not sure what "s" signifies to a plasma cutter, though. One thing that strikes me about the G-codes you quoted, though: you seem to be using an alphabetical "O" in the G01 command where you should be using a zero ("0"). Have you tried editing the g-code to get it to work?

mactec54
09-22-2014, 03:48 PM
bigdipper

S=Speed (spindle Speed) F= Feed-rate at what the axes will move at

There must be something else, as this is not what is causing the problem

Cut paste the 2 programs, what control are you using

bigdipper
09-22-2014, 04:34 PM
Here is the first bit of my code:This is the one that won't work. Pierces and torch goes out I am using mach 3 with sheet cam have a DHTC IV Ethernet height controller

N0020 (Post processor: DTHC-HYT-TAP_SoftPierce+Marker.scpost11.scpost)
N0030 (Date: 22/09/2014)
N0040 G20 (Units: Inches)
N0050 F1
N0060 G53 G90 G40
N0070 (Part: rolla_bulldog2)
N0080 (Operation: No Offset, Colour 7, T1: 16 gauge Mild Steel)
N0090 (tool number: 1 Feedrate: 225)
N0100(Preset Volts: 116 Preset AMPS: 45)
N0110 ( Air Pressure Preset: 85)
N0120( Suggested Tip Size: 45 , Default DTHC Delay )
N0130 ( Soft Pierce : 50 percent )
N0140 S900
N0150 M22
N0160 S3116
N0170 M22
N0180 S445
N0190 M22
N0200 S885
N0210 M22
N0220 M00
N0230(Check the DTHC Settings Hit RUN to continue)
N0240 G00 Z0.5000
N0250 X1.4206 Y0.6680
N0260 G28.1 Z0.02 (Start Touch-Off )
N0270 G92 Z0.0
N0280 G00 Z0.1520 (Switch Offset Lift)
N0290 G92 Z0.0
N0300 G00 Z0.1500 S15 (Soft Pierce Active)
N0310 M03
N0320 G01 Z0.0600 F1.9685
N0330 S20
N0340 G01 F225.0
N0350 G02 X1.4748 Y0.6701 I0.0629 J-0.9301
N0360 G01 X1.5869 Y0.6520
N0370 G02 X1.7736 Y0.5864 I-0.2471 J-1.0025
N0380 X1.8720 Y0.5332 I-0.2352 J-0.5518
N0390 X1.9184 Y0.4560 I-0.0256 J-0.0680
N0400 X1.9042 Y0.4331 I-0.0842 J0.0365
N0410 X1.8708 Y0.3985 I-0.2255 J0.1842
N0420 X1.7295 Y0.3029 I-0.3506 J0.3659
N0430 X1.2708 Y0.2185 I-0.4628 J1.2269
N0440 G01 X1.2613 Y0.2181
N0450 Y0.2652
N0460 G02 X1.2674 Y0.6756 I7.6938 J0.0907
N0470 G01 X1.2676 Y0.6766
N0480 X1.2682 Y0.6765
N0490 G03 X1.4206 Y0.6680 I0.1180 J0.7426
N0500 M05
N0510 S10 (DTHC is off)
N0520 G00 Z0.5000
N0530 X1.4491 Y0.8871
N0540 Z0.1500
N0550 Z0.1500 S15 (Soft Pierce Active)

Here is the one that does work

:N0010 (Filename: hornyG.tap)
N0020 (Post processor: DTHC-HYT-TAP_SoftPierce+Marker.scpost11.scpost)
N0030 (Date: 15/08/2014)
N0040 G20 (Units: Inches)
N0050 F1
N0060 G53 G90 G40
N0070 (Part: hornyG)
N0080 (Operation: No Offset, Colour 7, T1: 16 gauge Mild Steel)
N0090 (tool number: 1 Feedrate: 350)
N0100(Preset Volts: 115 )
N0110 ( Air Pressure Preset: 85)
N0120( Suggested Tip Size: 45 , Default DTHC Delay )
N0130 ( Soft Pierce : 50 percent )
N0140 S900
N0150 M22
N0160 S3115
N0170 M22
N0180 S885
N0190 M22
N0200 M00
N0210(Check the DTHC Settings Hit RUN to continue)
N0220 G00 Z0.5000
N0230 X5.3531 Y1.0956
N0240 G28.1 Z0.02 (Start Touch-Off )
N0250 G92 Z0.0
N0260 G00 Z0.1520 (Switch Offset Lift)
N0270 G92 Z0.0
N0280 G00 Z0.1500 S15 (Soft Pierce Active)
N0290 M03
N0300 G01 Z0.0600 F30.0
N0310 S10
N0320 X5.3533 Y1.0959 F350.0
N0330 S10
N0340 X5.3456 Y1.0845
N0350 S10
N0360 X5.3531 Y1.0956
N0370 S10
N0380 M05
N0390 G00 Z0.5000
N0400 X6.6528 Y4.2898
N0410 Z0.1500
N0420 Z0.1500 S15 (Soft Pierce Active)

These are not the complete code but should be enough to compare and maybe see what is happening.
Thanks

mactec54
09-22-2014, 06:08 PM
bigdipper

What control are you using,who's machine, different company s use the code differently, M22 turns off Continuous Path

bigdipper
09-22-2014, 06:58 PM
no manufacturer, I built the machine from the ground up. I have a gecko G540 together with a CANDCNC MP3500 Ethernet THC

mactec54
09-22-2014, 08:32 PM
bigdipper

Your control is Mach3 with Candcnc screen set, you should have everything from Candcnc as to what codes do what, here is there sample program that tells you what some of the codes do

Torchhead
09-23-2014, 07:58 PM
The S codes in the DTHC product line (including your Ether-Cut ) are custom and only work with the MACH profiles and our plugins. The list of what the codes do is in our document Using Dynamic Cut Control with SheetCAM and DTHCII- REV3 located in the Manuals page of the website. Pretty boring document unless you are into deep detials. The M22 is a brief pause because you cannot load back to back S codes For example the S3115 (S3 is a preset volts call) sets the Preset Volts at 115 while the S3116 sets it at 116...hardly a big change. The S4 series sets the Cut Current (IF you have the HyT-Connect RS485 SIM option) otherwise it does nothing. A lot of the toolsets provided may need some values changed.

First thing: Go to the manuals page and download the Advanced Posts at the very bottom and get the 11b version and run the job through that
Second:: Turn off the Soft Pierce. You don't need it on 16ga!
Third: there are a lot of arcs int he first one and none in the second is the main difference
Fourth: post on the CandCNC Support Form under Software support. The POSTS are very custom, the codes are not "standard" in all cases and the DTHC does things no other MACH based THC can do.including talk to the Hypertherm though the optional RS485 port. All of those things are outside typical G-Codes and need to be looked at by a CandCNC person
Fifth: Did this cut before with the MP3500-DTHCIV Ether-Cut or was it an earlier control?


If you need to you can send me the SheetCAM jobs and let me see what they do here

TOMcaudle
www.CandCNC.com