Author Topic: Z Axis Feedhold Reverse Run problem  (Read 6075 times)

0 Members and 1 Guest are viewing this topic.

Offline kanowee

  • Active Member
  • Posts: 3
    • View Profile
Z Axis Feedhold Reverse Run problem
« on: November 21, 2012, 06:26:55 AM »
Hello,

Have a plasma CNC machine, running MACH3 .066. I'm using Sheetcam with the THC300-G31 post processor.

When a plasma machine loses the plasma arc, there is a need to resume the cut from this exactly postion in order not to loose the cutted part. My machine have a floating Z axis, connected to a probe switch.

I'm doing the following:
1- The machine loses the plasma arc, them the motion stop. So I press feedhold, then reverse run to make the machine back to the lost arc point.
2- The X and Y axis reverse OK, but the Z axis go up, instead of staying at 0.00 coordinate.  The amount of Z that go up, could not understand. Sometimes it go up 7mm, sometimes 4.5mm, sometimes fractioned units like 5.85mm.
3- If I try to manually lower the z axis and then Zero it manually, a "Preparation to move" dialog appears, making the process more difficult to the operator. And the Z axis continues to go up if it do not reached the "desired" Mach3 position.

I think that there must be an error with my Gcode, or the G92 codes are telling Mach some offset that I dont need.

Resuming: The machine must not aleatory move the Z axis when clicking Reverse Run.

Here is a simple code:

N0000 (Filename: letra a.tap)
N0010 (Post processor: Plasma THC300 - G31.scpost)
N0020 (Date: 21/11/2012)
N0030 G21 (Units: Metric)
N0040 G53 G90 G40
N0050 F1
N0060 S500
N0070 (Part: letra a)
N0080 (Process: Offset externo, 0, T7: CHAPA 18 = 30A = 123V)
N0090 M06 T7  (CHAPA 18 = 30A = 123V)
N0100 G00 X37.1672 Y55.5242 Z20.0000
N0110 G31 Z -100 F500.0
N0120 G92 Z0.0
N0130 G00 Z3.0000
N0140 G92 Z0.0
N0150 G00 X37.1672 Y55.5242 Z1.5000
N0160 M03
N0170 G02 X32.5154 Y58.3262 I-0.9249 J3.7269 F2050.0
N0180 G03 X31.3515 Y58.3295 I-0.5823 J-0.1445
N0190 G01 X26.2010 Y38.0647
N0200 G03 X26.1999 Y37.7736 I0.5815 J-0.1478
N0210 G01 X29.1288 Y25.8648
N0220 X23.6707
N0230 G03 X23.0909 Y25.4191 I0.0000 J-0.6000
N0240 G01 X20.4083 Y15.3403
N0250 G03 X20.9826 Y14.5860 I0.5798 J-0.1543
N0260 G01 X32.0952 Y14.4832
N0270 X34.2447 Y4.8691
N0280 G03 X34.8302 Y4.4000 I0.5855 J0.1309
N0290 G01 X45.1313
N0300 G03 X45.7136 Y5.1445 I0.0000 J0.6000
N0310 G01 X32.5154 Y58.3262
N0320 M05
N0330 G00 Z20.0000
N0340 X17.1087 Y70.6367
N0350 Z1.5000
N0360 M03
N0370 G02 X19.8784 Y65.9655 I-0.9508 J-3.7204
N0380 G01 X19.7630 Y65.5141
N0390 X4.4187 Y5.4702
N0400 G03 X4.9872 Y4.7218 I0.5813 J-0.1486
N0410 G01 X15.0737 Y4.5074
N0420 G03 X15.6682 Y4.9601 I0.0128 J0.5999
N0430 G01 X30.9052 Y65.2184
N0440 G03 X30.3235 Y65.9655 I-0.5817 J0.1471
N0450 G01 X20.3443
N0460 X19.8784
N0470 M05
N0480 G00 Z20.0000
N0490 M05 M30

Thank you for any help.

« Last Edit: November 21, 2012, 06:29:05 AM by kanowee »

Offline BR549

  • Mach4 Alpha
  • Posts: 6,855
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #1 on: November 21, 2012, 12:32:05 PM »
YES the RFH and the RR is a known problem with Mach3 and plasma.  

A work around solution is to call the TOM(top of material routine) from a Macro. THEN the RevRun and RFH and Pause resume with axis movement will work correctly as well.

The Prep Move is required for safety reasons and that will not change.  ANYTIME you move off position in a paused mode you will get that Prep Move Box

I have asked Brian if it can be fixed. We will have to wait and see.

(;-) TP
« Last Edit: November 21, 2012, 12:39:27 PM by BR549 »

Offline kanowee

  • Active Member
  • Posts: 3
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #2 on: November 21, 2012, 02:41:38 PM »
I took the afternoon trying to workaround the problem.

Instead of using the G92, I made a macro for setting the machine coordinates to zero, when the Z touch the plate.

With this, the Z axis machine and work coordinates are equal, and mach does the Reverse Run very nice.

Here is the Gcode with the workaround:

N0000 (Filename: letra a.tap)
N0010 (Post processor: Plasma THC300 - G31.scpost)
N0020 (Date: 21/11/2012)
N0030 G21 (Units: Metric)
N0040 G53 G90 G40
N0050 F1
N0060 S500
N0070 (Part: letra a)
N0080 (Process: Offset externo, 0, T7: CHAPA 18 = 30A = 123V)
N0090 M06 T7  (CHAPA 18 = 30A = 123V)
N0100 G00 X37.1672 Y55.5242 Z20.0000
N0110 G31 Z -100 F500.0 (probe touch)
N0120 M668 (Set Mach Zero and Work Zero Macro)
N0130 G00 Z3.0000 (Z switch offset)
N0140 M668 (Set Mach Zero and Work Zero Macro)
N0150 G00 X37.1672 Y55.5242 Z1.5000
N0160 M03
N0170 G02 X32.5154 Y58.3262 I-0.9249 J3.7269 F2050.0
N0180 G03 X31.3515 Y58.3295 I-0.5823 J-0.1445
N0190 G01 X26.2010 Y38.0647
.
.
. and the code goes on.

Don´t think its the best aproach, but´s it´s finally working. Run Reverse and Cycle Start without problems.

Hope to help other guys with the problem.

Here is the Macro:
SetMachZero(2)
DoOemButton(1010)

Will try the TOM routine, think will best suit my needs.

Thank you for the help

Offline BR549

  • Mach4 Alpha
  • Posts: 6,855
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #3 on: November 21, 2012, 02:47:53 PM »
'TOM macro M1234
Code" G31 Z -100 F500.0 "
Code" G92 Z0.0 "
Code" G00 Z3.0000 "
Code" G92 Z0.0 "
end

Offline kanowee

  • Active Member
  • Posts: 3
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #4 on: November 21, 2012, 04:03:49 PM »
So calling a macro instead of inserting the code directly inside the Gcode, makes Mach Reverse Run OK? Strange.

This TOM macro is exacly what the PostProcessor does, and it´s exactly what causes the problem. So I ripped of this and make the SetMachZero macro.

Will try this, calling the macro, and see what happens.

Thank you,

Offline BR549

  • Mach4 Alpha
  • Posts: 6,855
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #5 on: November 21, 2012, 04:16:30 PM »
When you invoke the routines Mach3 checks for all the modal  values and GETS confused with the constant G92 offsetting and does not know how to handle it and the G31 routine during the post check of the modal values.

Putting all of that problem code inside the macro stops the pretesting of the code as MACH3 does NOT prerun macros for modal code values such as the G92.  In plasma the actuall Z offset value is not important as it is constantly being reset with each TOM routine ran.

IF you notice in a long program with lots of starts the actual Z offset gets larger and larger each time it cycles in the Gcode.

It would be NICE if we had a new G CODE that did the TOM routine . That way it could be blocked when the RR or RFH routines are ran.

OR maybe Brian will come up with an answer(;-).

Just a thought, (;-) TP


Offline BR549

  • Mach4 Alpha
  • Posts: 6,855
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #6 on: November 21, 2012, 04:28:24 PM »
The nice part about only using 1 macro is that it can be programmed for Sheetcam. Values like switch offset can be applied directly to the macro. You have up to 3 vaules you can bring in.

M1234 P********* Q********* R*********

Just a thought, (;-) TP

Offline CREA

  • Holding
  • Posts: 1
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #7 on: August 30, 2013, 05:55:41 PM »
Hi, I'm having the same problem but I don't know how to do the macro... can you send it to me? so I can do some cuts?

Offline Bradnificent

  • Holding
  • Posts: 2
    • View Profile
Re: Z Axis Feedhold Reverse Run problem
« Reply #8 on: February 07, 2019, 06:11:53 AM »
Hi kanowee can you please explain how and where do I insert the macro in mach3 as I have the same problem as you

Bradley