Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: mrpeja on May 19, 2010, 01:56:05 PM
-
Last days I experienced serious problem. I have build plasma table one year ago and works well. But I want to convert it to oxy fuel cutter. Very often I need to activate Run reverse. And there is big problem.
First I press Hold and then Run reverse. Program starts reverse, but sometimes instantly and sometimes after couple of lines, Z axis goes UP to Rapid clearance and stays here and I don't have control anymore. I have test everything I can remember, but problem persists.
So I need help.
I'm not sure where is the problem: in Mach3 or in SheetCam or I missed something to do in my config or in sequence of pressing buttons or in place where to press Hold, or...
I use Sheetcam post processor THC300 G31 and floating head switch.
Mrpeja, licensed user
-
this is exactly my problem
-
Do you have SafeZ turned on?
-
I think the problem IS that mach does not know how to deal with the TOM routine(top of material) and the constant resetting of the Z with G92.
In order for the TOM with a G31 OR G28.1 to work it HAS to cycle the code first to find the surface then Reset the Z with the G92. SO when the planner runs the code backwards it does not know to CYCLE the TOM routine first as it processes the code in reverse.
Here it also does not cycle the Torch start/stop properly it just leaves the torch on til the EOF.
We have learned to just repeat the section of code rather than ReverseRun.
Hope that helps
-
From my understanding "Reverse Run" will also NOT read MCodes and such.
If you press the stop button rather then resuming from a FeedHold do you get the same results?
-
i do , Z goto up and Z-safe is off.
Very strange.
amir
-
To zealous: when I press Stop instead of Hold, than all is lost, much worse than Hold.
To BR549: Do you have idea how to solve problem with G31 and G28.1 for oxy fuel and plasma use?
To Ger21: I have SafeZ turned OFF.
-
Sorry but to my knowledge there is NO solution for Jet cutting using rev run. The only solution is to feedhold, stop then reset the last section to recut and restart the cut.
The fix would have to be done at the CORE LEVEL in mach.
(;-) TP
-
Hi BR549,
Thx for the reply. Maybe someone in charge could do things at the CORE LEVEL in Mach.
Community will appreciate this.
Before this happens, please explain this: fedhold, stop, reset last section and restart the cut with more details.
For now, I do something like this in SheetCam, extracting parts being cut and start new job.
Maybe you know simple way to do?
-
I have THC, and have "FAULT pin" .
if torch was turn off then fault is ON. we connect fault pin to buttom "feedhold" and if in While cut torch was off, then Automatically machine pause and we repair our problem
I think the pause is more safe than the reverse run
It is practical ?
-
Some years ago, I worked with a basic software(For several weeks) that was written by a family for plasma device . The button "pause" and "reverse run" worked very very well and no problems were not created anywhere (Even in the curves)
The software was very very basic. I do not know why these two button mach3 isnt safe.
-
To properly maintain position on the table you would do
Feedhold (until motion stops)
Stop
This allows Mach to come to a controlled stop witout LOOSING position.
Then you can do what ever you need to do to fixe the problem.
Then you can move back into position at a start point ahead of where you had a problem then use Set Next Line and RUN.
We have a special macro we run called restart that does all of this automatically so IF there is a cutting problem it is easy to remedy.
That way we don't have to rely on reverse run.
Hope that helps, (;-) TP
-
Hi BR549,
Good solution.
I have a question: vouldn't Stop command abort entire job?
And, can you send me this macro you have to remedy the problem?
mrpeja
-
It depends on how you have mach setup as to how it reacts to stop.
BUT even with that jet cutting is very basic 2d cutting rarely would you see anything other than basic lines and arcs. SO that being you can restart anywhere without having to parse throught the entire program to get all the proper modes reset(run from Here).
You can simply restart with set next line fire the torch and run.
I will dig out the code for restart. It is a 2 part process one button to stop thye machine safely saveing all the important info to variables. Then a another button to return to the restart point , fire the torch and restart 1 line previous to the original startpoint.
This gives you a point between buttons that you can correct the torch problem.
Just a thought, (;-) TP
-
To BR549 :
Solution seems to be very good.
please share macro
-
OK this is the first macro that stops the machine and gathers data to return. You may have to modify it to soot your machine and process
***********************************************************
'F13 Feedhold/stop to check torch
DoButton(1) 'Feedhold
While IsMoving 'Wait for movement to stop
Sleep(100)
Wend
DoSpinStop ' Turn OFF torch
Sleep(100)
SetVar(601,Getdro(2)) 'Setvar to Zpos
Sleep(100)
DoButton(3) 'Set Stop
Sleep(100)
DoOemButton(104) 'Move to SafeZ
While IsMoving()
Sleep(100)
Wend
SetVar(602,GetDro(0)) 'Setvar to Xpos
SetVar(603,GetDro(1)) 'SetVar to ypos
SetVar(604,GetDro(18)) 'SetVar to Feedrate
SetVar(605,GetDro(16)) 'SetVar to CurrentLine#
End
This is the second macro that returns the machine to work. You may have to modify it to soot your machine or process
**************************************************************
'F14
DoOemButton(104) 'Go To SafeZ
While IsMoving()
Sleep(100)
Wend
Code"G0 X#602 Y#603" 'Return To Stop Point
While IsMoving()
Sleep(100)
Wend
Code"G28.1 Z0.500" 'ReREF Head to TOM
While Ismoving()
Sleep(100)
Wend
Code"G92 Z0.000" 'Reset Dro
sleep(100)
Code"G0 Z#601" 'Return Z to stop Point
While IsMoving()
Sleep(100)
Wend
SetDro(16,Getvar(605)) 'Reset SET NEXT LINE #
Sleep(100)
SetDro(18,GetVar(604)) 'Reset Feedrate
Sleep(100)
DoOemButton(156) 'Run SET NEXT LINE
Sleep(100)
DOSPINCW 'Refire Torch
Sleep(100)
DoButton(0) 'Resume Program from Stop Point
End
Hope it helps
-
i test this macros in PC ,It seems M113 is ok but when run M114 :
feedrate change Be more.
what ?
in addition i modify M114:
SetDro(16,(Getvar(605) -1) ) 'Reset SET NEXT LINE #-1
No problem there?
-
Hi BR,
Why Feedrate changes after executing M114 macro?
-
another problem:
-
IF your system does NOT use an ARC OK signal then you may have to add more dwell time before the RUN signal is given . That will give the machine time to get the torch fired and steady BEFORE movement occurrs
DoOemButton(156) 'Run SET NEXT LINE
Sleep(100)
DOSPINCW 'Refire Torch
Sleep(1000) 'ADD MORE TIME HERE
DoButton(0) 'Resume Program from Stop Point
End
AS to the feedrate? Are you using feedrate override?? IF so then the stop command may cancel out the FRO. The macro copies the Current Feedrate then just applies it back so the values should remain the same.
-
thx for reply
we use "SetVar(604,GetDro(18)) 'SetVar to Feedrate"
then should not feedrate change but what?
in addition please see my image and read text. I questioned about what torch is ON when nozzle dont reach to T spot ?
-
let me explain:
When the torch is turned off During cutting ,nozzle moves a path without cut .
When we use these two macro.in fact with M114 The nozzle continue to move from Point that was stopped.
i change macro 113 to form:
""" SetVar(605,(GetDro(16)-1)) 'SetVar to CurrentLine# """
With this change, nozzle move to first line of unfinished.
now my problem :
when nozzle go back to first line of unfinished ,torch is ON
how i could change macro 114 for the nozzle go back and stop here then torch ON ,DELAY And finally START.
please guide me.
-
OK ARE you testing this on a machine OR testing it on a PC without the Mach driver running??
IF the driver is NOT running then many things may NOT work correctly as the driver controls many key timing points.
IF the torch is shutting OFF before the stop point OR turrning ON before it gets to the restart point,
then MACH is "ignoring" the While Ismoving() command. I can't fix that for you(;-) that would be an internal mach VB problem
*** You may try increasing the Sleep Values to 1000 or 2000
I don't see "either" of the problems running it here on a live machine. But i am on an older version of mach that may not have the problem.
-
OOPS pushed the wrong button
-
i have ArkOk. when torch is shutting OFF ,ArkOk cause stop mach.From here explain.
please Describe How to act ? ( i mean two macro)
For better understanding.
i test in pc with mach driver
-
ARE you running in DEMO mode?
-
no . i have license
I think that you not read my previous posts.
-
i solve feedrate problem .
"""SetOemDro(58,GetVar(604)) 'Reset Feedrate
but Still remains one problem.
i use Arkok ,and when torch shutting off ,Movement ends. now i press button M113.
for example in line 111 trigger Macro113 .
i change code to :
SetVar(605,GetDro(16)-1) 'SetVar to CurrentLine#
With this change nozzle go back first line 111 and So far is ok, but issue is During Move through middle line111 to the first line111 the torch is ON.
How i could repair this problem ?
sorry for bad english and thx all
-
IF I read you correctly then just remove the -1 and just restart where you left off.
-
i dont understand your mean :(
i generate a g-code file with sheetcam(THC G31) and again test it, The result was strange.
feedrate again change. im confuse.
what? sometime feedrate change ,sometime not change and is ok
its possible that you test it ?
-
see video
i set feedrate 700 ,i have two button "M113 pause" and "M114 resume"
when i press M114 feedrate change to 2000~2500
in addition i attach .tap
and i use this macro :
'F13 Feedhold/stop to check torch
sleep(100)
DoButton(1) 'Feedhold
While IsMoving 'Wait for movement to stop
Sleep(100)
Wend
DoSpinStop ' Turn OFF torch
Sleep(100)
SetVar(601,Getdro(2)) 'Setvar to Zpos
Sleep(100)
DoButton(3) 'Set Stop
Sleep(100)
SetVar(602,GetDro(0)) 'Setvar to Xpos
SetVar(603,GetDro(1)) 'SetVar to ypos
SetVar(604,GetDro(18)) 'SetVar to Feedrate
SetVar(605,GetDro(16)) 'SetVar to CurrentLine#
End
and
'F14
Code"G0 X#602 Y#603" 'Return To Stop Point
While IsMoving()
Sleep(100)
Wend
Code"G31 Z-100" 'ReREF Head to TOM
While Ismoving()
Sleep(100)
Wend
Code"G92 Z0.000" 'Reset Dro
sleep(100)
Code"G0 Z#601" 'Return Z to stop Point
While IsMoving()
Sleep(100)
Wend
SetDro(16,Getvar(605)) 'Reset SET NEXT LINE #
Sleep(100)
SetDro(18,GetVar(604)) 'Reset Feedrate
Sleep(100)
DoOemButton(156) 'Run SET NEXT LINE
Sleep(100)
DOSPINCW 'Refire Torch
Sleep(100)
DoButton(0) 'Resume Program from Stop Point
End
-
I do test it, about every day here. I have used it for about 1 1/2 years now and I don't see your problems here. Not saying that you don't have the problems.
-
Please guide to get the desired result.
are you test my attach ?
are you use sheetcam? if yes which post processor ?
-
OK as a test just commnet out the lines of code that store and reset the feedrate
In M113
' SetVar(604,GetDro(18)) 'SetVar to Feedrate
In M114
' SetDro(18,GetVar(604)) 'Reset Feedrate
' Sleep(100)
The feedrate routine is only there in case something you ran between button pushes that changed the feedrate
-
then i must delete it and again do test?
in addition attach my .SET
-
i test without feedrate but result is same.
i do manually this macro , all thing is ok( i mean : first pause then stop then "SET NEXT LINE" and start)
but when i run macro with button ,feedrate change
i was crazy.
-
(;-) I don't see anything in the button code OR GCODE that should cause what you see. Looking at the video "MACH" is violating the set feedrate for a short while THEN goes back to normal.
You guess is as good as mine at this point.
I will search for the problems as I get time.
In the meantime you need to be carefull with it IF you use it.
WHAT version of MACH are you running?
-
very thanks for help
i use mach3 VER 3.042.020 +sheetcam G31 +THC
are you do test my code on your PC .?
not problem ?
-
Attach your xml as well please as it will make things easier to test.
Hood
-
I take it your machine is SETUP in metric units?
I will try a setup in metric units to see if it makes a difference.
-
OK I moved to another computer with the latest dev ver. AND I now see what you are seeing.
THat is really strange(;-) I can't say I have every seen that one before. Even doing the steps manually without the macro I can get it to do the same thing.
THere is NOTHING I can do code wise to fix that problem it is internal with mach.
Sorry
-
thx for try
i attach .XML .SET and .tap
BR549 -
what version of MACH are you running?
i want use it version
and video in vimeo:
http://vimeo.com/11992679 (http://vimeo.com/11992679)
-
i think find problem :
Code"G0 X#602 Y#603" 'Return To Stop Point
and
Code"G28.1 Z0.500" 'ReREF Head to TOM
-
Testing here shows the problem STARTS in the FEEDHOLD, at that point I loose control of the jogging feedrate it jogs very slow. Then when I try to apply Gcode at the correct feedrate after that it runs the G1 at JOGGING feedrates until it comes to another Fcall and returns to normal.
AS long as I do not JOG in between buttons it works ok BUT the whole idea is to jog away to a work point and fix the torch problem(consumables)
SO at this point the routine is BUSTED please do not use it.
I will try to work on a workaround but I don't how with only Gcode to work with. I have tried resetting the G0 and G1 to force Mach to reset BUT it did not work either.
Sorry
-
thx.
but when i delete Line: Code"X#... Y#..." it work well
in addition ,dont work even if dont JOG
-
OK I have tried it every way I know of . Even using the internal mach Remember and return routines. Something in the Feedhold/stop is corrupting the jogging and feedrate control when USED with VB .
So until it is fixed this handy routine is a bust in the new versions. I heard Brian was working on a new routine for plasma so you could feedhold/jog.
Sorry
-
I think that Mach have big problem with plasma.
with G31 & G28.1 & macro & reverse run
Are problems that almost impossible work with Mach.
I am very sad for these problems.
-
NO mach does NOT have a big problem with plasma cutting I use it every day. The G31 or G28.1 TOM routines work fine. YES there are quirks BUT in 40 years of cutting I have NEVER seen a system that did not have quirks.
You already know that reverse run does not work so why keep beating on it. I would suggest learning HOW to properly plan and setup your cuts SO you would not need to do a reverse cut to correct a poorly planned cut. (;-)
If you can't plan your consumeables change outs to ensure good cutting OR keep the air supply clean and dry then please DON""T blame mach, look in the mirror for your problem.
There are plenty of PROVEN manual restart routines that are used every day that allow you to do an OCCASIONAL restart as needed.
Sorry but enough is enough
-
I think that you want to hide the facts .
I know the style of cutting, but the problem is that the my customer ,do not accept this issue.
They think the economy and want to make the most use of iron sheet.
This reason is that During cutting a lot of events occur ,at this time require that they return and solve the problem.
Amir
-
Amir now would be the time for YOUR customers to invest in a commercial controller. I know that mazaks,Seimans and Fanuc can do "exactly" what you THINK they need. AND they are only about $10k per machine(;-) plus integration cost.
I have been cutting for about 40 years now so I might have an idea about how it works and HOW to do it at the best economic RETURN on my Dollar.
Now in all fairness there are some things that mach does not do as well as the $10k controllers BUT for $175 what exactly are you expecting???
BUT keeping in the SPIRIT of mach and the mach forum AND after many gallons of midnight to daylight oil I may have a solution(;-)
This has been working this morning without fail for several hours of testing with the latest MACH lockdown version V.040.
And you know the routine"Use it at your own risk" AND you may need to modify it to suite your machine or process.
-
'Stop Button Feedhold/stop to check torch
DoButton(1) 'Feedhold
While IsMoving 'Wait for movement to stop
Sleep(100)
Wend
DoSpinStop ' Turn OFF torch
Sleep(1000)
DoButton(286) ' Set positions
Sleep(1000)
DoButton(3) 'Set Stop
Sleep(1000)
SetVar(604,GetDro(18)) 'SetVar to Feedrate
SetVar(605,GetDro(16)) 'SetVar to CurrentLine#
Code"G0 Z1.000" 'Move to a SafeZ
While IsMoving()
Sleep(1000)
Wend
Code"(Stop Routine Complete)"
End
'***************************************************************************************************************************************X
'Restart Button to return to work
Code"G1 Z1.000 F#604" 'Go To a SafeZ
While IsMoving()
Sleep(1000)
Wend
SetDro(16,Getvar(605)) 'Reset SET NEXT LINE #
Sleep(100)
SetDro(18,GetVar(604)) 'Reset Feedrate
Sleep(100)
'************************* Setup TOM to suite machine
'Code"G28.1 Z0.500" 'ReREF Head to TOM
'While Ismoving()
'Sleep(100)
'Wend
'Code"G92 Z0.000" 'Reset Dro
"Code"G1 Z0.150"
'Code"G92 Z0.000"
'sleep(100)
'*************************************************
DoOemButton(285) 'Return to stop position
While IsMoving()
Sleep(1000)
Wend
Code"G1 Z#601 F#604" 'Return Z to stop Point
While IsMoving()
Sleep(1000)
Wend
DOSPINCW() 'Refire Torch
Sleep(100)
DoButton(0) 'Resume Program Run from Stop Point
Code"(You are now back ONLINE cutting )"
End
-
I have been cutting for about 40 years now so I might have an idea about how it works and HOW to do it at the best economic RETURN on my Dollar.
I have to accept you're a master, I confess in front of you I am human illiteracy.I am young and inexperienced
Please share with our valuable experiences and idea about cutting .
Now in all fairness there are some things that mach does not do as well as the $10k controllers BUT for $175 what exactly are you expecting???
I accept, you say right
This has been working this morning without fail for several hours of testing with the latest MACH lockdown version V.040.
very thx for try
-
I might not know ALL the ways it can be done, But I do know most of the ways that it can be messed up.
If you have a problem just ask for the help, Baggering the product does not help it only gets you fussed at(;-)
Been there done that as well.
-
when we use this Command (DoOemButton(285) 'Return to stop position) on the page is displayed warning.Like the image below
I use modbus pendant and I dont want verified this warning as manually( Because I am away from PC) .
Is there a way that it does not show this warning?
Amir
-
(;-) That was why we had the OTHER version as one did not have to deal with the restat window, But is does not seem to work on your end.
Right now I don't have any other suggestions other than working with the old version and see what it takes to make it work on your end.
(;-)