-
Hello,
This is my 1st post in Machsupport.
I have a 3 axis cnc router and I want to convert it to a plasma machine, so far this is what I have done:
http://s1220.photobucket.com/albums/dd459/happytriger2000/Machsupport/?action=view¤t=M4H02695.mp4
I wan the Z axis to do the same as in this video:
http://asooke.com/videos-cnc-plasma-with-thc-and-floating-%5Ban5HYBQWTpg%5D.cfm
Can anyone guide me from this point onwards?
thanks,
-
You can set it up one of two ways using the G28.1 method OR use the G31 method.
With the G28.1 method you set up your floating head as the Z home and have it home toward the bed. Then the Cam that you use must generate the following type code.
N0120 G28.1 Z0.50
N0130 G92 Z0.0
N0140 G00 Z0.1370
N0150 G92 Z0.0
N0160 G00 Z0.2000
With the G31 method you setup the floating head as a Probe then you cam must generate code like
N0120 G31 Z -100 F19.685
N0130 G92 Z-0.0800
N0140 G00 X5.5505 Y9.8813
N0150 Z0.0000
Hope that helps, (;-) TP
-
Hi Br549,
Thanks.
(http://i1220.photobucket.com/albums/dd459/happytriger2000/Machsupport/Flotinghead3.jpg)
I'm still hesitating on what the exact vulue should it be for the distance between the MicroSwitch and the Torch collar?
Currently is 13.7mm.
Should this distance be the thickness of the plate that going to be cut, 6mm,?
thanks,
-
That distance PLUS the amount of travel in the switch is used to move the head BACK up so the tip of the torch is exactly at the top of the material.
Using the G28.1 method and assuming the distance + the travel equals .250" NOTE: your Cam program will have a place for THAT setting
G28.1 Z.50 ' references the head down until it trips the switch
G92 Z0.000 'Sets that point to ZERO
G0 Z0.250 ' Moves the head UP the amount of the head travel + switch movement
G92 Z0.000 ' Sets that position to ZERO, that will be TOP of the material,
G0 Z.100 ' Move the head up to a clearance position
NOW you head is referenced to the TOM and you are ready to start a cut.
Note that most CAMS rereference the TOM every so many inches of torch travel . If the setting is every 50" then the next torch start after the machine has cut 50" then it will ref the head before it cuts again.
Collar Distance?? Make it anything you like (;-) normally the closer the better.
Hope that helps (;-) TP
-
Thanks again BR549,
I'm new to Sheetcam, still using a demo version downloaded yesterday.
I was wondering if it's possible to use Mach 3 to do the Z axsi floating offset without Sheetcam?.
Like the Mach blue screenset that has the Autotool zero feature, Link:http://www.cnczone.com/forums/cnc_wood_router_project_log/36099-another_aussie_auto_tool_zero.html,
instead of touching the plate, Z home switch is tripped, reset Z DRO to zero, raise Z to Swtichoffset value so tip is setting on top of material, reset Z to zero as top of material, raise Z to pierce height, fire torch.
I haven't used a plasma machine before, only hand cut.
-
It would be best to let the Gcode side drive that part and use Sheet Cam to post the code. At that point it is an automatic function.
(;-) TP
-
I use a macro in Mach3 to handle the torch referencing. I use one of 3 methods for sensing. Ohmic, floating head or capacitance. The machine is set up with all 3 and I never really know which one I'll use, so in Sheetcam I just insert the M code for the macro. Each method uses a different offset. The macro looks at a few different parameters to determine which method is in use and runs the referencing routine. After the macro runs, M03 is called to fire the torch.
If pierceHeight <= 0 Then
MsgBox("Please enter a valid pierce height")
code "M30"
Else
code "F30"
code "G31 Z-1"
While ismoving
Wend
code "G92 Z" & offset
While ismoving
Wend
code "G00 Z" & pierceHeight
While ismoving
Wend
End If
-
rrc1962,
Will try your code, I kind of forgot how to edit the M03 code, please guide me,
Thanks,
-
Ok I think I know,
C:\Mach3\macros\Mach3Mill
-
rrc1962,
I entered the code in M03, when I test run .nc file, when M03 is called I was asked to enter a valid pierce geight, and where do I put this pierce height value?
-
I'm using the Mach blue screen set, and on the right side of the screen there's a Z plate offset, I'm thinking of modifing the code of that Z plate offset.
When Z plate offset is pressed, the Z axis lower down and stop when switch is tripped, and from here I want to add some code so that it raise to 13.7mm then fire torch, woul'd anyone be kind enough to provide this code for me?
thx
-
I have a DRO on screen for the pierce height which is somthing that is usually handled by Sheetcam. You'll have to tweak the code to fit your application. You can add a DRO for pierce height or you can just hard code it in the Macro.
-
hello...i built my own cnc plasma table and i bouch mach 4 since its all new n ********* so i was like hey ********* it im down....in with the new out with the old right? the down side though is the majority of all the plasma post processors on sheetcam dont really help out much or dont read the instruction correctly. i built a floating head, "touch and go", auto touch off doohickey on my zaxis where my torch is mounted and its all bad ass n ********* right, but its freaking useless...the only one that works right is the "mach 3 plasma" post but whats the point. none of the post processors seem to work with mach 4 and ive tried to rescript the lua scripts in sheetcam and ive even corrected a few post errors which are not consistent with mach 4 but it still doesn't give me the functions i need.....everytime my torch moves it cuts on the traverses and ive read some mach 4 language is very different than the mach 3. i just want the damn auto touch off feature reference which utilizes the g28.1 z0 code to work so i can cut bigger ********* on my 4x8 table and im losing my mind here...anyone have some experience with this subject or can help?
-
I use mach 4 plasma with a torch touch . I use the vitalsystems arch pro screen that works with the hilcon controller. you can down load the arch pro screen and check it out . torch hight is all dun in the screen . and the settings for torch touch. the post processor I use in sheet cam is the mach 3 plasma . I also have one written buy sheet cam for an engraver using the marker not to fire the torch it all works good no problems
-
is there anyway the lua script in the post processor "mach 3 thc with scribe" in sheetcam can be edited in order for the touch off function to work ?.......will the vitalsystems arch pro screen work with my machine if i have a warp nine smooth stepper?
-
Hi,
the lua script in the post processor
Lua is the scripting language of Mach4. A post processor is software associated with your CAM program.
There is no such thing as a Mach4 post processor, but rather a post processor that works with your CAM
program to produce Gcode. The Gcode to be of use must be Mach compatible.
To my knowledge no CAM manufacturer uses Lua to write their post's therefore there is no Lua script in a post
processor.
i just want the damn auto touch off feature reference which utilizes the g28.1 z0 code to work so i can cut bigge
To my knowledge G28.1 has no role in Auto Touch Off......are you confusing G31?.....G31 is used for probing
which is very much related to Auto Touch Off.
Craig
-
here something what a simple search in the Forum showed:
You can set it up one of two ways using the G28.1 method OR use the G31 method.
With the G28.1 method you set up your floating head as the Z home and have it home toward the bed. Then the Cam that you use must generate the following type code.
N0120 G28.1 Z0.50
N0130 G92 Z0.0
N0140 G00 Z0.1370
N0150 G92 Z0.0
N0160 G00 Z0.2000
With the G31 method you setup the floating head as a Probe then you cam must generate code like
N0120 G31 Z -100 F19.685
N0130 G92 Z-0.0800
N0140 G00 X5.5505 Y9.8813
N0150 Z0.0000
Hope that helps, (;-) TP
-
thank you for clearing that up big joe!
in sheetcam there are some post processors which you can set the type of reference you want....either g31 or g28.1. i had my eyes set on using the g28.1 type but none of the post work for me since these are all for mach 3. is there no other way i can use these feature so i can put my floating head to work in order for it to reference its self before every cut? is the only option that vytalsystems arch pro screen? or is there any way someone can maybe tweak the post processors which have been written for mach 3 in order to be compatible with mach 4? and if so what would be the best approach in order to do so?
and another question for jcoldon......is the feature im seeking in that vytalsystems screen?......can i buy and use that screen and that reference feature even though i dont have a proma torch height control at the moment? ( i will be buying one soon tho)
thanks guuys
-
i assume that you fire up the torch via M3 command.
so you can modify M3 macro code to do the Floating head procedure.
i am not familar with LUA coding of Mach4, so somebody else must
guide you, if you want to go this road.
-
correct tps dude, i saw that as well.....but thats all for mach 3 and its talking about the post processors which are functions that generate the gcode depending on how you set it up when you click "edit post" in sheetcam. but since im using mach 4 its not really working out so well.......
-
ya i do use and m3 to fire but im not too familiar with modifying a macro code......can you elaborate ?
-
as i have written in Reply#18
am not familar with LUA coding of Mach4, so somebody else must
guide you, if you want to go this road.
-
Hi,
sounds like we're starting to make some progress.
I've used Mach3 but never that G28.1 trick, really really kool. I've used G31 extensively in Mach3 and for the last 18 months in Mach4.
Look for:
Mill GCode Programming
in Mach4 Docs. Note there is NO G28.1 mentioned. I don't know whether that's an oversight or what.
What I have found that all the gcode jobs that I used to run in Mach3 all pretty much works in Mach4. When all said and done Mach of whatever
flavor is a Gcode interpreter....conforming Gcode should work in either. Its my experience that Mach4 conforming Gcode is somewhat stricter in
interpretation than Mach3 compliant Gcode, there are a lot of tricks and shortcuts we used in Mach3 which really aren't good practice and often wont work
in Mach4.
I do recommend the use of G31.nnnn, you can generate probe files and all sorts of things and all extremely accurately.
For a plasma table you really really REALLY NEED THC. THC is a realtime feature and is enacted by the controller. Vital Systems HiCon board is the only Mach4
board I know of which has implemented it at this time. Nice screen addition in the GUI to support it too. The HiCon is not cheap but it is good....suck it up!
You may be required to do a little Lua coding to tie it all together but probably only 20 lines or so. Knowing what those lines are and where to put them is another
matter but you will find help on the forum.
Craig
-
but no matter witch road you are trying to go (G28/G31/M03),
your Hardware has to work first.
means Limit Switch has to be set as refZ or probe, and has to work.
if M3 script sould handle this, it also has to use one of this two methodes.
if you have for the example the G31 working, i think it should be no Problem to Setup
your sheetcam to generate the right code, it is only GCode, witch is not Mach3/Mach4
specific.
-
Hi,
Thomas is right, you could have the post just issue a M3 and the M3 would contain touch off code. You don't have to have the post include all that code explicitly.
Anyway once you get your HiCon and realize what features and code they've built in you wont be worried about some fancy post....
Craig
-
thank you guys so much for all the info...im sure this wont be my last question
heres a link to my youtube channel just in case you guys wana check out my build.....any feedback or tips and pointers would be appreciated
https://www.youtube.com/user/gus3291/videos?view_as=subscriber
-
Hello all I have Built a CNC plasma/router. The plasma is my first priority and I am pulling my hair out trying to get the touch off to work. I am cutting a few letters out that is encompassed by an oval to make a plaque. The program starts out with a probe as it should. it raises up for pierce and delays, it cuts out the first letter. Then it raises the safe Z (.5") rapids to the next letter and probes. rather than zeroing again it raises up around an inch and then starts to cut the letter 1" above the steel. it shows that it is at cut height on the dro but it is not. The next letter it will stair step up even higher and each letter does the some until the z axis runs up to its limit. I have included the first part of the code below to let you see what fusion produced. each contour in the program has this same start to the profile. I am new to Mach so hopefully this is easy. Thanks in advance
- Running mach3
nvem ethernet controller.
drawing and producing code in fusion 360
I have modified one of the latest posts off of the Fusion forum For a G31 touch off
(Plaque)
N10 G20
N15 G90
(2D Profile2)
N20 M6 T1
N25 G54
N30 M9
N40 G0 X0.3374 Y1.0667
N50 G31 Z-100
N55 G92 Z 0.05 reseting axis
N60 G0 Z 0.2
N65 M3
N70 G4 P 2
N75 G0 Z 0.15
N80 G1 X0.3863 Y1.0771 F39.37
N85 G2 X0.387 Y1.0789 I0.0295 J-0.0096
N90 G1 X0.3889 Y1.0838
N95 Y1.0839
-
Hi,
the code you have posted looks like it doesn't quite cover the first letter....can you post more so that we can see how the code calls for the transition from one letter
to the next.
Craig
-
Thank you for the reply. The code is quite long but, here are a few letters. I took at some of the Mumbo Jumbo in the Midddle
Weldsmith
(Plaque)
N10 G20
N15 G90
(2D Profile2)
N20 M6 T1
N25 G54
N30 M9
N40 G0 X0.3374 Y1.0667
N50 G31 Z-100
N55 G92 Z 0
N60 G0 Z 0.1
N65 M3
N70 G4 P 1.5
N75 G0 Z 0.065
N80 G1 X0.3863 Y1.0771 F39.37
N85 G2 X0.387 Y1.0789 I0.0295 J-0.0096
N90 G1 X0.3889 Y1.0838
N1900 X0.3833 Y1.0676
N1905 Y1.0678
N1910 X0.3848 Y1.0724
N1915 Y1.0725
N1920 X0.3863 Y1.0771
N1925 X0.3529 Y1.1143
N1930 M5
N1935 G0 Z 0.5
(2D Profile3)
N1945 M6 T1
N1950 M9
N1960 G0 X0.8993 Y0.9748
N1970 G31 Z-100
N1975 G92 Z 0
N1980 G0 Z 0.1
N1985 M3
N1990 G4 P 1.5
N1995 G0 Z 0.065
N2000 G1 X0.9778 Y0.9904 F39.37
N2005 X1.0878 Y1.3138
N2010 X1.0105
N3570 X0.9721 Y0.9749
N3575 X0.974 Y0.9801
N3580 X0.9759 Y0.9854
N3585 X0.9778 Y0.9904
N3590 X0.925 Y1.0505
N3595 M5
N3600 G0 Z 0.5
(2D Profile4)
N3610 M6 T1
N3615 M9
N3625 G0 X1.3546 Y1.2446
N3635 G31 Z-100
N3640 G92 Z 0
N3645 G0 Z 0.1
N3650 M3
N3655 G4 P 1.5
N3660 G0 Z 0.065
N3665 G1 X1.3146 Y1.3138 F39.37
N3670 X1.2168
N3675 X1.19 Y1.2351
N3680 X1.231
N3685 G2 X1.2603 Y1.1941 I0. J-0.031
N3690 G1 X1.1317 Y0.816
N3695 X1.2081
N3700 X1.3435 Y1.2141
N3705 G2 X1.3729 Y1.2351 I0.0293 J-0.01
N3710 G1 X1.4357
N3715 X1.4625 Y1.3138
N3720 X1.3146
N3725 X1.2746 Y1.2446
N3730 M5
N3735 G0 Z 0.5
(2D Profile5)
N3745 M6 T1
N3750 M9
N3760 G0 X1.4445 Y1.0039
N3770 G31 Z-100
N3775 G92 Z 0
N3780 G0 Z 0.1
N3785 M3
N3790 G4 P 1.5
N3795 G0 Z 0.065
N3800 G1 X1.4745 Y0.9519 F39.37
N3805 X1.5461
N3810 X1.5653 Y1.0082
N3815 X1.4261
N3820 X1.407 Y0.9519
N3825 X1.4745
N3830 X1.5045 Y1.0039
N3835 M5
N3840 G0 Z 0.5
-
Hi,
I would guess that its the M6 T1 and/or the M9 lines between letters.
Do you actually need a toolchange? I suspect not. May I suggest commenting out the M6 T1 lines,
or edit them out, even just the first few occurances, and see what happens.
Craig
-
I have done exactly that. and no luck. I thought it might be a check box in settings in Mach?
-
Hi,
the only other possible culprit then is:
G92 Z0
You may have noted that the short Gcode reference in Mach3 does not recommend this legacy G code. I don't recall having used it or had
any Gcode generated by a CAM/post that used it either.
I'm wondering if it updates the work co-ordinates ie your current G54 or whether it changes your machine co-ordinates?
I think some experimentation on the effects of this code are in order.
Craig
-
Mine is doing the exact same thing except with g28.1, it’s gotta be something simple!
Hello all I have Built a CNC plasma/router. The plasma is my first priority and I am pulling my hair out trying to get the touch off to work. I am cutting a few letters out that is encompassed by an oval to make a plaque. The program starts out with a probe as it should. it raises up for pierce and delays, it cuts out the first letter. Then it raises the safe Z (.5") rapids to the next letter and probes. rather than zeroing again it raises up around an inch and then starts to cut the letter 1" above the steel. it shows that it is at cut height on the dro but it is not. The next letter it will stair step up even higher and each letter does the some until the z axis runs up to its limit. I have included the first part of the code below to let you see what fusion produced. each contour in the program has this same start to the profile. I am new to Mach so hopefully this is easy. Thanks in advance
- Running mach3
nvem ethernet controller.
drawing and producing code in fusion 360
I have modified one of the latest posts off of the Fusion forum For a G31 touch off
(Plaque)
N10 G20
N15 G90
(2D Profile2)
N20 M6 T1
N25 G54
N30 M9
N40 G0 X0.3374 Y1.0667
N50 G31 Z-100
N55 G92 Z 0.05 reseting axis
N60 G0 Z 0.2
N65 M3
N70 G4 P 2
N75 G0 Z 0.15
N80 G1 X0.3863 Y1.0771 F39.37
N85 G2 X0.387 Y1.0789 I0.0295 J-0.0096
N90 G1 X0.3889 Y1.0838
N95 Y1.0839
-
Here are the first couple of sections of the code.
Running sheetcam
Mach3
PROMA THC (works)
Floating head
N0020 (Post processor: MP1000-THC.scpost)
N0030 (Date: 29/05/2018)
N0040 G20 (Units: Inches)
N0050 G53 G90 G40
N0060 F1
N0070 (Part: sumospeed logo 12 in at 100 feed rate wo lines)
N0080 (Operation: Inside Offset, CAD, T1: Plasma, 0.0591 in kerf)
N0090 M06 T1 F60 (Plasma, 0.0591 in kerf)
N0100 G00 Z1.0000
N0110 X5.5555 Y1.3313
N0120 Z0.0000
N0130 G28.1 Z0.12
N0140 G92 Z0.0
N0150 G00 Z0.0520
N0160 G92 Z0.0
N0170 G00 Z0.0000
N0180 M03
N0190 G03 X5.4906 Y1.2266 I0.1570 J-0.1699 F60.0
N0200 X5.4740 Y1.0999 I0.2268 J-0.0942
N0210 X5.4761 Y1.0921 I0.0293 J0.0039
N0220 X5.5732 Y0.9847 I0.2069 J0.0894
N0230 G01 X5.7340 Y0.8544
N0240 G02 X5.8234 Y0.7373 I-0.2290 J-0.2674
N0250 X5.8333 Y0.6398 I-0.2239 J-0.0719
N0260 X5.7847 Y0.4332 I-0.8676 J0.0947
N0270 G01 X5.7837 Y0.4299
N0280 G02 X5.6196 Y0.1543 I-0.5282 J0.1278
N0290 X5.1657 Y0.0295 I-0.4043 J0.5824
N0300 G01 X5.1608 Y0.0294
N0310 G02 X4.8678 Y0.1252 I-0.0364 J0.3849
N0320 X4.8310 Y0.2328 I0.1042 J0.0957
N0330 X4.8813 Y0.4558 I0.8337 J-0.0708
N0340 G01 X4.8816 Y0.4568
N0350 X4.9077 Y0.5344
N0360 X5.2554
N0370 X5.2090 Y0.3969
N0380 G03 X5.1897 Y0.2827 I0.2109 J-0.0943
N0390 X5.1947 Y0.2686 I0.0294 J0.0025
N0400 G01 X5.2145 Y0.2397
N0410 G03 X5.2392 Y0.2268 I0.0244 J0.0167
N0420 X5.4178 Y0.3745 I-0.0020 J0.1843
N0430 X5.4443 Y0.5703 I-0.3059 J0.1410
N0440 X5.4385 Y0.5837 I-0.0292 J-0.0048
N0450 X5.2797 Y0.7245 I-0.4588 J-0.3573
N0460 G01 X5.1501 Y0.8264
N0470 G02 X5.1035 Y0.8842 I0.1018 J0.1296
N0480 X5.1159 Y1.1474 I0.3261 J0.1166
N0490 G01 X5.1178 Y1.1528
N0500 G02 X5.2956 Y1.4462 I0.5615 J-0.1397
N0510 X5.6633 Y1.5597 I0.3481 J-0.4752
N0520 G01 X5.6650
N0530 G02 X5.8817 Y1.5372 I0.0202 J-0.8598
N0540 X5.9946 Y1.4763 I-0.0561 J-0.2392
N0550 X6.0316 Y1.3747 I-0.0833 J-0.0879
N0560 X5.9771 Y1.1495 I-0.9292 J0.1060
N0570 G01 X5.9767 Y1.1484
N0580 X5.9626 Y1.1062
N0590 X5.6149
N0600 X5.6431 Y1.1895
N0610 G03 X5.6670 Y1.3034 I-0.2869 J0.1198
N0620 G01 X5.6661 Y1.3111
N0630 G03 X5.5841 Y1.3618 I-0.0669 J-0.0166
N0640 X5.5611 Y1.3353 I0.0065 J-0.0288
N0650 G01 X5.5555 Y1.3313
N0660 M05
N0670 G00 Z1.0000
N0680 X6.6562 Y1.3628
N0690 Z0.0000
N0700 G28.1 Z0.12
N0710 G92 Z0.0
N0720 G00 Z0.0520
N0730 G92 Z0.0
N0740 G00 Z0.0000
N0750 M03
N0760 G01
N0770 X6.6489 Y1.3624
Mine is doing the exact same thing except with g28.1, it’s gotta be something simple!
Hello all I have Built a CNC plasma/router. The plasma is my first priority and I am pulling my hair out trying to get the touch off to work. I am cutting a few letters out that is encompassed by an oval to make a plaque. The program starts out with a probe as it should. it raises up for pierce and delays, it cuts out the first letter. Then it raises the safe Z (.5") rapids to the next letter and probes. rather than zeroing again it raises up around an inch and then starts to cut the letter 1" above the steel. it shows that it is at cut height on the dro but it is not. The next letter it will stair step up even higher and each letter does the some until the z axis runs up to its limit. I have included the first part of the code below to let you see what fusion produced. each contour in the program has this same start to the profile. I am new to Mach so hopefully this is easy. Thanks in advance
- Running mach3
nvem ethernet controller.
drawing and producing code in fusion 360
I have modified one of the latest posts off of the Fusion forum For a G31 touch off
(Plaque)
N10 G20
N15 G90
(2D Profile2)
N20 M6 T1
N25 G54
N30 M9
N40 G0 X0.3374 Y1.0667
N50 G31 Z-100
N55 G92 Z 0.05 reseting axis
N60 G0 Z 0.2
N65 M3
N70 G4 P 2
N75 G0 Z 0.15
N80 G1 X0.3863 Y1.0771 F39.37
N85 G2 X0.387 Y1.0789 I0.0295 J-0.0096
N90 G1 X0.3889 Y1.0838
N95 Y1.0839
-
Got it, changed the G28.1 to G31. Thanks for all the info. It works now!