Pokey57cnc + Mach3 + Sheetcam

Mach3 and Mach4 questions, tips and topics can be posted here
Post Reply
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

I just got done converting my windows XP with parrallel port and BOB system to a windows 10 system with a Pokeys57cnc controller. Everything is almost working as it should, but I have a weird issue with my Z losing reference.

My issue: I have a floating head and a switch. I am using a post processor profile for constant touchoff which goes down and finds the material before each feature is cut using G31. I mapped the switch to pin 19 on the pokeys board which is labeled "probe". It seems to work okay except that the plamsa is up too high. I have it set to cut at 0.060" above the material. However it is cutting at about double that above the material. I used this same profile with the old hardware setup and it worked flawlessly.

Also a weird thing is happening where when the cutting is finished my torch moves to about an inch above the material height, but Mach3 reports it being about 1.5" above material. If I click the go to zero command it tries to go down 1.5" and it crashes into the material. It almost seems like every time it probes for material height it adds that distance onto the position, so by the end of the cut it is 1" + all the probed heights. I am probably way off, but I don't know what to look at to fix it. I've gone through EVERY menu to make sure it matches my old setup. To me it should just work like it did before.
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

nick7251 wrote: Mon Jun 15, 2020 4:19 pm My issue: I have a floating head and a switch. I am using a post processor profile for constant touchoff which goes down and finds the material before each feature is cut using G31. I mapped the switch to pin 19 on the pokeys board which is labeled "probe". It seems to work okay except that the plamsa is up too high. I have it set to cut at 0.060" above the material. However it is cutting at about double that above the material. I used this same profile with the old hardware setup and it worked flawlessly.
Do you have a switch offset set within sheetcam post processor?

Check the gcode (or post a snippet here)....
It should say something like

Code: Select all

G31 Z-xxxx Fxxxx 
G92 Z-yyyy (where Y is the offet of the switch)
Some gcode does it the long way...

Code: Select all

G31 Z-xxxx Fxxxx
G92 Z0
G0 Z0.125  (where 0.125 is the switch offset)
G92 Z0
both achieve the same result .... just one is a little longer to do
nick7251 wrote: Mon Jun 15, 2020 4:19 pm Also a weird thing is happening where when the cutting is finished my torch moves to about an inch above the material height, but Mach3 reports it being about 1.5" above material. If I click the go to zero command it tries to go down 1.5" and it crashes into the material. It almost seems like every time it probes for material height it adds that distance onto the position, so by the end of the cut it is 1" + all the probed heights. I am probably way off, but I don't know what to look at to fix it. I've gone through EVERY menu to make sure it matches my old setup. To me it should just work like it did before.
The post processor is probably telling the torch to rise to a safe clearance position

In sheetcam go to Job Options, and look at "rapid clearance" or have a look at the "parking Options tab"

In Mach3, the machine is probably set to send the Z axis home..... the problem is you machine does not know where home is I suspect (do you home the z-axis?)

In Mach3, go to Config menu and at the bottom is "Safe_Z Setup" and the options should be self explanatory as to whether you want them set or not


It is probably worth while clarifying what YOU think the Z-axis direction is and what the machine thinks it is.....
For Plasma Z UP or away from the table is (+) direction
Z DOWN or towards (or below) the table is (-) direction

so G31 Z-4 F100 is a probe downwards towards the table at a feedrate of 100

a G0 Z-10 will sent the machine in a downwards direction after a G92 Z0 has been performed

but G53 G0 Z10 will tell the machine to move in Machine Co-ordinates to the position Z10.... that could be 10" above the home switch if home has been set at the top of the machine..... or 10" above the work if you use G28 instead of G31......

if in doubt.... post your gcode and someone will review it..... post your profile or provide some screenshots of your setup and again someone will comment..... you can never have too much information when trying to figure something out sadly.... we get asked why something is not working in 60 words or less and have to guess.....
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

Do you have a switch offset set within sheetcam post processor?
Check the gcode (or post a snippet here)....
It should say something like

Code: Select all

G31 Z-xxxx Fxxxx 
G92 Z-yyyy (where Y is the offet of the switch)
Some gcode does it the long way...

Code: Select all

G31 Z-xxxx Fxxxx
G92 Z0
G0 Z0.125  (where 0.125 is the switch offset)
G92 Z0
both achieve the same result .... just one is a little longer to do
Yes, I have a switch offset of .160". Here is my code

Code: Select all

switchoffset = -0.16
function OnPenDown()
   if(dist >= (refdistance/scale)) then
      dist = 0
      post.ModalText(" G31 Z -100")
      post.ModalNumber (" F", 500 * scale, "0.0###")
      post.Eol()
      post.ModalText(" G92")
      post.NonModalNumber(" Z", switchoffset, "0.00")
      post.Eol()
      post.CancelModalNumbers()
   end
--[[   post.ModalText (" G00")
   post.ModalNumber (" X", endX * scale, "0.0000")
   post.ModalNumber (" Y", endY * scale, "0.0000")
   post.Eol()]]
   if (preheat > 0) then
      post.ModalText (" G00")
      post.ModalNumber (" Z", cutHeight * scale, "0.0000")
      post.Eol()
      post.Text(" M801\n G04 P 0.5\n M802\n G04 P0.1\n M902")
      post.Text ("\n G04 P")
      post.Number (preheat,"0.###")
      post.Eol()
   end
   post.ModalText (" G00")
   post.ModalNumber (" Z", pierceHeight * scale, "0.0000")
   post.Text ("\n M03\n")
   if (pierceDelay > 0) then
      post.Text (" G04 P")
      post.Number (pierceDelay,"0.###")
      post.Eol()
   end
end


function OnPenUp()
   post.Text (" M05\n")
   if (endDelay > 0) then
      post.Text (" G04 P")
      post.Number (endDelay,"0.###")
      post.Eol()
   end
end


function OnNewOperation()
   post.Text (" (Process: ", operationName, ")\n")
   if (plungeRate <= 0) then
      post.Warning("WARNING: Plunge rate is zero")
   end
   if (feedRate <= 0) then
      post.Warning("WARNING: Feed rate is zero")
   end
end
I did not write this code, and don't fully understand it either. It was provided to me by Write CNC with the Write table I am using.
The post processor is probably telling the torch to rise to a safe clearance position

In sheetcam go to Job Options, and look at "rapid clearance" or have a look at the "parking Options tab"

In Mach3, the machine is probably set to send the Z axis home..... the problem is you machine does not know where home is I suspect (do you home the z-axis?)

In Mach3, go to Config menu and at the bottom is "Safe_Z Setup" and the options should be self explanatory as to whether you want them set or not
Rapid Clearance is set at 0.5". parking position is not selected and all values say 0.

I usually home the z axis initially to the top of the material. May be redundant but I do it anyways.
Material.JPG
Material.JPG (35.18 KiB) Viewed 1164 times
Parking.JPG
Parking.JPG (22.62 KiB) Viewed 1164 times
When I go to "Save_Z setup"... Allow safe_Z Moves is not selected. The radio button is set to SafeZ DRO is in work coordinates, and safe_Z is set to 0.5.
mach Safe Z.JPG
mach Safe Z.JPG (20.94 KiB) Viewed 1164 times
It is probably worth while clarifying what YOU think the Z-axis direction is and what the machine thinks it is.....
For Plasma Z UP or away from the table is (+) direction
Z DOWN or towards (or below) the table is (-) direction
Yes, Page up (+) moves my torch away from the material and page down (-) moves it closer.
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

Ahh.... All units in the sheetcam post processor must be in millimetres.... Not inches....

Basically sheetcam applies a scale factor to all movements if you tell it you want the machine to move in inches

0.16 inches is 4.064 mm
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Pokey57cnc + Mach3 + Sheetcam

Post by acourtjester »

let me ask a question is the Pokeys57cnc a USB motion controller, and is it setup to do Plasma. Another in the Mach for home and limits menu do you have the Z set for home negative, the G31 command is a home command, if you have home positive it will go up not down. I just gave up with a USB motion controller as I have a G31 problem for that I found a work around. I put a delay in the post processor just before the G31 line this worked. But since the USB was not setup for plasma I could not get the THC signals through Mach to the computer. It could see the ARC ok but no up or down signals, they showed on the diagnostic page but that was it.
g31 delay.JPG
g31 delay.JPG (79.43 KiB) Viewed 1163 times
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

In sheetcam machine config is the machine set as top of material (just check please)
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

Pokeys is supposed to be setup for plasma (thc etc).... But I've recently struggled to set it up for a lathe and mach4 and gave up.. (it was my Bob and it's pin availability not really pokeys issue... But found it hard work...).. Now using uccnc which does not officially do turning....
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

robertspark wrote: Mon Jun 15, 2020 6:03 pm Ahh.... All units in the sheetcam post processor must be in millimetres.... Not inches....

Basically sheetcam applies a scale factor to all movements if you tell it you want the machine to move in inches

0.16 inches is 4.064 mm
Curious how you could tell the post was in mm instead of inches? Trying to learn this stuff so bear with the dumb questions. My sheetcam is set up in inches, to me the post looks like the values are inches, and Mach is also set in inches.
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

acourtjester wrote: Mon Jun 15, 2020 6:04 pm let me ask a question is the Pokeys57cnc a USB motion controller, and is it setup to do Plasma. Another in the Mach for home and limits menu do you have the Z set for home negative, the G31 command is a home command, if you have home positive it will go up not down. I just gave up with a USB motion controller as I have a G31 problem for that I found a work around. I put a delay in the post processor just before the G31 line this worked. But since the USB was not setup for plasma I could not get the THC signals through Mach to the computer. It could see the ARC ok but no up or down signals, they showed on the diagnostic page but that was it.
g31 delay.JPG
Please help me understand the p0.2/n on your delay?

Pokeys57cnc can be set up as USB or Ethernet. Right now I am running USB but some of my research is leading me to believe that could pose some timing problems compared to running it on Ethernet. So I plan to switch over to Ethernet.

In Mach I have it set for Home Positive. So are you saying I need to set that parameter?
Home limits.JPG
Home limits.JPG (45.77 KiB) Viewed 1158 times
As far as the torch height controller. I may be having issues there too. I am nervous about how I finally got it to work. I mapped the Pokeys board to simulate a Page up and page down keyboard command to mach. I think this could be problematic, and although I haven't done much testing to verify, it feels like a cheat that won't work in the end. It was the only way I could figure out to get the controller to move the torch head while my Proma THC was in test mode.
User avatar
djreiswig
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1929
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Pokey57cnc + Mach3 + Sheetcam

Post by djreiswig »

nick7251 wrote: Mon Jun 15, 2020 10:57 pm
robertspark wrote: Mon Jun 15, 2020 6:03 pm Ahh.... All units in the sheetcam post processor must be in millimetres.... Not inches....

Basically sheetcam applies a scale factor to all movements if you tell it you want the machine to move in inches

0.16 inches is 4.064 mm
Curious how you could tell the post was in mm instead of inches? Trying to learn this stuff so bear with the dumb questions. My sheetcam is set up in inches, to me the post looks like the values are inches, and Mach is also set in inches.
All the SheetCam posts are coded in mm. If you set SheetCam up to use inches, the measurements are scaled in the post. 1" = 25.4mm. So if you put a switch offset value in the post it should be in mm.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

djreiswig wrote: Mon Jun 15, 2020 11:14 pm

All the SheetCam posts are coded in mm. If you set SheetCam up to use inches, the measurements are scaled in the post. 1" = 25.4mm. So if you put a switch offset value in the post it should be in mm.
That would mean based on my code that the switch offset being set at .160 would only be .006"? That doesn't make a lot of sense to me because I know it is more than .006" and this code worked fine before. Just more pieces to the puzzle. This is kind of fun to figure out and work on, but at the same time I want to get this thing cutting again. Luckily it is a hobby table, and I don't have a business relying on it.
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

So it seems I can run a job okay. But when it finishes the torch moves up to the .625" safe clearance even though I set it at .5". but the real issue is the DRO is saying it is at +1.2707 height. So when you say go to zero it pushes it past the material by quite a bit. I don't understand why Z is growing in the DRO.
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Pokey57cnc + Mach3 + Sheetcam

Post by acourtjester »

As to your question about the P0.2 delay I put in the Post processor, it was a guess on my part. The reason was I could single step the G-code and it worked normally, but normal operational speed it would not work correctly. By this I mean when the G31 command was executed (normal speed) it would slightly move down then move to the next step and function correctly. I figured this was a timing issue and that is why I put the delay in.
With the USB BOBs I have used they require a .DLL file to be installed in the plugin folder in Mach 3 for them to work. I think this is for the interpolation of the signals between the USB BOB and Mach 3 to perform the operations. These are assumptions on my part to add to that the BOB will work fine as a router but is not setup for Plasma use and therefore no THC function.
Does the Pokeys57cnc require a .DLL file to be used for its operation?
you may want to look at this
https://www.cnczone.com/forums/plasma-e ... 3-4-a.html
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

acourtjester wrote: Tue Jun 16, 2020 9:45 am As to your question about the P0.2 delay I put in the Post processor, it was a guess on my part. The reason was I could single step the G-code and it worked normally, but normal operational speed it would not work correctly. By this I mean when the G31 command was executed (normal speed) it would slightly move down then move to the next step and function correctly. I figured this was a timing issue and that is why I put the delay in.
With the USB BOBs I have used they require a .DLL file to be installed in the plugin folder in Mach 3 for them to work. I think this is for the interpolation of the signals between the USB BOB and Mach 3 to perform the operations. These are assumptions on my part to add to that the BOB will work fine as a router but is not setup for Plasma use and therefore no THC function.
Does the Pokeys57cnc require a .DLL file to be used for its operation?
you may want to look at this
https://www.cnczone.com/forums/plasma-e ... 3-4-a.html
Yes, it has a plug-in .dll file. But it is also set up for plasma. Polabs (the maker of pokeys57CNC) makes their own THC even, or has it made for them. It looks like the proma but it is fiber optic isolated. It looks pretty nice. But the Proma came with my machine so I plan to use it.

I've read that thread you posted before. It was written in 2018 with no replies that I could see. Maybe because I'm not a member on cnczone?
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

I switched over to Ethernet control last night. It has the same problem but with reporting in the DRO a much higher z location than the actual torch distance from the material.

It also did something interesting. Every other feature would not probe the surface of the material, and would start it's movements from the rapid clearance z height. And the opposite every other feature it would probe the material. I think I'm going to generate another test file to ensure its not the file that is screwed up. Even though this file worked fine in the old setup. I'll also generate a file with a delay in the post.
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Pokey57cnc + Mach3 + Sheetcam

Post by acourtjester »

the was a reply to your post on CNCzone see attached screenshot, not a real answer. Have you tried to single step your G-code to see what happens. You can just edit the G-code by adding this line before the G31 line G4 P0.2 then save it.
Pokey CNC zone.JPG
Last edited by acourtjester on Tue Jun 16, 2020 3:07 pm, edited 1 time in total.
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

No I haven't tried stepping through the g-code, that is a good idea. I will admit that I am fairly new to all this, and don't know how to single step the g-code in Mach3. I'm sure a quick google search will tell me.

I really didn't want to start talking about the THC in this post as it isn't enabled yet. I want to fix one problem at a time. The problem at hand is the DRO reading much higher than the torch actually is. So going back to zero plunges the torch into the material. I guess it could be a Pokeys57cnc issue, but I think it is probably something from porting all the stuff over from my old system to the new that is messed up.
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Pokey57cnc + Mach3 + Sheetcam

Post by acourtjester »

On the program page you click on the single step button and then the cycle start button will move one line for each button push
You are learning and doing fine, things move slowly sometimes
single.JPG
single.JPG (58.63 KiB) Viewed 1142 times
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

acourtjester wrote: Tue Jun 16, 2020 3:12 pm On the program page you click on the single step button and then the cycle start button will move one line for each button push
You are learning and doing fine, things move slowly sometimes
single.JPG
Thank you. You really are an Elite Member. I'll give that a try and see if I notice anything weird.
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

Okay, so I stepped through the G-code one line at a time. It seemed to behave properly until the last line of code. The last line is

Code: Select all

N1300 M05 M30
So I looked in the post and it is as follows:

Code: Select all

function OnFinish()
   post.Text (" M05 M30\n")
end
Can anybody clue me in on what the \n means after the M30? It was on the final line that the DRO jumped up to a weird number without moving the torch up to match that number.
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

"/n"

means NEW LINE..... i.e. create a new line (same as EOL() which you may see [end of line]]

M30 is programme end and rewind

i.e. stop the gcode but rewind it to line 1

https://machmotion.com/blog/knowledge-support-mcode
robertspark
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1807
Joined: Mon Jun 12, 2017 6:43 pm

Re: Pokey57cnc + Mach3 + Sheetcam

Post by robertspark »

there is a table here which may be of use to you

https://www.lua.org/pil/2.4.html
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Pokey57cnc + Mach3 + Sheetcam

Post by acourtjester »

That is a normal end to a g-code, if you have a problem at the very end there may be some underlying code snippet or cut rule you are not aware of.
Let's back up a small bit, are you saying the g-code operated as you wanted it to when single stepping? just the end screwed up.
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
nick7251
2.5 Star Member
2.5 Star Member
Posts: 108
Joined: Tue Dec 17, 2019 6:28 pm
Location: Utah (Nothern)

Re: Pokey57cnc + Mach3 + Sheetcam

Post by nick7251 »

acourtjester wrote: Tue Jun 16, 2020 8:07 pm That is a normal end to a g-code, if you have a problem at the very end there may be some underlying code snippet or cut rule you are not aware of.
Let's back up a small bit, are you saying the g-code operated as you wanted it to when single stepping? just the end screwed up.
Yes. The step just before this the torch went to the rapid movement height of 0.5" like it should. Then after or during the last line or at some point around there the DRO jumped up in value. Weird.
User avatar
djreiswig
4.5 Star Elite Contributing Member
4.5 Star Elite Contributing Member
Posts: 1929
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Pokey57cnc + Mach3 + Sheetcam

Post by djreiswig »

Can you either copy/paste or post the gcode? It might help us to figure out what is happening if we see the whole code.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)
Post Reply

Return to “Mach3 & Mach4 CNC”