[CastleWorks]

Hi,

I currently have a CNC router that I built (48"x48" table), I have been using it for years with no problems. For my CAM software I use Vectric, and Mach 3 as my controller software.

I would like to convert this table to use a plasma cutter on it.

Questions:

1. What are some of the more popular CAM programs used in plasma cutting? Do most people also use Mach 3 as a controller in the same manner as I do (CAM program generates G code....then load G code in Mach 3)...or is the plasma software a totally different process?

2. On my plasma cutter, (Miller 625 Spectrum) I have three signals "remote start", "OK to Move" and "voltage Sense" I understand what these are used for, however I am not sure where to connect them into my machine / I/O board

I appreciate any input.

Thanks!

[Greolt]

Sheetcam would be the most popular generic CAM software for plasma cutting.

However don't think that you can't use Vectric. I use Aspire for my plasma, because I have it and am very familiar with it. Vcarve and Cut2D will do the same as far as plasma is concerned.

If you use a THC such as CandCNC then there are very specific and complex post processors written for Sheetcam and that THC.

If like me, you use a simpler THC, then Vectric will do a very adequate job.

Just need to write a post processor to put out the appropriate gcode. That is not difficult and I can assist if you need help.



"I have three signals "remote start", "OK to Move" and "voltage Sense" I understand what these are used for, however I am not sure where to connect them into my machine / I/O board"

On a simple THC like mine, "Remote Start" and "OK to move" will be output and intput to Mach3 respectively. "Voltage sense" will go to the THC.

There are a lot of different THCs so these connections will depend on which you use.

[CastleWorks]

I would be interested to hear what THC you are using, sounds like it works fine

As for the input and output signals ( OK to move and remote start) I assumed they would go to the I/O, just was not sure on how Vectric would read and write to these.....I definitely welcome your input on the post processor details.

Thanks, I appreciate the input


QUOTE=Greolt;1841396]Sheetcam would be the most popular generic CAM software for plasma cutting.

However don't think that you can't use Vectric. I use Aspire for my plasma, because I have it and am very familiar with it. Vcarve and Cut2D will do the same as far as plasma is concerned.

If you use a THC such as CandCNC then there are very specific and complex post processors written for Sheetcam and that THC.

If like me, you use a simpler THC, then Vectric will do a very adequate job.

Just need to write a post processor to put out the appropriate gcode. That is not difficult and I can assist if you need help.



"I have three signals "remote start", "OK to Move" and "voltage Sense" I understand what these are used for, however I am not sure where to connect them into my machine / I/O board"

On a simple THC like mine, "Remote Start" and "OK to move" will be output and intput to Mach3 respectively. "Voltage sense" will go to the THC.

There are a lot of different THCs so these connections will depend on which you use.[/QUOTE]

[Greolt]

I would be interested to hear what THC you are using, sounds like it works fine

A popular simple THC is the Proma 150

Proma-Elektronika - Produkty

I am using the THC3T-01

Compact THC3T-01

I would not recommend it for a production environment. There are better (more expensive) options out there, but for what I do it works fine

.....I definitely welcome your input on the post processor details.

As far as the PP for Vectric, the following are the relevant parts of my PP.


+ ---------------------------------------------------
+ Commands output for Plunge Moves
+ ---------------------------------------------------

begin PLUNGE_MOVE

"M12"

"M3"

"G4 P200"

"G0 Z1.5"

+ ---------------------------------------------------
+ Commands output for Retract Moves
+ ---------------------------------------------------

begin RETRACT_MOVE

"M5"

"G0 Z20"


You can put as little or as much code that you need in the commands.

I have a "M12" this calls my touch off macro, which ends with the torch at pierce height. This could also be done with straight code rather than a macro.

Followed by a "M3" which turns on the torch

Then a "G4 P200" which is a 0.2 sec delay for pierce

And a "G0 Z1.5" which moves the torch to cut height.

Then for Retract, I have a "M5" to turn the torch off, followed by a "G0 Z20" retract.

[CastleWorks]

Thanks for the input on the THC and code. I don't have any experience with using macros in Mach 3, can you shoot me an example of your macro code.
I think I am still missing something though....would I simply just edit the G code from V Carve and insert this code prior to any move where I needed the torch to pick up and move? Where do the signals from my plasma machine that I would connect to my I/O card come into play?

Thanks

[Greolt]

I think I am still missing something though....would I simply just edit the G code from V Carve and insert this code prior to any move where I needed the torch to pick up and move?

The job of the Post Processor is to produce the code required to carry out the job. No need for any editing of the gcode.

I don't have any experience with using macros in Mach 3, can you shoot me an example of your macro code.

Here is my macro that is called each time a touch off is required. This suits my needs. Others will vary.

Pierce height = GetUserDRO(1159) 'get Pierce height from on-screen DRO
Code "G90 G31 Z-40 F1300" 'probing move
While IsMoving()
Wend
Call SetDro (2, -1.5) 'set the Z axis DRO to match floating head switch over run
Sleep 50 'Pause for DRO to update.
Code "G1 Z" & Pierce height 'move Z up to pierce height
While IsMoving()
Wend

Note this touch off routine can be done with gcode only. Dispensing with the need for a macro if preferred.

Where do the signals from my plasma machine that I would connect to my I/O card come into play?

There are many variations of THC. The simple ones like I use are like this.

1. Signal from controller to plasma cutter to start and stop arc.

2. Signal from plasma or THC to controller that arc is established and OK.

3. Up or Down signals from THC to controller.

[shad71]

Hello!
CastleWorks, look how work my Neuron Simplicity THC.
Torch slide and cutter under full Neuron control.No makros.
Just use Neuron post processor with THC control rules for sheetcam for making program in XY plane.
Load to Mach3.
Cut.
All what you need now and in the future provide the controller.
Please read user's manual.
http://neuroncnc.com/assets/docs/Neu...UserManual.pdf