How to do tool changes with CNC plasma

[Econdron]

I'd like to cut out a couple hundred mounting brackets and I'd like to etch my company name and/or logo on them. So I'd like to go through and do the marking in one step then change the consumables to cutting and finish cutting the brackets. How would I do this? I'd like to avoid not loading two separate TAP files into CommandCNC if possible, I'd like to it all be the same program so I don't have to worry about offset errors. I'm using SheetCAM. It's a Hypertherm 45XP if it makes a difference. It's not just this one part, I'd like to do this similar process every time I etch my logo on a part that I cut out, which may only be a one-off. Is this possible?

[djreiswig]

From my personal experiences I don't think I would mark that many parts before cutting them. What happens if your torch crashes and you mess a part up. It's easy to nudge your drawing over a little and start cutting again and not waste a bunch of material. That's just my experience. Now, if they are small parts, it may not be that big of a deal.
As far as how to do it with CommandCNC, can't help you there. I'm a mach3 guy, however you should be able to make 2 different layers in sheetcam and make a tool for each layer and use a different operation. Stop after the marking and switch your consumables.

[tcaudle]

Are you marking with the torch or with a plate marker? You just need to setup a different tool for the plate marker with the offsets and it will do it in any sequence you want. If you simply want to change the plasma arc current and nozzle (or other parameters you need to put them both in the same job but insert a code "snip " in Sheetcam between the two operations taht moves the torch to a location and pauses motion while you make the changes and make any manual changes and then loads the new tool for that operation and runs when you hit resume


1. Setup a G cnip in the tools and enter the g-code
2, Setup an operation between the two opeartions you want to do and use that snip as the operation

Code snip might look something like this: for the torch reconfigure:
G00 X12 Y12 Z2 (moves the tarch to x12 and Y12 and raises the Z to 2)"
M1 (pauses motion)

Do either one first or last. or break it up in other layers or operations but you need to put in the code snip before each change in cut type

[tcaudle]

You can also setup a default tool change action in SHeetCAM that sees a new tool and alwyas does thet action. Options/Job Options/Toolchange. It will stick the code in before each operation where there is a tool change.

[tnbndr]

If you are running a torch and scriber mine you just need to put the scribe operations on one layer and the cutting on another layer and then apply your sheetcam tools in the proper order.
For instance all my drawings have three layers, inside , outside and scribe. When I apply tooling in sheetcam scribe is always first, then inside cuts and finally outside cuts.

[Econdron]

Sorry, should have been more specific. I'm using the plasma cutter as the plate marker. The 45XP has the new ability to do plate marking at 10amps. But it requires different consumables as well. So it's not as simple as just doing two different operations with different settings, I need a pause in between the two operations so I can swap out the consumables.

I think that's what I was looking for, Tom. I didn't realize I could do just a code operation. I'll give that a shot and see if I can get it to work.

[tcaudle]

You can make it do just about anything you want. If you have the RS485 option you can even have a tool with a 10A current setting. It won't change the consumables for you but you can make the G-code snip send a message to the screen to remind you to change the consumables when it moves to the tool change position! Drop me an email if you want to include a message in the code snip.