I’d like to incorporate this all in one gcode file. I have a bracket I’m building but I keep getting an error that it can’t cut the 1/8" holes, so I’d like for just a simple spot pierce at least and I can drill them out.
Not sure what the issue really is. I’d hope that the machine would at least TRY to cut out the 1/8th" holes, but in fusion, during the 2D profile creation, it discards the contours for the 1/8" holes.
Using Fusion 360 and Crossfire with Mach 3
look up arclight sheetcam videos on YT or drill/center punch with sheetcam.
I switched from Fusion to sheetcam, soooo much easier but I assume you are also using fusion for creating drawings, all my drawings are done in solidworks.
How I used to do it in fusion… My kerf was 0.055 so I set the hole size 0.056" on the holes I wanted center punched. Create a new 2d profile for them holes only but make sure to select no lead on or lead out.
I do it the same way you do, now I use sheetcam. Although for some reason it would not work until I set the pierce delay to at least 400ms. Not sure if that’s due to the delay in the system and relays etc. (I use the razor weld 45 and the crossfire pro table)
so that would be two separate g code files to run with Mach 3, correct?
I’ve heard strange stories about mismatch of pierce delay and actual pierce timing on the FireControl system. Do you think the torch timing is actually less than 400mS?
I find 150-225 leaves a pretty nice tic, but I have modified the practice a bit after a suggestion from @jamesdhatch to try it without going to smaller tip. It seems to work well enough with a 40A tip that it’s probably not worth swapping unless you really want a nice tight central punch.
In fusion before you click the button to generate your g-code make sure all the 2d profiles are selected. It will put it all into one job then. The highest in the list will take priority so you will want to do any pilot holes before outer cuts incase the part moves.
As you say it leaves a tiny indent in the material so I do think it fires less then 400ms. Under that value it would not fire at all. It’s a quick flash and it’s all over.
I keep the same tip and the same power as per the job and just run with it. I created a separate tool in sheet cam so I could alter the heights and delays etc the run it as a drilling operation. I’m not at my computer now but I’ll post the values tomorrow for reference to help anyone else.
Yeah, exactly. That’s the key. Put all your ‘holes’ on the same layer and same ‘Drill’ operation. I’m interested in seeing your settings.
I’ve been using the 45A setup and just have a tool setup with a quick pierce and get good results on aluminum and steel. The peck is around 0.7-1.0mm and seats a drill bit nicely.
Here is the settings I use…
I assume you do a ‘Drill’ operation since that’s the real ‘secret sauce’ here…
FWIW, your pierce height is a tad higher than mine. I use 0.093" (2.36mm) and, of course, as we discussed, spec a shorter pierce delay (150-225mS). I also spec a pause at end of cut (250mS) to make sure the torch is off, but I can’t attest that does anything useful except make me comfortable 
Thanks for posting!
Your welcome. Yup, I put all my holes on a separate layer and call them as a drill operation.
can someone guide me a little here on this “drill operation” setup?
I’m down to use a separate gcode file if it will allow me to add pilot holes for drilling.
check out the archlight videos on YT. pretty good explanation on how to configure it. There are also a few others. Search for sheetcam drill operation or sheetcam center punch.
As a quick and dirty guide…
Add a new plasma tool so you can give it the settings needed to only pierce and run. You can use the settings I posted above and go from there for starters
You will need to create a new layer on your part with the holes you want to punch. (I think there is a way to auto select holes under a certain size but I prefer to make a new layer). To make a new layer, control and click on the holes you want to select, making sure at the top you have contour tool selected. Once you have selected the holes right click on any of them and choose create new layer. Give it a name like center punch or something.
In the operations box, click on the drilling operation (2nd one down). It will pop up asking you to select what layer, choose the layer that you called your holes, then choose the tool to what ever you named your tool.
Its also going to ask you what size holes, I think this is the part where you can make it auto select holes from one layer with in a certain size. Since I have all my holes on one layer i don’t need it to auto choose so i set the upper limit to 1". Before I done this it would not let me drill my holes as they were over the tolerance in this box.
If all went well you should now see the tool path on you part that runs around the holes. Do this operation first before any cuts as the piece could move on the table once its cut out.
Another thing I do, right or wrong is keep all my settings in a template. I’ve lost count the number of times I’ve lost tools or path rules by not saving the tool set. So i keep a template updated every time I make a change and every time I want to cut something I load up that template.
Forgot to add, this will give you one g-code file with the rest of your cuts. No need for multiple files. If you watch the archlight video it runs through all this on his screen to follow and shows more ways to select holes rather then control and click etc.
This is all instructions for sheetcam. If you are using fusion its a little different but I would recommend downloading sheet cam and trying it out. You can cut small parts free until you start getting into bigger parts or nesting. Having said that I was able to cut some large pieces free on sheetcam by breaking up the g-code but for 140$ its not worth the hassle.
Brand new here for crossfire and plasma cutting but I’m well versed with 3D printing and G code reading so my company just got our shop a crossfire pro and of course immediately guys want to start cutting holes basically smaller than the Kurf width and cut offset and lead in length combined so using fusion 360 it doesn’t even register the hole anymore. Is it better to use sheetcam? Does sheetcam just take DXFs, some machine settings and generate gcode pretty well or is it best to stick with Fusion for right now and if so what is best practice for just making single through holes by just piercing without xy movement or just a punch divet on surface through fusion360? Thanks for the help and I look forward to hearing from the community.
So would you say it’s best for the crossfire pro to just use sheetcam instead of Fusion360 then? Thank you and I’ll check out some videos about sheetcam soon.
