Thanks! Appreciate it
Oops. Sorry.
In the Post-Processor screen in Fusion where you enter the “Delay” setting just enter it in milliseconds. In Fusion you only have one place to do that & it controls for all of the delays/dwells.
Sheetcam users can specify the setting for each toolpath they define.
Awesome!! Thanks so much. I thought I was going crazy with this!
1 Like
I just got sheetcam and I set the pierce delay in ms for each tool but when I post process, it still comes out in fractions of a second instead of milliseconds…
Example: G04 P0.25 instead of G04 P250
Any fix for that?
I’ve noticed this very same thing. I only have the trial version and was wondering if that was the reason… I’ve changed the time in sheetcam to ms also but, when you look at the G-code, it’s showing up in seconds, not ms… Still using Fusion here but, would like to resolve in Sheetcam sooner than later if possible… 
No. I believe it’s the Sheetcam Mach3 Post that’s the issue. Their post-processor assumes seconds because that’s the standard Mach3 install.
So you either have to alter the post-processor so you have a ms version or trick it by entering ms in Sheetcam (but telling it those are seconds) and then telling Mach3 in the General Config G04 setting to be ms. Sheetcam will not do the math in the post processor to convert your entry to ms as it’s doing by default but it is ms and Mach3 will be happy. Clear as mud eh? 
Here’s what’s happening in Sheetcam using their Mach3 post processor.
Sheetcam set for seconds
Enter 1 second
GCode is “G04 P1”
Sheetcam set for ms
Enter 1000
GCode is “G04 P1” which is not what we want. But it’s doing that because the post processor is coded to output in seconds.
The hack:
Sheetcam set for secs
Enter 1000 (milliseconds)
GCode is “G04 P1000” which we do want because our implementations of Mach3 is going to treat these as milliseconds.
So that’s the quick & dirty of things. You would think that Sheetcam’s post would output stuff correctly since we tell Sheetcam if we’re using seconds or milliseconds. But the post doesn’t do that.
I think I have a millisecond based custom Sheetcam post processor but before I upload it so people can use it I’d prefer another set of eyes on it. If you’re a Sheetcam user and want to test my post processor, let me know.
What I’m doing in there is changing the G-Code generation step to take the numeric portion of the Sheetcam G04 output and multiplying by 1000 to offset what Sheetcam has done when you specify ms in your Sheetcam settings (it’s converting to seconds and sending that to the post processor - mine simply reverses that).
i’ll test it out for ya. i was messing with the code last night and adding/deleting a few different things but couldn’t make it show milliseconds. it would always show P0.
I’ll toss it over to you tonight after I get back home. It’s not a huge change but I don’t want to eff up someone’s material without someone else trying it out too.
Ok sounds good… I’ll try it the other way you mentioned too.
Just remember to undo the hack when you try the new post processor or we’re going to be very confused 
That sounds great guys… Very interested to see how this goes… The other thing that was getting me was entering ms type number for pierce delay when setting up a tool in sheetcam… Then run the simulator in sheetcam and sit there and wait for 400 actual seconds… Wasn’t making much sense to me.
I’m probably ok with the hack for now but, the simulation would still be wonky… Right?
Right. But you can slide the speed bar all the way to the right to get some of the time back
1 Like
Right on!! Thanks James!
i just tried your “hack” and it seemed to work. I set time unit to seconds, restarted sheetcam, set the pierce delay in my tool to 300 s and post processed a simple file and when i opened the TAP file, the GCode line shows G04 P300
1 Like
Okay here’s the modified post for Sheetcam. Download it and delete the .dxf extension so it’s called “Mach3 plasma milliseconds.scpost” and copy it to your Program Files (x86) > Sheetcam TNG > Posts directory.
Then in Sheetcam, click on Options, Machine, Post Processor tab and in the middle click the down arrow and find the new Mach3 millisecond post processor. (ignore the blackout in the screen snip - it’s where I store my tap files and it’s got some network info that I’d rather keep obscured)
EDIT: Keep your Sheetcam using seconds for the pierce delay (in the tool setup screen) and the new post processor will convert to milliseconds. This one will come out as “G04 P500” which is 1/2 second or 500 milliseconds. Use ms in Sheetcam (like “500ms” to be 1/2s) and Mach3 will be happy with the tap file produced.
The post processor is attached as a fake dxf (since that’s what the forum allows) - you just need to strip off the .dxf so it’s a .scpost filetype.
Mach3 plasma milliseconds.scpost.dxf (4.1 KB)
Ok i’ll try it out. thanks!!
ok i imported it and set everything per your instructions and the tap file displays the G04 output to milliseconds, ie… P300 for example.
then, for shits and giggles, I went back to application options and set the TIME units to ms then edit my tools pierce delay to 300 ms instead of .30 and post processed using your modified post and it still output using milliseconds.
without actually running a live cut, i would say it works. I would keep the time units to MS in sheetcam to match mach3 and cut out the confusion.
Actually that makes sense the way I coded the post. Sheetcam sends a value to the post in seconds regardless of how you specify the units in your tool definition. My version of the post knows that and always outputs in ms.
So if you say “300ms” Sheetcam sends .3 to the post. If you say “.3s” it sends .3 to the post. I’m converting that to ms in the post (the default doesn’t - it just leaves .3 which is what Mach3 fails on if you’re doing seconds in Mach and if you had G04 milliseconds checked in Mach that would be treated as .3ms which is hugely wrong).
I’ll be using the new post to cut a couple of things for someone this weekend and will make sure it’s not doing anything bad. Then I’ll update this (probably start a new thread so it can be found more easily) with pictures & arrows and skip the “use seconds in Sheetcam” as you noted.
(I’ve updated the post above as well in case someone stumbles across this in the future.)
confused! lol. - but that’s easy for me. I need to do this conversion as I’m using sheet cam, mach3 and a finicky Everlast 60s
on a serious note, which set of instructions do I start to follow above? I’m gonna give this a run shortly.
If you’re going to use my updated post processor then you need to have Mach3 set to milliseconds. Then in Sheetcam specify your times as #ms in your torch definition. The tap file will work correctly for Mach3.