Different cut speeds. <Resolved>

[AWFAB]

If Im using sheet cam and I set the speed to say 50 for a hole then 120 ipm for the outside, the centroid acorn ignores it and sets the speed the same for the hole and outside at what it is set in the profile manager. Its cool I can change the speed in the profile manager but I want the hole one speed and the outside a different faster speed, how do I do that?
THanks

[Joey]

The M61 in the Gcode calls the Profile manager information.

So the commanded feed rate will need to come after the M61 on the Cut you need to slow down.

You can do this in sheetcam by creating a Path rule to slow down by a specified percentage.

I think the reason the sheetcam does not put in a commanded feed rate after the M61 is because of the specific Post.

The current Post available on the forum will need some edits to get the feed rate posted

[Joey]

Heres a Post that should do what you're looking for

centroid_plasma_thc_sheetcam with optional feed.zip

(1.51 KiB) Downloaded 40 times

If you edit the post and change the second line to:
useFeed = false

Sheetcam Feed rates will not be posted in the Gcode

If you edit the post and change the second line to:
useFeed = true . It will use SheetCam's feed rate.

[AWFAB]

I installed that post and it said use feed rate equals true.
I made 4 of the same circles and one at 20 ipm 40 ipm 60 ipm and 80ipm
It ran them all at 61 ipm with smoothing off
Then I turned smoothing on and it ran each one at 220 ipm
I got to look at a bunch of videos whatever I did wrong Im sure its simple.
in the profile manager it was set to 100 ipm

[AWFAB]

I should also say im in drive type bench test still if that matters, but xyz moves exactly the amount it says it does.

[Joey]

Looks like that post was converting all the feed rates to Metric.

This post should post in Imperial

centroid_plasma_thc_sheetcam with optional feed.scpost.txt

(3.85 KiB) Downloaded 49 times

[Joey]

I installed that post and it said use feed rate equals true.
I made 4 of the same circles and one at 20 ipm 40 ipm 60 ipm and 80ipm
It ran them all at 61 ipm with smoothing off
Then I turned smoothing on and it ran each one at 220 ipm
I got to look at a bunch of videos whatever I did wrong Im sure its simple.
in the profile manager it was set to 100 ipm

That first Post was converting Sheetcams commanded feed rates to Metric. So if we could see your Gcode I Bet there was a F1270 in the Gcode.

Your machine could only run the Circle at 61ipm with your current Accel/Decell and Overall Turns settings. CNC12 was trying to run F1270 ipm but could only do 61ipm with your settings.

With Sheetcam putting in Commanded Feed Rates, that will override the Profile Manager. If you Set a Tool in sheetcam as 0ipm speed then Sheetcam will not insert a feed rate and CNC12 will run that cut at the Profile managers Feed rate.

[AWFAB]

That last post did it can control all speeds from sheet cam!
Thanks Joey