Sheetcam and trying to generate spotting gcode.

crowloy wrote:

looks like that will work. I posted on the sheetcam forum, since I believe that the issue shown above is still a bug. Not completing the operation before changing the setup is just wrong.

I don't think its a bug. Expected use is to use spotting on a seperate layer with a drill operation. This then locates the centre of the hole. You can't locate the hole centre on a jet operation.

rodw wrote:

I don't think its a bug. Expected use is to use spotting on a seperate layer with a drill operation. This then locates the centre of the hole. You can't locate the hole centre on a jet operation.

That is exactly how I have used it for a long time...

I did some work on the temporay materials and have a test branch if anyone wants to give it a try.

github.com/phillc54/linuxcnc/tree/phillc54/temp_materials

This was tested with the gcode that Rod posted on this thread so it should work with the PP that Les posted on this thread.

It allows any number of temporary materials so in theory you could have an empty <machine_name>_materials.cfg file and just use the temporary materials from gcode.

The only changes from a user perspective are that you can add a material name to a temporary file with the "na=" option. If you mix and match adding materials, editing materials, and temporary materials then all temporary materials must appear after any add/edit materials.

It uses material numbers starting at 1000000 so hopefully it won't conflict with materials in the <machine_name>_materials.cfg file.

The material change for temporary materials is also handled by QtPlasmaC and should not be in the gcode file.

LesNewell wrote:

File Attachment:

File Name: plasmac_20...4-28.zip
File Size:3 KB

forum.linuxcnc.org/plasmac/42374-sheetca...code?start=40#207300


I think there is a bug in the Sheetcam Plasmac Postprocessor done by Les in this link (I believe / it appears to be the latest)

post.NonModalNumber(", fr=", GetFeedRate() * scale, precision)

fr is coming out as "100", despite me setting it at "4800"

Sorry for the late reply but better late than never I suppose.
I can add more information if enough people want it.
snowgoer540, if you edit a post your edited version is kept in SheetCam's settings directory. Updates will not overwrite it. If the post name is shown in the post list with (edited) at the end of the name, it is in your settings directory.

Roberspark, I can't replicate your feed rate issue. Just a thought - are you changing the tool's feed rate? The post uses the operation's feed rate which may not be the same as the tool feed rate.

I've found a couple of bugs in the sheetcam postprocessor (and one in QTplasmac too).
I've also edited it to support QTplasmac's hole processing modes which is on by default
I've posted it on the sheetcam forum but a copy is also attached here. Hopefully Les will take the revisions back into Sheetcam's post processor library
forum.sheetcam.com/viewtopic.php?f=5&t=8651&p=29441#p29441
 

Delete the .txt extension before use.
If you don't want to use the hole processing. edit the post and set holeMode = 0

So the post I shared above and on the sheetcam forum will find its way into the next version so it would be good to test this

What is hole processing from  QTPlasmaC and how is it used? I did not find the qtplasmac docs on it.

I am using the rules in sheetcam to slow the feedrate to 50" on holes smaller than .5".

bevins wrote:

What is hole processing from  QTPlasmaC and how is it used? I did not find the qtplasmac docs on it.

I am using the rules in sheetcam to slow the feedrate to 50" on holes smaller than .5".

By default it is slow to 60% for holes < 1.26" (32mm)
There is another mode that also applies the slowdown to arcs < 16mm (50% of 32mm) which will be good for slotting
And another mode does an overcut (default 4mm) at the end of the hole

All of those numbers can be overridden using gcode variables like #<h_diameter> = 0.5So basically with the combination of the rules and velocity anti dive means you should never need to use sheetcam rules

It would be good if you could give that post a whirl to confirm the imperial settings work. Just view the gcode and you'll see whats going on in the preamble