Sheetcam and trying to generate spotting gcode.

LesNewell wrote:

Another spindle question - What are the spindles actually used for? At first I assumed they were used to select offsets but looking at the manual I see you need to use tool offsets as well.

M3 $0 S1 = Start the plasma cutter
M3 $1 S1 = Start the scribe after loading T1 to apply tool offsets for the Scribe.
M3 $2 S1 = Start a spotting operation
Spindles >= #3 can be used for any other feature that has a spindle.

Scribing is explained in the QTplasmac manual here
linuxcnc.org/docs/devel/html/plasma/qtplasmac.html#qt_scribe
and Spotting is the heading immediately following

Each spindle has its own spindle.N.on signal in hal which is used to energise the torch $0 and scribing tool $1
Setting the offsets to the scribe in the tool library using T1 was the simplest method to apply the X,Y offsets in keeping with the Linuxcnc paradigm.
When spotting was added, it seemed to make sense to select it with the $2 spindle as it was a way to tell Plasmac we were using the torch in a different way to $0.

If another tool was added such as a drilling head or a router, I always envisaged it would be used as Spindle $3 and the precedent set for the scribe was followed. But nobody has needed this yet so its never been formalised.

Here is a post to try.

I tried to keep the look and feel close to Phillc54's original with a few changes:
It does not use tool names to control functions
Feed rate override from action points or rules now works (within the limits of M67 E3).
It can be configured to automatically generate temporary material file entries based on SheetCam's tool table. This effectively overrides the Plasmac material table.

This is a test release so there may be issues. I wouldn't recommend using it to cut a big sheet of expensive material

Cool, I'll try and test this later today (says he at 3:00am)

I can confirm that this new pp produces gcode for both spots and cutting without the user switching tools.

One thing I noticed:
Line #161: I believe begin cut gcode should be M3 $0 S1
www.linuxcnc.org/docs/devel/html/plasma/...mac_specific_g_codes

Where does the user set the cutAmps variable for a tool? I'm not seeing an input box for it in the jet tool dialog box.

[ edit ]
I've been farting around with sheetcam trying to find an answer to my previous question. If the pp has any DefineCustomToolParam lines then sheetcam will add input boxes for these lines in the tool dialog box after sheetcam sees these params in the pp (either when loading or after running the pp) Does that all sound correct?

Also, the Pause at end of cut variable doesn't appear to do anything. Honestly I don't know if it worked in the original pp either. A pause is at least necessary for the hypertherm powermax 45xp. I found I needed at least 10 seconds between spots, I believe this is consistent with at least one other 45xp user's experience here on the forum and with what my user manual indicates... but chances are better than decent I'm just doing something wrong with my cutter's settings. I only need this for spotting, and I think it has something to do with the 45xp not detecting a arcOK for at least 0.5 seconds.

Anyway, I previously hacked the pp to achieve this before realizing there was a pause setting in sheetcam. Utilizing the pause setting would be ideal.

I propose adding this to OnDrill and OnPenUp

AgentWD40 wrote:

I can confirm that this new pp produces gcode for both spots and cutting without the user switching tools.

One thing I noticed:
Line #161: I believe begin cut gcode should be M3 $0 S1
www.linuxcnc.org/docs/devel/html/plasma/...mac_specific_g_codes

Where does the user set the cutAmps variable for a tool? I'm not seeing an input box for it in the jet tool dialog box.

[ edit ]
I've been farting around with sheetcam trying to find an answer to my previous question. If the pp has any DefineCustomToolParam lines then sheetcam will add input boxes for these lines in the tool dialog box after sheetcam sees these params in the pp (either when loading or after running the pp) Does that all sound correct?

I agree with the S1, Linixcnc needs a spindle speed.
To enable your RS485 features, there is a flag at the top that should be set to true.

I don't have rs485 on my machine. I modified my pp to add a custom M100 P<amperage> that pauses linuxcnc and executes a python script that shows a QMessageBox in big bold red letters to manually set the correct amperage. Is this something that would be useful to others? If so I can share the python script, and I'd suggest making those rs485 settings always available.

AgentWD40 wrote:

I don't have rs485 on my machine. I modified my pp to add a custom M100 P<amperage> that pauses linuxcnc and executes a python script that shows a QMessageBox in big bold red letters to manually set the correct amperage. Is this something that would be useful to others? If so I can share the python script, and I'd suggest making those rs485 settings always available.

I think its best to leave this out of the current discussion as its not a feature of the current post.
There is only one brand of machine with the RS485 and its an added cost feature so its best to leave it disabled. Many users (probably the majority?) use a different brand of machine...

rodw wrote:

I think its best to leave this out of the current discussion as its not a feature of the current post.
There is only one brand of machine with the RS485 and its an added cost feature so its best to leave it disabled. Many users (probably the majority?) use a different brand of machine...

But that's my point. Most cutters have adjustable settings correct? But we can only talk to one specific type of machine. My question is if we could broaden the usefulness of these settings to a larger audience.

Given the context of the linked thread from the sheetcam forum and Les jumping on to rewrite the pp I figured this was as good a time and place as any to discuss.

I'd be willing to write an 'official' PlamaC post. Maybe it's worth starting a thread on the LinuxCNC forum to discuss PlasmaC's requirements.

Or was another thread started that I overlooked?

With the exception of this line which I edited before I started, the post seems fine.
I got an error loading the magic comment version about it taking too long. But I don't think thats a post issue.

I have a lot of tools on a 120 amp machine so I think Plasmac probably needs to wait a bit longer. It must process those comments in the gcode filter.

I really need to upgrade to QTPlasmac as my version is quite old!