Forgot to mention...

[booski]

Could have done with this tonight

Milled a board using a 0.1mm pyramid engraving bit. Yes, the edges are a little rough as it's really rubbing material away rather than cutting but WOW can you do fine traces with them!

Except, I used my program file for a V at 0.05mm depth cutter rather than pyramid and it despite cutting, it was so small that the surrounding copper started to peel when the rough edges where smoothed over, it could have done with another 0.05mm or 0.1mm extra depth to make it a little wider. Unfortunately, I couldn't do that

[booski]

I've just realised something.
Am I right in thinking that when LinuxCNC probes an area the values are stored?

So, if I wanted to re-cut the area, all I'd need to do is is simply use the 'run from here' option and skip the probing g-code?

[Country_Bubba]

Yes, I believe they are stored in memory so as long as you do not exit linuxcnc they should be there.

[daedelus]

I just had a look at the LinuxCNC gcode page myself. Here's what it says about parameter persistence:

When LinuxCNC is shut down, volatile parameters lose their values. All parameters except numbered parameters in the current persistent range [1] are volatile. Persistent parameters are saved in the .var file and restored to their previous values when LinuxCNC is started again. Volatile numbered parameters are reset to zero.

It also says:

The range of persistent parameters may change as development progresses. This range is currently 5161- 5390. It is defined in the _required_parameters array in file the src/emc/rs274ngc/interp_array.cc

So, although Art is correct and it should store probed values, I have used the range 500-1000 (which is correct for Mach3) in the autoleveller output, so for LinuxCNC it will not store the probe values probably. This is an easy fix to make however and I will do it ASAP.

Incidentally Art, do you know what this range is for TurboCNC? If there is a range that is. I can then make a TurboCNC option in the autoleveller which will use this range.

[Country_Bubba]

James,
Here you go directly from the manual:})

"There are 10000 of these locations available, each named with its location from 1 to 9999. Variables numbered 1 to 999 are persistent, meaning that their values are stored in the configuration file upon exiting TurboCNC and re-loaded when TurboCNC is restarted. Variables with names from #1000 through #9999 are transient. "

As as I am basing my processor on the Mach profile, I am using its variable range so we are already covered as to the range that is stored. 1-999

[booski]

OK so for the sake of saving a little confusion lets summarise.

1. Linux cnc saves all the probe point variables to a .var file.
2. There is a section of this file that is non volatile as defined elsewhere
3. Autoleveller saves variables to the volatile memory.

This is important:

4. Linuxcnc variables are only erased WHEN the software is restarted

In this case, should you cut a board and there are air cuts, you can skip the probe code and run the in the autoleveller file and recut SO LONG as you dont restart the program.

Thats good to know. Might have to test it.

With linuxcnc, if the non volatile variables are pre defined, couldnt you change the definition file to include the variables you need?

[daedelus]

Yes, I dont see why not but not everyone who uses the autoleveller will do that or know how, so it is best if the change is made within the autoleveller itself.

I have made the changes to the autoleveller and am just testing before I upload the new version.

Regarding point 4. I dont think this is true. When I tried this a while ago and I clicked on stop then resumed from a line past the probing section the variables were reset even though I never closed LinuxCNC down. I could be wrong though.

[daedelus]

OK I have changed and uploaded the changes. The latest version on the download page (still 0.7.7) should use the new range for LinuxCNC. The Mach3 version should be unchanged.

Let me know if theres a problem with it.

[dunkum]

What I would like is an equivalent in Mach3 and others, so if anyone knows how to do it then please let me know.

In Mach3 there is a function, OpenDigFile(), which gets the probe trigger positions written to it from G31 commands. A simple(ish) script to probe a grid and output the Z data to a file is thus achievable.

I would like to pursue this approach since I generally drill before etching, and probing a board full of holes is going to end in tears at some point. The reason for this sequence is because small pads with thin annular rings can be pulled off by the torque from a drill bit, but that same ring is more robust when etching round it. Thus it is better to etch a small pad after drilling than vice versa.

[daedelus]

Thanks dunkum, From my brief googleing, OpenDigFile() does a similar thing to the M40 command. M40 might be easier to use from the GCode itself. Not sure, I shall investigate this.

Great tip about the order of CNC operations by the way, but for now you might need to risk milling first and drilling 2nd.