Wrapper Plugin

[dh42]

Hello,

Apart from:G2/G3, G81 ...G89, are there any there any others that might or should get flagged?

There is no other that come to my mind ...

There is no G89 defined in the cambam PP, ... there is a G98 but I never see it in any Gcode ; not sure it is used.

++
David

[kvom]

Given that users can add any gcodes in headers, footers, and drill scripts, I'd flag anything that looks wrong.

[GeoffreyGRoy]

Here is the new version of the Wrapper plugin that includes warnings on invalid G-Codes (for wrapping) - both in the code and user doc.  I think I have identified most of the invalid codes - but I may have missed some - please let me know if you find any missing.  The plugin will still produce an output file even if any invalid codes are found - only a warning is given displaying the line in the G-Code file containing the invalid codes.

I am also attaching the sources as requested by Armando

Geoff

[dh42]

Hello Geoff,

It seems that the .dll in the .zip is the same that the previous ; it is called 1.0.3.0 and it don't detect the G2/G3 (but it's the 1.0.4 doc)

++
David

[GeoffreyGRoy]

Oops! Here is the correct 1.0.4  dll version

Geoff

[dh42]

Hello Geoff,

For an unknown reason, with some files the G2/G3 are not detected and I get no warning.

I attach a file that give the warning (test_ok) and the other that give no warning when conversion (test_bug)


- in the warning window, the list is very long and it can't be moved with a slider ; maybe it's not really useful to list the errors ; I think that the warning alone is sufficient.

- when converting long gcode, a progress bar can be useful, because one would think that the PC is crashed.

++
David

[GeoffreyGRoy]

Dear David

Thanks for the feedback, I obviously did not test a file with a large number of "errors".  I have removed the list or "error lines" from the warning dialog, just included the number of lines with "errors".

I cannot see any problems with test_bug.nc file - the only explanation I have is that the warning dialog was so big that it failed to display "correctly".  As far as I can tell both files (now) give a reasonable dialog.

Updated version attached.

thanks again

Geoff

[dh42]

Hello,

Ok, that works for me too !

Thanks 

Thanks for the feedback, I obviously did not test a file with a large number of "errors"

And the first Gcode where I found this problem is ... 7Mb lol (3D) ... a long time to compute (maybe an "abort" button can be useful too)

Good night
++
David

[dh42]

Hello Geof,

I found a little problem with wrapper if I use of G53 in the Gcode.

In my code, I've a G0 G53 Z-1 to retract the Z to the highest Z pos in machine coordinates. (minus 1mm)

problem, after the code is wrapped, the G0 G53 Z-1 is changed to G0 G53 Z19.25 (because diam = 40.5 and Zbase = 0)  ... and it should not, of course ...

++
David

[GeoffreyGRoy]

Dear David

Please try out this new version where I have looked for G53 codes, and left that line un-transformed.

There may be other G-codes that need to be treated in this way, any advice would be appreciated.

thanks

Geoff

[dh42]

Hello Geof

Thanks for the new version ... and the very quick answer !!

++
David

[kvom]

I used this today for a cylindrical engraving test piece.  Worked perfectly.  Needed to use the reverse checkbox as my axis is mounted on the left of the table.

Mach3 doesn't display the toolpath as it does for planar work.  It just ignores the A moves and shows a bunch of lines on the x axis.

As for the Z values I think it makes better sense to regard Z0 as the top of the stock rather than the centerline of the axis, since it's simpler to touch off on the stock.  Alternatively a button to calculate and insert half the diameter as the Z base value.

[Bubba]

As for the Z values I think it makes better sense to regard Z0 as the top of the stock rather than the centerline of the axis, since it's simpler to touch off on the stock
*****************
I strongly disagree. It is widely accepted practice in the industry to have the Z0 at the centerline. In my case knowing the distance between the centerline and the top of the tailstock setting the Z0 is easy.


"Mach3 doesn't display the toolpath as it does for planar work."

Are you sure about this? Mach3 on my machine displays rotational toolpath,
 

[dh42]

Hello,

Are you sure about this? Mach3 on my machine displays rotational toolpath,

Yes, me too ..

https://www.youtube.com/watch?v=1gAxXwLRjQw

++
David

[kvom]

Thanks for that.  The youtube video solved both the toolpath display issue and also the timing issue I had with coordinating the axes.  Seems the radius setting in the Settings tab is ignored unless the Use Radius box in the Toolpath dialog is checked.

Checked both the appropriate fields in the Toolpath dialog and all is well.   

As for Z0, I won't be using the tailstock often, so using it for setting Z isn't practical.  I think having a button to set Z0 as half the defined radius is an innocuous addition.