Gcode tools - lathe extension develop

Questions to discus

1. Cutting tool parameters
2. Additional lathe parameters
3. Lathe's Gcode features
4. Special places
5. ...

Desired features list

1. Special mode for 4axis mills
2. Automatic flip along axis

Awaiting of realization

1. Automatic flip along axis

Done

1. Path calculation
2. Export path to gcode
3. Defailt X and Z axis remap

Ok, I'll do it...

Now I'm finishing offset function which will provide a real final cut. For the rough cutting we offset a path by 0.1 mm and then do the final cut at the original cut as much time as we need.

Ok !
Very happy to test it !

Hi again!

Here what has been done in Revision 124:
1. Offset almost done. It works almost fine on not very complicated paths.
2. Offset have been integrated into lathe procedure. See the attachment.

What has to be done:
1. Offset bugfixing. (It might be not very important for lathe but if offset procedure gives two separate path it could lead to a problem - one of the paths could be not computed. It is not very important for the lathe extension because the offset distance should not be big, so the probability of separate loops is low.)
2. Export procedure . I have not done it yet, but I think that almost all is ready for it. So I think I'll write it soon.

This have been done in one click :

Revision 126

Lathe Export has been done and now it's ready for testing.
Unfortunately I have not any Gcode checker nearby now. So if anybody can test it I'll appreciate it .
After applying lathe should look like this:

Revision 127

Lathe now works on both ccw and cw (counter/clockwise) paths.
So now we can lathe a pawn from left to right and from right to left .

Ok for the I,J,K problem you must just add the G17 or G18 or G19 word before G02 command for select the good working plane because
the default one in EMC² is the XY plane.
For example when remapping in gcode tools is
X rempa to Z
and
Z remap to X
or X to X an Z to Z
The gcode after G21 must be G18 see the screenshot !
and gcodefile
gcode file:

If generate gcode for lathe config of EMC² : gcodetools remaping X to X and Z to Z .the AXE for arcs are invert in J and K see screenshot in next post for see the effect... big problem...
I must set remap with X remap to Z and Z remap to X to have gcode who show good shape in emc..
And must add the G18 after G21 !
And the last move for return the tools to G0 X0 Z0 was broken and Gcode tools have set G0 X0 "Y0"....that's block loading and running of the gcode in the EMC² lathe config...
After this change the code load and run good in EMC² config and in emc mill config and run like a Vertical lathe : Wonderful ! Big thank's for this that's give to almost cnc mill config to turn little part or Big part if big CNC or BIG mill that was convert to EMC ...

another problem !
If generate with lathe config setting for axis remap:
So X to X and Z to Z:
The gcode load look likes this one... I think it's because you have invert I,K coordinate for this mode.
Have a nice day !
Thank's again.

1. I'll add G18 or etc if plane is not XY.
2. The last G01 x0 y0 are taken from the default footer. You can add your own header and footers if you want (just add "header" and "footer" files into output directory).
3. Gcode breaks because of that X and Z axis have been flipped. If you flip the axis ccw turns to cw, so G03 and G02 has to be swapped. I'll fix that.

4. By the way are you using full version of inx file or not. If not try to run "python create_inx.py" and then copy all created inx's into your inkscape's extensions directory. A new section Gcodetools will be added into extensions menu.

Ok !
Yes I use full version of inx and have a menu gcodetools-dev in inkscape for 1.6 that's great! I download them from launchpad. Or with bazaar command you have done !

I'm not quite sure that you've understand me. So if you'll do what I've written, you will have separate for different functions which can be easier to use.

Revision 128

If I've done all right then I've fixed that bugs... But maybe I was wrong... somebody has to check it .

Effectively I'm wrong.
I'll do that you say to have separate windows for each function

I' have tried the ZX , XZ mode remap !
works in lathe mode and mill mode with ccw or cw . Cool !

The xy, yx doesn't work... giving now... invert arc...
And the YZ , ZY same problem arc invert.....

the g17...g19 plan selection is good.

Try now, should be fine now.

Hum I have done the test with rev129 and you say me to try now but no new revision ?

Ups... sorry probably I've forgot to make a push. Now it's pushed up to revision 131.

Ok ! Very nice !
All this fonction are working great.

I've think to another problem.
For example generate gcode remap to XY.
the tool is on the Y axis and penetration goes from Y+ to Y0.
If we want the penetration goes from Y- to Y0 we must setting
the tool parameter "penetration angle" to -90 !
But if setting to -90 that have any effect... I d'ont know wich is the role you want for tool parameter penetration angle ?

Perhaps adding a function to mirror an axis will be the solution ? with the remap function add some polarity setting to be able to set the polarity of penetration from axis+ to 0 or from axis- to 0 ?

Perhapas it is possible with 3-point modes orientation points ?
I'll must do some test.

Have a nice day.

I've try to change the polarity of the tool cut with miror with the 3 point reference but this doesn't work.

Yes we probably should add check box or something like that. Using orientation points to solve this is not correct.

The lathe goes from "Lathe width" to curves position. And if we flip the axis before the plug-in calculates lathe trajectory we'll see something like this, because the plug-in would not know that axis is flipped. I think we should do it using a post processor. We are discussing it right now at the Russian developing thread.
As the quick fix you can try add to your ngc at the top and do the following replaces. (Just ordinary replace not regex.)

" Y" to " Y#1*"
" J" to " J#1*"
"G03 " to "G0! "
"G02 " to "G03 "
"G0! " to "G02 "

This will flip your y axis.