Strange circles added in gcode

[MS]

Hello!
I'm starting with CNC and gcodes. I ran into a problem when generating gcode.
I draw some shapes in inkscape, in this case letters "MG", conveted to path and saved as dxf.
In dxf2gcode imported this file and added tool compesation for 5mm tool and exported gcode.
In openSCam on simulation everything is good, but in linuxCNC strange circles appeard.
Why is this happening? How can i avoid this situation?

My second question is what  in layers tab means "start rad. (comp) 0.2"? For example when i want to use 5mm tool what should i write there in config file?

Best wishes

[Christian Kohlöffel]

Hello MS,

the strange circles you may see are the lead in moves of a contour. They are based on the parameter "start rad. (comp)" by choosing this value as low as possible you are able to reduce them, but since this is the only type of lead in which is implemented in dxf2gcode it's just possible to reduce them to a minimum but not to avoid them. The value is given differential which means it's not dependent on the tool diameter you use. By setting it to 0, it would disappear. However i don't think that EMC can handle that. Try to have it just like 0.01 and it may work while you even will not be able to see it. this will only happen if you add tool compensation.

regards
Christian 

--
--
You received this message because you subscribed to the Google
Groups-group "dxf2gcode-users".
To post a message, send mail to dxf2gco...@googlegroups.com
To unsubscribe, send mail to dxf2gcode-use...@googlegroups.com
See http://groups.google.de/group/dxf2gcode-users?hl=en for more options
and the dxf2gcode project page at http://code.google.com/p/dxf2gcode/
---
You received this message because you are subscribed to the Google Groups "dxf2gcode-users" group.
To unsubscribe from this group and stop receiving emails from it, send an email to dxf2gcode-use...@googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

[MS]

Thank you for reply.

I think maybe i didn't correctly described my problem
Maybe this screenshot will explain this better

I undestand that leadin move is need for compensation but i have different circles there ;/

[Christian Kohlöffel]

Sorry,

now is see the problem. I think this is a accuracy problem of EMC2 or of
the view of EMC2. Does the maschine also produce the same circles. I had
the same problem within the graphics of DXF2GCODE but this was just a
graphics problem. This problem can only be solved by EMC2 or by
modifying the GCODE itself. It's not produced by DXF2GCODE.

regards
Christian

[Anders Wallin]

does dxf2gcode output "R-style" or "IJK-style" arcs (G2 and G3)
with the R-style there can be some ambiguity due to numerical instabilities - probably what you are seeing here.

Therefore the IJK-style is probably preferred as it unambiguously defines where the arc-center should be.

Did you run this on LinuxCNC? Did linuxcnc follow the path shown in the preview - OR very strangely did it actually cut the letter-shape OK and the preview is plain wrong!?

AW

[MS]

So here is how it looks like:
LInuxCNC is moving along this circle path - but the lines in gcode are not changing when moving on circle move. I think this is normal behaviour. But in openscam there was no circles...

I've uploaded short clip when my diy machine is moving along this path (in air), it's around 28 second

http://youtu.be/s8suKJyD3QI

How can i prevent this situation? Is this linuxcnc bug?

First circle is on line: 1129, it goes into a circle in this point where I placed mouse cursor. (I and J style is used)

[Anders Wallin]

Can you pastebin the G-code for this somewhere?

Maybe just a minimal example near the line 1129 that causes problems?

I'd be quite surprised if this is a linuxcnc problem.

Clearly you are getting an anticlockwise arc when you want a clockwise arc (or vice versa)!?

AW

[MS]

Well, if I remeber correctly, it was anticockwise direction.

http://pastebin.com/YSnVrQbv here is the code.

[Anders Wallin]

Looks OK to me!
http://imagebin.org/321557

latest linuxcnc master from git, i.e. "2.7.0-pre0"

maybe post that g-code pastebin link, your tooltable, and the linuxcnc version you are using to the linuxcnc-users list and see if someone else can reproduce.

Anders

[MS]

Just installed debian and linuxcnc 2.6.3. Still the same
Can you show me your tool table in linuxcnc?

I think i will have to post this  on linuxcnc-users...

[Anders Wallin]

Only T5 was used, and I just put diameter=0.1 I think, to have something there. What do you use?

Since this is programmed using G42 cutter-compensation, the tool diameter may indeed have an effect!

the problematic line was G3 X   6.205 Y 176.582 I  15.844 J  -9.274

if we take sqrt(I*I + J*J) I would get that the programmed radius is 18.3586331735

now depending on the combination of G41/42 and G2/G3 this move is not possible to complete with for example a D=20 cutter!

So in fact it may be the case that dxf2gcode asks linuxcnc to perform an impossible motion!?!

Anders

[MS]

Sorry i couldn't check earlier...
I have there DIAM 5mm.
Will check now with smaller diameter.

[MS]

With diameter 1 for exmaple, in linuxcnc there is no circles :) , so what settings in dxf2gcode should i set for 5mm diam? What "start rad" should i set and how to measure this value for different tools?