unwanted radiusing in LinuxCNC 2.8

I've recently upgraded from the Ubuntu 10.04 ISO version which for both my Sherline 2000 and Chinese 6040 Router was very effective and completely trouble-free.

But alas, the need for swifter graphics in my system's HP Elite 8300 led to the purchase of a Nvidia Super 1650. There was no driver available for Ubuntu 10.04 for this card, so I installed the Ubuntu 18.04 RTAI kernel and the additional modules required to make it work and (Voila!) it did work.

But I now have a problem I didn't have before.

Among other things I use the router to etch Printed Circuit Boards. The G-code for the boards is generated by a Plug-In ULP named pcb-gcode which converts an Eagle file to the Gcode needed to drill holes in the boards, etch and isolate the traces and mill the perimeter so that the board will have uniform dimensions and fit the box it goes into.

This has worked flawlessly for years using LinxCNC 10.04.

But look at his:


The arrows point to where the isolation trench adjacent to the trace has been radiused. These are not in my G-Code

They do not show if I run the code in CAMotics - a nifty visualizer which shows what the G-Code will do. Clearly this is something which LinuxCNC is doing. And with no consistent pattern although most of these are inside radii.

They do show up in the visual screen when LinuxCNC runs the code and of course they get cut. Initially I thought this was really only a cosmetic problem and for sure no-one else would know about them, but it wasn't that simple. I found a place where the radius in trench was cutting an adjacent trace - cannot have that!

Where should I look for the source of this problem? I did have to do a new stepconf for the router because the old one wouldn't load- not compatible with Version2.8. Could I have screwed up my INI?

Should I add a G64 statement to each job?

I would rather find out how this is happening and fix LinuxCNC itself.

Where would you look?

John Ferguson

G64 is the way to go. By default Linuxcnc prioritises velocity when moving. By adding G64, it tells the system how far away from the planned trajectory it is allowed to go so it forces deceleration to keep to the path. Most of us have learnt this lesson. In my case it was tracing 1.0m x 1.0m square on my plasma table and it was almost a circle.

how wonderful that this could be so easily fixed. I can add this line to the default front end of every file output from pcb-gcode and hopefully not have to worry about it again.

Thanks much to both responders,
john ferguson

a circle rather than a square and at that size. amazing.
It's nice to find I wasn't the only one to encounter this problem. Wouldn't you think how LinuxCNC prioritizes tracking should be a toggle somewhere.

Or maybe G64 is the toggle.

jferguson wrote:

Or maybe G64 is the toggle.

It is. You can add it to your startup code in the ini file

RodW,

I've got the 2.5 manual, have looked at my INI files and can find no startup code nor have I found out how to add it.
If you do have this in one of your INI files, could you attach a copy here?

I can pretty easily add this to the Eagle pcb-gcode routine, but it clearly would be better to have each of my machines set to G64 P0.015 or so.

Can I assume that the 0.015 above is 15 thousandths? My boards are pretty crowded and 40 thousandths seemed too much.

It cost a bunch to have the 2.5 manual pdf printed out. Is there a 2.8 manual and if so do you think it would be worth while to have that printed?

thanks much for helping me solve this annoying problem.

Have a look into f.x. 2.8 docs...
linuxcnc.org/docs/2.8/html/config/ini-config.html
....
2.4. [RS274NGC] Section
.........

RS274NGC_STARTUP_CODE = G17 G20 G40 G49 G64 P0.001 G80 G90 G92 G94 G97 G98 - A string of NC codes that the interpreter is initialized with. This is not a substitute for specifying modal g-codes at the top of each ngc file, because the modal codes of machines differ, and may be changed by g-code interpreted earlier in the session.

You say: "This is not a substitute for specifying modal g-codes at the top of each ngc file, because the modal codes of machines differ, and may be changed by g-code interpreted earlier in the session."

I think I'm lucky here. LinuxCNC seems to be the last G-code reader on my chain. Machines are dumb and in my case take only x,y,z axis direction from the LinuCNC in my computer.

It looks like I should write: "RS274NGC_STARTUP_CODE = G17 G20 G40 G49 G64 P0.001 G80 G90 G92 G94 G97 G98 " in the line under "PARAMETER_FILE = linuxcnc.var"
which is all I have in this section now.

Thanks much.
john
It looks like I put my version of "

If you look at the documentation linked to its for the ini file. SO place your code there....