Rounding the corners off

Many thanks,
This is what I believe happen to the sample above, the G61 post I used a manual set tool selection (as to increase feed rate) and that is the one. This is what I tried today, used "the lowest plastic feed rate, from table" in material selection for the stock, this cut at 60"/min max, cut to corners.

many, many thanks!

If you want to try making the machine move alot faster, try replacing every G61 in the file with G64P0.001.
That should significantly increase your feed rate through most corners that are not very sharp, but still maintain pretty close tolerances. You can then play with the size of the P value in the G64 command to find the right balance of speed and precision for your needs.

Running both of the G-code files you posted above in a simulation does not produce the corner rounding you showed above. (the file has G61s in it) Replacing the G61s with G64P0.001 still shows no detectable corner rounding in my simulation. In order to produce paths like you are showing I have to remove the G61s from your file and set G64 with no P tolerance.

PS: G64 with no P is the default setting when Linuxcnc is started. This is one example of why it is so important to have a proper preamble for your G-code files in order to put the machine in the correct state for properly milling your file regardless of the machine's state before you start the file.

Some codes I would consider essential for a proper preamble:
G20/G21 (T0 set the proper machine units to inches or mm.)
G17/G18/G19 (To set the proper machining plane.)
G90/G91 (Set the machine to absolute or incremental)
G40 (cutter compensation off)
G49 (Tool length compensation off)
G64Pn (Path blending with tolerance; n=some number such as 0.005)
G80 (Canned cycle cancel)
G94 (set units/minute feed mode)

Some other codes that could be very useful at the start of the file:
G7/G8/G9 (Flood or Mist coolant on/ coolant off)
G54 (or other G5x coordinate systems to set the machine coordinates as needed)
G92.2 (local coordinate system cancel)

Typically this happens when you tell LincuxCNC that it can go "so" fast but should only accelerate "so" hard.

When you configured the machine, what did you base your axis acceleration values on?

What _are_ your axis acceleration limits?

LinuxCNC will do what you tell it to do. If you tell it that it can only corner at 0.001g then you will get very swoopy paths.

Many thanks andypugh for all your great help for me and all the members! I have only recently cut other part with some rounding with it as well and the feed rate was way slow, I will look and try to understand all that you and Todd Zuercher have described. Both of you are complete and total gentlemen all the way thru, many, many thanks for you great help! The axis acceleration values, not altered from installed; the axis acceleration limits (I will need to check).

thanks!

edit:the max_acceleration=10.0, this was the original setting I believe. I am still working on the gcode preamble. many thanks!!

Many thanks Todd! I am not completely shore if this is of any value, the Bobcad has in the selection of tools, a set of options with a spot to set the "slowdown for the corner", it offers a 100% slow down, I just think that would do it. I will look and try to understand all that you included in your response. Help me understand what one should expect from cutterpath software, will I be able to set up a master template with the essentials, like you describe included? Should when cutting a pocket, to get the best most efficient path will I need to edit, most times? Like the example above, it had some long runs with tool not cutting. The mist is manual. Todd, many thanks for your help, I really appreciate it. Is there a way to simulate in linuxcnc w/o running the machine, so you don't have to tie the machine up?

many thanks!

Todd, many thanks to you for all the great help! I included the gcode as per your suggestion, this included the the following: G20 G17 G90 G40 G49 G64P0.001 G80 G94. In the attached file you can see that I have edited out some of these (using the find & replace) because there were doubles in that line when I would view it after it posted a gcode part file, and the linuxcnc would error out. Now it errors out around line 25 (as per linuxcnc).
From reading there is a debug mode, should I be working with that? Or should I just insist that Bobcad (they are based out of FL, so the storm is am issue) provide working post, I am right on the very end of support.
This is the post as I left it.

many thanks!