Cutting POM/nylon/Delrin ?

No, I am not using g64.
I am making toolpaths to follow arbitrary 3D shapes, and the actual velocity achieved is not as high as the requested velocity due to how emc2 interpretes accelleration.
It seems even a slight deviation in angle pr move is enough to make emc2 reduce velocity. If it didn't then a curved move should produce about 70% of the requested velocity in both axis when reaching 45 degrees. Starting and finishing at 100% for each axis except during accelleration and decelleration ofcource.

Now that I increased the accelleration a lot it is better but not even close to the velocitys I request.

I did a quick test now with the new velocity settings, and using G02/03 tracving a circle I get 600mm/min with F600.
Using G01 moves and making the same circle with an accuracy of 0.01mm using short line segments mapping to the arbitrary contour (yes yes right now it's a simple circle...) I get 570mm/min.
Close atleast. Before with my lower accelleration settings I was only getting 210mm/min with same circle.

Was hard to get high enough feedrate when the straights went at it 3x faster than the curves. Now it should be a lot easier.

Thank you!
Now it makes sence. The "come to a stop at the end of the move" part was the missing piece.
I simply assumed that, as long as the planner had more gcode to execute, it wouldn't be this silly.

I guess I should run with my required tolerance as the P parameter then.
Annoying though as all the code is generated by my cad sw and I really have no wish in editing it before execution. In fact I feel that the need for editing it proves the whole toolchain is faulty.

Well, it isn't all straight pieces. There's some short arch segments too when I run real shapes through there.
You can't very well make venus de milo in all archs, although a lot of her is curvey. I don't do simple pockets and machine parts, I do 3D fuse-shapes for rc boat, subs, planes and the odd uav as well as some art.

I see the gcode contains a G61 up in the top there. Looks like all I need is to swap that for the 64 and add my tolerance. I think I can rewrite the python script that is doing the readout as it should also have the tolerance value in the code.
I may suggest this as a patch for the HeekcCNC guys later as it is pointless to produce G61 code with full accuracy when at the same time have a user input box that clearly states 0.05mm. I get the feeling that it's not finished yet so we'll see.

I did run a new test today with red spirits (denaturated alcohol) as cutting fluid. Keeping the velocity on the finishing passes up I did notice a tad better surface, but not much.

I mostly get .stl files or other mesh files which are then translated into toolpaths for inner/outer or upper/lower etc.

kreature wrote:

Well, it isn't all straight pieces. There's some short arch segments too when I run real shapes through there.
You can't very well make venus de milo in all archs, although a lot of her is curvy. I don't do simple pockets and machine parts, I do 3D fuse-shapes for rc boat, subs, planes and the odd uav as well as some art.

I see the gcode contains a G61 up in the top there. Looks like all I need is to swap that for the 64 and add my tolerance. I think I can rewrite the python script that is doing the readout as it should also have the tolerance value in the code.
I may suggest this as a patch for the HeekcCNC guys later as it is pointless to produce G61 code with full accuracy when at the same time have a user input box that clearly states 0.05mm. I get the feeling that it's not finished yet so we'll see.

I did run a new test today with red spirits (denatured alcohol) as cutting fluid. Keeping the velocity on the finishing passes up I did notice a tad better surface, but not much.

could you use a bigger end mill? 5mm(.196") may give better results. don't know
if you need the groove around the half moon. and as for the feed/speed, you need to change
one at a time.either change the feed up and down to see any changes in finish. changing both
is harder since you don't know which one made the biggest change. your material looks like
polyurethane, if so that needs a "VERY" sharp tool. you could get a better finish on a lathe
and tool steel.(if you had a cnc lathe)