Cutting POM/nylon/Delrin ?

More
01 Jun 2011 21:53 #10242 by kreature
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.

Please Log in or Create an account to join the conversation.

More
01 Jun 2011 22:20 - 01 Jun 2011 22:20 #10243 by kreature
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.
Last edit: 01 Jun 2011 22:20 by kreature.

Please Log in or Create an account to join the conversation.

More
01 Jun 2011 23:35 #10246 by BigJohnT
If you have not read this short bit it is important to understand how the trajectory planner works.

www.linuxcnc.org/docview/html/common_User_Concepts.html#r1_1_3

The EMC rule is never go faster than you can stop at the next end point based on the acceleration settings and velocity. That is why G64Pnnn (not G64) can achieve much higher speeds as it combines moves using the naive cam detector.

John

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 01:49 #10248 by kreature
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.

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 11:19 #10259 by BigJohnT
Well it is not being silly but safe. And yes you should change your post processor to give you the proper G code for the machine.

John

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 12:03 #10264 by andypugh
kreature wrote:

Annoying though as all the code is generated by my cad sw and I really have no wish in editing it before execution

Can you persuade the CAM software to program arcs as arcs, not as short straight lines?
This is the root of the problem, EMC2 is struggling to cut the millions of sharp corners that your CAM software is demanding.
G64PN is called "Naive Cam Detector", Perhaps it should be called "Stupid CAM Software Detection" to make it a bit clearer.

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 18:34 #10273 by kreature
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.
Attachments:

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 19:09 #10274 by andypugh
kreature wrote:

3D fuse-shapes for rc boat, subs, planes and the odd uav

Aren't splines traditional for boat building?
linuxcnc.org/docs/html/gcode_main.html#r1_7

Please Log in or Create an account to join the conversation.

More
02 Jun 2011 22:36 #10281 by kreature
I mostly get .stl files or other mesh files which are then translated into toolpaths for inner/outer or upper/lower etc.

Please Log in or Create an account to join the conversation.

More
03 Jun 2011 09:57 - 03 Jun 2011 10:15 #10283 by piasdom
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)

Last edit: 03 Jun 2011 10:15 by piasdom.

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.158 seconds
Powered by Kunena Forum