Machine is rounding of square internal corners

More
03 Mar 2021 10:32 #200881 by BastianMC
Hi, im struggeling with a strange issue here.
My machine is rounding of internal corners that should be square with a tool diameter as corner radius only.

I initialy thought the machine was struggeling to get my velocity of 3000mm/min in the corners causing this issue but even when lowering the feed override to 50% 1500mm/min the corners are stil not square?

What is causing this issue? Please see attached pictures.
Attachments:

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

More
03 Mar 2021 10:54 #200884 by BastianMC
Sorry to take your time guys, this post fixed my issues.
Apparently it was a Fusion 360 problem and not a linux CNC

forums.autodesk.com/t5/fusion-360-manufa...-fillet/td-p/7689373

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

More
03 Mar 2021 14:48 #200905 by andypugh
No, it is definitely a LinuxCNC problem, that Fusion thread is just how to fix it for a particular postprocessor.

If you have this issue then what it really means is that you have configured a machine to move very fast but with disproportionately low axis acceleration.

If you configure the PP as suggested then your part geometry will be corrected, but the machine will slow more that it needs to in the corners.

When you say that a machine can move at X m/s but can only accelerate at Y m/s2 (or imperial equivalent) then you are actually defining a minimum turn radius that the machine is capable of following.
Without instructions to the contrary (ie a G64 command) then LinuxCNC will run at the programmed feed speed, and modify the corners according to your stated acceleration limit.

What I would recommend you do is increase the acceleration limits in your INI file to something that is actually experimentally validated rather than guessed at.
The following user(s) said Thank You: akb1212, BastianMC

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

More
03 Mar 2021 17:12 #200913 by BastianMC
How do i determine my acceleration values?

I have now 100 velocity and 750 acceleration for x and y axis?
The acceleration is as it was when the machine was configured but i change my speed.

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

More
03 Mar 2021 22:01 #200947 by Todd Zuercher
To figure it out experimentally, for a stepper machine increase the acceleration until the motor stalls, then reduce by a safety margin. I'd say at least 30% but depending on the machine 60% might be more appropriate. The test will need to be done at or near the max velocity, because that is where a stepper is weakest.

On a servo with feed back, it is simpler, set the f-error high for testing and the acceleration to something way too high. Do a test move watching the velocity feedback in halscope. The slope of that will be the max possible acceleration. Set the max acceleration to something less, perhaps 10%-20% less.

It might be wise to load up the moving joint with the max theoretical load for testing. (put something heavy on the table, load up your biggest tools...) and make sure the machine is bolted down good, this could be quite violent if the machine is powerful. (read this as it may not be safe.) Fortunately on a servo the speed doesn't need to be high or the move large to find the limit. so make the moves small and not particularly fast, just enough to see linear acceleration.

More importantly learn how to use G64 Pn in you g-code to get the path following tolerance you need.
The following user(s) said Thank You: akb1212

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

More
04 Mar 2021 02:10 #200980 by Michael
A G61 would make linuxcnc follow the exact g code that fusion is spitting out but you will slow in the corners to change directions. You can play with a mixture of G61 and G64 P .xxx values to see what you prefer.

linuxcnc.org/docs/2.8/html/gcode/g-code.html#gcode:g61

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

More
04 Mar 2021 07:53 #200997 by robertspark
what about using constant velocity g64 for roughing cuts and a finishing cut using G61 exact stop mode.

(as posted above)

careful of chip thinning / rubbing as it will blunt you tool / shorten it's cutting life.

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

Time to create page: 0.117 seconds
Powered by Kunena Forum