JUMPY CHOPPY MACHINING

[toolmaker101]

Hello all,
I have a 2017 M400 control #102978.

When I run a waveform toolpath the mill has to slow way down and it is a jumpy choppy path not smooth.
The control has look ahead but don't know about it my installer sead don't mess with that.
I am posting code made with Fusion 360.
I have attached a program and a report and a photo of the part I'm making. around line 300-500 is a place it jumps around.
Any help would be great!
Thank You in advance,
Travis

[tblough]

Trochoidal machining can be tough as there are lots of little moves entering and leaving the cut. If your accelerations are short, the tool paths can be jerky. You don't need to worry about look ahead, but you can look into toolpath smoothing. That will reduce the jerkiness but be aware that it can have a detrimental impact on cutter engagement as it smooths out the curves in the toolpath. In the line range you mentioned, most of the moves are only about 0.014" long so smoothing should help here.

I'm not sure where it is in F360, but somewhere in machine setup there should be a setting for maximum feed rate (or max rapid). Try reducing that and see if it helps. Normally the feed-ins/outs and actual cuts are done at the calculated feedrate for the material, but the clearance moves and fast moves back across are done at the max feedrate. Those transitions between the max feedrate and the cutting feedrate are what is causing the banging. You are jumping from 45ipm to 120ipm and back.

Here's a short video of trochoidal machining on some 1/2" thick 17-4PH stainless with somewhat smooth transitions:

[toolmaker101]

Thank you for your reply!

I will look in to the smoothing, F360 will let me adjust lead in and out non engagement feed and smoothing.
It seems as though Centroid is accelerating and decelerating at each line. I can see how longer lines will help.
I do not know why F360 dose not use arks instead of lines.
Thanks again and happy Machining
Travis

[cnckeith]

in addition to the cad/cam settings.

try one of the default smoothing profiles in CNC12 smoothing menu. "contouring mill" will round off sharp corners and turn arounds therefore smoothing sharp short jerky g code.

[converterking]

In your cam settings, increase the min radius to a large amount like .250. See if that makes a difference.

[ashesman]

Watch the feedrate number. If it is jumping around a lot then you have sudden acceleration/deceleration.

I am having similar issues too in this post viewtopic.php?f=64&t=6181&p=53693#p53693.