Just got my Nomad, I have a ton of HDPE laying around from some molds I made. So I figured I’d use it to test some models before diving into nice hard woods. But ive run into some issues.
I used the HDPE setting in meshcam’s carbide auto tool path. For the roughting pass Im using the .125" ball. Everything cuts quickly, quietly and smoothly. Switching to the .063 for the clean up is were the trouble starts. At about 40% it just seems to suddenly drive the bit into the plastic causing it to snap. I lowered the plunge and sped up the bit, and lowered the steps and again it just snaps it. 2 out of 3 cutters are broke, now. Just wondering what others have had luck with. The chips looked good and it seemed to be going so well then just errrrrrrrr snap… =/
Congratulations on your Nomad 883 Pro!
I’m running a Starboard (modified HDPE) project right now.
Please post a window snapshot of the MeshCAM cutting parameters for you job. Also tell us the RPM that each tool is running with. Could you also please post the STL of your job?
Sudden plunges could be caused by a software problem, a hardware problem, or a parameter setting problem. As a new machine, we’ll start by assuming its OK and look at the software and parameters.
I just ran with the default for the HDPE settings in carbide which i believes has the RPM at 7500. I’ve attached the settings, on the second attempt I dropped feed rate to mid/lower 60’s and the plung rate to 16’s.
I don’t think its a hardware issue as I’ve cute the renshape it came with and another piece of renshape with no real issues.
I’ve attached the stl, its one side of a gun grip for a client. I wanted to cut it in the HDPE to make sure all the wholes and groves fit correctly before using wood.
Gun Grip Test.stl (2.4 MB
I need to think about this a bit but my immediate reaction is that is way too fast for an end mill that small.
I’ve roughed HDPE at 75 IPM and it’s a but noisy but OK. I usually work around 50-60 IPM.
@rev66, I will guess that you are using supports since this is a double-sided piece. In that case, depending on the roughing stepdown vs. the support thickness, the supports might not be roughed out to their outer end. In that case, the parallel finishing might plunge into the material in an un-roughed area. Check the discussion http://grzforum.com/viewtopic.php?f=3&t=15619 for a situation of that type.
You could turn off the finishing and look at the toolpath simulation, and then look for where the finishing toolpath starts. You’d be safer also if you recaculated the finishing toolpaths with a machining margin of maybe .035 (i.e. just over the radius of your finishing cutter).
Plus what Mark said…
I’m new too. I encountered this same problem last night with some wood using an very small bit (1mm).
I learned that it’s caused by the waterline pass. I did some digging and found that if I change the Toolpath Order from “Depth First” to “By Layer” (or something like that I don’t have the software in front of me). This causes the waterline to do an entire layer first, and then move to the next layer and so forth. Rather than sometimes (why I don’t know) plunging and trying to move.
My next pass with By Layer made everything work perfectly, but was a little slower. Try that and see if it solves your problem.
It would be good to hear from an expert why it plunges so deep sometimes on waterline. In my case, I assumed it was because I was skipping a roughing path (which had already been done).
@randy I did notice that the first time it had snapped it was by the support. So I have a feeling that’s the cause. When I get home late tonight I’ll try again. Dropping to speed and widing that setting as per your recommendation.
I’ll keep you posted. Thanks guys!
I did notice that the first time it had snapped it was by the support. So I have a feeling that’s the cause
Learning to avoid collisions comes with the territory. Do take some time and examine your machine, stock and fixtures. I use a 'ole standby - a Starrett solid Al 6 inch ruler - to triple check that nothing will collide.
Just as I suspected, the finishing rate for an 0.063" end mill is considerably too high. I would rough@40IPM and plunge@10IPM.