Looking to see if anyone has a “best practice” on removing a decent amount of material quicker than the standard (using Carbide Create). What I was thinking… was that I could create 2 different paths. 1 - increased feed rate and depth of cut (but leave room on the bottom and sides), 2 - final pass using the “standard” feed and speed. For number 2, it seems that I could also go deeper than the standard to still get a good finished edge?
If it helps, I am working with HDPE.
I have read a little on Adaptive Toolpaths, and I think I generally understand, but it looks like I will need to switch to Fusion 360 (or similar). For now, I am ok with everything not being completely optimized, but would like to speed things up a bit.
you can do semi adaptive with CC and a post processing step
right now you likely set your feedrate to the worst case of the whole toolpath… .this kind of processing changes that so there is no worst case (the worst case is usually 2x the normal case)…
What kind of endmills and feeds and speeds are you using currently? In HDPE one can feed surprisingly fast and get away with it.
What you describe is pretty much the “roughing+finishing” approach and it’s the way to go (when you care about finish quality/dimensions).
For pockets in wood or HDPE, I often rough the pocket leaving no stock at the bottom (=cutting down to target pocket depth, because the surface finish at the bottom is often more influenced by the quality of the tramming than by the feeds and speeds, in wood at least). Then I run a finishing toolpath that consists in a single contour pass at full depth (minus a hair, to not touch the bottom of the pocket while going around), it will go along the walls once and shave off the remaining material, using the full endmill length of cut, leaving very few tool marks. Using a downcut endmill for that finishing pass also ensures very clean top edges / no tearout.
Adaptive clearing is indeed another way to reduce the number of passes by cutting (much, much) deeper, but at a much lower stepover. Sometimes the material removal rate benefits from going to adaptive, sometimes it doesn’t.
I am using the 1/4 or endmill from Carbide and accepting their defaults when selecting a tool in CC. This sounds like a good step for me (and I do care about the finished edges). I have also read that an O flute can create a better finish with HDPE.
CC’s defaults are somewhat conservative (for good reasons, they need to be a safe place to start for everyone), you can push them further especially in HDPE (a.k.a “butter”, from the machine’s perspective)
Experimentation is key as usual, you could for example use CM’s feedrate override during your cut to incrementally bump up your feedrate (it’s a safe way to experiment, because you can dynamically lower/reset the feedrate very quickly if things start to go bad).
I see that CC defaults to 0.05" per pass for a #201 in HDPE, for a 1/4" you can go deeper (experiment again)
BUT, I have found that chip evacuation is paramout when cutting plastics, which is where O-flutes shine (that, and their specific geometry and sharp/acute flutes optimized for cutting plastics). Amana’s 51404 is possibly my preferred cutter. If you cut a lot of plastics, getting one (and using it ONLY to cut plastics) won’t disappoint.
Regarding finish quality versus tool geometry, I’ll let others comment as this is not something I have been overly concerned about when cutting HDPE, but my understanding is that O-flutes shine there too.
For HDPE I use a Single Flute. For slotting I use a minimum feed per tooth of .004". My router lives at 18Krpm. This is 72in/min. I use corner compensation to help alleviate the substantial deflections in corners. I have a stock Shapeoko XXL, the endmill is a noddle, particularly in the Y axis. I feed override from here. I typically US manufactured uncoated cutters specifically engineered for hard and soft plastics. These are notably superior to the C3D coated single flutes when used with plastics.
As for adaptive vs pocketing, I generally pick the faster option. Creating addional geometry to utilize adaptive paths on HDPE is normally enjoyable to watch, but generally a waste of machining time. Standard pocket or slotting operations pushed aggressively, followed by lighter finishing passes work just fine. This is where I find the greatest difficulty with my Shapeoko on all plastic projects. Finding the right balance between cutter engagement and deflection. Most plastic cutters have some rubbing baked into the recipe, too little engagement, the machine deflects and the plastic heals. You’ll have to experiment.
For reference purposes, my supplier cuts around 250ipm at 18-20K. Full WOC. DOC=Cutter Diameter. They use a stock to leave of appox. .015". This is using standard size cutters, say .25" and larger. I believe they typically run a .375" single flute.
I had a chance today to cut some parts and pushed the DOC to .125 and it went pretty fast. I set the paths up to leave .01 and do a full depth finishing pass. Came out pretty well, but not as good as I would like. I didn’t mess with the default router speed of 10k (suggested by CC). I will probably buy an O flute to see i that helps and try pushing the rpm. I learned the hard way that clamping down is even more important when you increase the DOC on an upcup bit
I run full depth finishing passes at 0,0. Often called a spring pass. But rarely do I bother with them as often suggested for finishing stock removable on the Shapeoko working with plastics. You get into the hard balance territory. For what I do, which is attempting professional results with a hobby machine, I prefer to take a higher resolution doc, evenly spacing the passes. It is uniform and passes with little fuss. I have largely given up trying for a router finish on acrylic, and I have now opted to do my best and sand the rest. HDPE does not present that option, and so this is where I have arrived.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.