Does anyone have recommendations for carving Delrin or Acetal Plastic (not on the standard material list)? I’m a newbie and this is the first material I’m carving on the X-Carve - but getting terrible results. I’ve slowed the feed down to 10 IPM, .005" DOC using a 2 flute spiral upcut bit (1/8" dia). Just trying to carve out shallow (.020" - .040" deep) simple shapes into a flat surface to make a tool with multiple cavities. Need clean, uniform cavities with very consistent depth of cut. Recommendations please ??
I have cut quite a bit of it, one of my favorite materials. I have been mostly cutting with a 1/16 fishtail upcut about 45ips and .03125 depth per pass. Be sure you have good ventilation and have fun!
Thanks David. I’ve tried a few different bits, including an 1/8" Fishtail spiral upcut. I started with the ABS matl selection (40 ips, .05" DOC) but got very rough cuts as well as lots of curls of matl on the bit and around the holes. It took a lot of cleaning to get rid of the mess and was still very rough. I slowed down the feed to 10 ips, and .010" DOC and got slightly better results, but still very rough and messy.
Acetal cuts like butter, unless its a poor bit, poor feedrate/rpm combination.
Using a 1/8" 2F tool I´d try 60IPM at Dewalt minimum RPM (16k)
As Easel allow you to play with feed override during carving I´d simply try 60 and increase/decrease feed and see if a sweetspot could be dialed in. As you are carving shallow you have a larger envelope to explore in terms of feed rate vs machine rigidity.
Speed up. If your passes are that shallow, go much faster. You’re rubbing the material away and melting plastic. Even at 60 inch/min, you’re pretty conservative for the material.
Agreed, I think he is cutting too slow, a hard lesson learned about cutting, you think slowing down is the right thing to do when you are not getting the cuts you want but in fact, it can and usually is the opposite. I found this out the hard way when I first started trying to cut MDF. I was literally eating bits every few minutes and my board was burning. Once I figured out that I was rubbing the board instead of cutting the board because I was going to slow I was able use the same bit with perfect cuts for several thousand linear inches.
Use Delran it wont melt, I cant find the project I used it on, but it cuts and chips easy. Runs very well and no smell, perfect cuts. I used the Inventables 1/8" 2 flute straight bit on it.
So you are saying that I’m cutting TOO SLOWLY? That seems counter intuitive, but hey I’m willing to give it a try. Thanks for the tips.
PS - I am pleasantly surprised by how helpful everyone here is. THANKS!
Well as Tom Cruise learns in Days of Thunder “Rubbing is racing!” but it’s not milling. You want to push through fast enough that the flutes have to carve a chip off, too slowly and it keeps rubbing on the surface after taking that chip out. There is obviously a balance of pushing too quickly and the tool snaps or gouges into the material faster than it can clear a chip away.
in milling: Rubbing is friction, which is heat, which is melty-plastic…
Assuming you’re running at the Dewalt min RPM of 16k,
Chipload = FeedRate / flutes * rpm = 10 / 2 * 16000 = 10 / 32000 = .0003
If it were me, I’d start at AT LEAST a chipload of .001 if I didn’t know anything else.
Since I know you’re cutting a soft-ish plastic, I’d go for .004 ish. On a machine i don’t know (your X-Carve), I’d say you should easily be able to handle .002 (64ipm) and go up from there.
I have cut a lot of plastic - Lexan, Acetal, Acrylic, ABS, PVC and Delrin. I personally like using a single flute up-cut for plastic. I find it more forgiving and easier to use than multi-flute mills. Single flute mills remove chips better than multi-flute, which is important if you are making deep cuts without clearing passes - which is what easel does. Also, you can run at half the speed of a two flute. I like to use a 3/16" SF is I can get away with the larger size. You can push through the material faster and it clears chips better than an 1/8" SF.