Mill cutting Delrin Speeds and Feeds anyone?

[jgaertner]

Hello Forum,

I am trying to mill a 0.0940" deep pocket/hole by 0.400 diameter in a rod of Delrin using a 4 flute rounded corner end mill that is 1.125" long, cutting area. (I could not find a rounded corner 3 flute end easily for this job.

I used a BORE command and had it spiral into the hole thinking this would be best to allow the removed material to exit the bored hole as it was being made.

I used G-wizard to start with on my feeds and speeds but it was WAY to fast and the Delrin really heated up and became a big mess.

Anyone have any experience milling Delrin?

Thanks,

jgaertner    

[LibertyMachine]

Low surface footage, high(er) feed.

Using carbide tooling , around 150-175 sfm and a chipload of....maybe .004 per tooth. You want to run coolant, if possible.

So, a .375 endmill, 4 flute, would be runing around 1700 rpm and feeding around 27 ipm. You could actually go up to the low-mid 30's, assuming your workholding is secure.

Keep in mind, that would be a linear feed. If you are trying to use a BORE cycle for an internal pocket and there is only a small machine 

motion going on, your machine may not be too thrilled at that rapid feedrate over such a small distance. Proceed accordingly

[LibertyMachine]

It can be a headscratcher, working in plastics. You are inclined to think that you can go as fast as you want, due to it's softness. And while there does exist tooling that will allow you to fly in certain plastics, general metal cutting tooling isn't often designed with the geometries needed for efficient plastic machining.

It's been my experience that a nice sharp HSS (high speed steel) uncoated endmill can often out-perform carbide in plastics such as Delrin (acetal) UHMW, Teflon

Edit:

And for workholding, that's another fun one. Since the material is slippery, you often need to hold onto a lot more than you would with metals. In working with metal, I've got almost no issue holding onto .050" of stock and roughing away (using serrated jaws and whatnot). If I'm holding onto less than .150" in plastic, chances are I've got a part coming out of the vise. Plastic is cheap (enough) and easy to remove excess material

[jgaertner]

OK, Thanks for the help. I will give it another try. I am using a C5 collect to hold the .75" diameter piece of Delrin, but I think it is slipping, if that is possible? I will work on that issue to.

Jgaertner

[friesendrywall]

Ditch 4 flutes as fast as you can, and get something like an onsrud single flute 65-000 series or similar.  It will be tough though if you have to have it rounded though.

Single flute cutters are so superior in plastic.  I think the recommended onsrud chipload for a 3/8 bit is around .010.  You can run it fast too.

[LibertyMachine]

While I don't disagree with you at all, as Onsrud cutters are quite nice indeed, if you are putting around and just have a handful of parts, or perhaps you are on a shoe-string budget, 4 flute HSS will work just fine. Is the Onsrud superior? Absolutely. Is it the only thing that will work, no.

All depends on what your end-goals are. Mass quantity parts at the lowest cost possible, Onsrud. Handful of parts for yourself or on a "cost plus" job? Use what ya got

[friesendrywall]

Yes, I would probably do the same.  Having tried both though..

I'd like to know what the original feed and speed was to melt the plastic.  Sometimes melting happens from too low a chipload.  I assume you used coolant?

One problem is that 4 flutes can hardly clear the chips good enough in plastic.

[jgaertner · Accepted solution]

OK, so I solved my feeds and speeds issues. I do not seem to understand how setting speeds and feeds in the Fusion Parameters makes any difference? They just change on you, so I did everything at my CNC mill. I ran the RPMs at 1200, and the feed at 48%, Velocity at 39% Feed rate was 12.4 ft per minute and this all worked fine.

I have a good solution to the stingy cuttings that come off the mill and wrap around it. I use my shop vac to pull them off the tool from the very start of the cut! It works a TREAT! No coolant and everything is as smooth as silk.

Also to note: When using a bull nose mill, the depth of cut does not seem to be the bottom of the mill? I ran the part 2 times and it was always off by 0.030"! Then I realized that was the end mill radius edges. I could not select the bottom of the feature no matter what I did so I added the 0.030 to the Bottom Depth Offset.

Now, if I could only solve why the mill will not cut my four  0.020 radius edges on the parts?

Jgaertner

[LibertyMachine]

Yeah, sometimes working with a bull nose tool can be a pain, especially when you don't have a solid procedure how to selct the features and define depths.

If you don't mind sharing your file, I'd be happy to take alook at it this evening, amke a few edits and kick it back to you so you can see what I did

[Steinwerks]

Your bottom issue doesn't seem correct, so share the part if you can.

An air blast is what we generally use for cutting Delrin, coolant if a perfect finish is really needed, but air does well. I've defaulted to coolant for UHMW as the finish is generally that much better. The key in plastics is to avoid chipping (like acetal has a tendency on sharp corners) and feed it hard enough (.003/flute easy). A .01" finish bare minimum, I run a .02-.03" finish for profile milling and .05" for face milling. We made a couple parts in Delrin earlier today running a 1/2" end mill at 6k (roughly 800SFM) and they turned out beautiful.

[kb9ydn]

---

@jgaertner wrote:

OK, so I solved my feeds and speeds issues. I do not seem to understand how setting speeds and feeds in the Fusion Parameters makes any difference? They just change on you, so I did everything at my CNC mill. I ran the RPMs at 1200, and the feed at 48%, Velocity at 39% Feed rate was 12.4 ft per minute and this all worked fine.

---

That doesn't make any sense.  The feeds and speeds you put in for an operation should show up in the program.  One thing to be aware of though is that if you reselect a tool (a different one or even the same one) in an operation, the feeds and speeds will reset to the default for the selected tool.  For this reason I always input feeds and speeds last after I've gotten all the other parameters set.

---

@jgaertner wrote:

I have a good solution to the stingy cuttings that come off the mill and wrap around it. I use my shop vac to pull them off the tool from the very start of the cut! It works a TREAT! No coolant and everything is as smooth as silk.

Also to note: When using a bull nose mill, the depth of cut does not seem to be the bottom of the mill? I ran the part 2 times and it was always off by 0.030"! Then I realized that was the end mill radius edges. I could not select the bottom of the feature no matter what I did so I added the 0.030 to the Bottom Depth Offset.

Now, if I could only solve why the mill will not cut my four  0.020 radius edges on the parts?

Jgaertner

---

I almost always cut plastics dry if possible and use an air blast to blow the chips away.  It's so much less messy and usually the air is enough to keep everything cool.

The bore operation will not recognize radiused corners at the top or bottom of a bore, so if you have those (and it looks like you do at the bottom) they will not be included.  To cut all the way to the bottom you need to override the bottom height in the heights tab, either with a manual offset, or by setting the bottom height to "selection" and then selecting the actual bottom of the bore.  The same thing goes for the top of the hole as well.  And radius or chamfer on the top of the hole will not be recognized.

C|