Machining Delrin

I have a job coming up where I have to turn & mill some Delrin. Any suggestions on type of carbide endmills, coolant or dry machining? Any help would be appreciated.

Thanks

I just hope you don't have to hold those 0.0005" tolerances mentioned elsewhere in these forums. Delrin machines like butter. It's hard to do anything wrong with this stuff. I use the same drills, HSS end mills and carbide cutters that I would use for steel and they all work great.
I haven't bothered with coolant and have had no problems so far,but it might help to keep temperatures under control if you are faced with tight tolerances.

Oh, one last thing: I found that Delrin sort of "collapses" around the finished thread when tapping so you might increase the hole size slightly if you're doing that operation.

I just cranked out some good size delrin parts that took sveral cubic feet of facing and what not. I'll say if you're gonna do that dry, hold your breath: It seems to be toxic, which is why I used coolant just so I wouldn't get light headed...

I agree with running the coolant for the fumes. I have heard that it releases the formaldahyde. You can run speeds and feeds faster than you would for aluminum. I generally use 2 flute carbide endmills. To get the coolant off wash in hot soapy water.

Michael

I'm just a hobby buy, but I will add that it deburrs nicely. Unlike many plastics, it files well, and sands easily. Sharp corners are easily de-burred with some medium steel wool, and any minor tool marks easily clean up with some extra fine steel wool.

Sharp, real sharp, tooling seems to be the key with Delrin along with efficient swarf removal so you don't get double cutting. May be a static electricity effect but sometimes, for no logically apparent reason, the swarf will fold back round the tool to be cut a second time. Apart from the jam up risk this considerably pushes up the heat fed into the tool.

The key to the collapse on a thread and other self re-shaping problems seems to be in keeping the actual cut as cool as possible hence the sharp tooling requirement. Shove a small, OK on steel but not super sharp, tap into the stuff and it can close up so much that its hard to get the tap out. When it does come out its surprisingly warm. I got over ambitious once with a "not very old" 6 mm slot drill working dry. Snapped the cutter and found the business end to be blue on extraction whilst the shaft in the cutter holder was hotter than I cared to touch.

Clive

I don’t machine Delrin very often, but I injection mold the stuff. A couple pertinent observations:

Delrin is polymerized formaldehyde. If you get it hot enough, it will break down and release formaldehyde gas. Very irritating to the eyes and nose.

I don’t know if you can get Delrin hot enough from machining operations to have it catch fire, but be aware that it burns with an invisible flame. If you see a piece that is foaming like a wet Alka-Seltzer, it is actually burning. It will eventually be entirely consumed, leaving only a little white powder residue. We see this effect when we clean mold components with a propane torch.

Delrin has a very low rate of water absorption, and is resistant to most oils, so coolant shouldn’t hurt anything, and would help with the gas and fire issues if doing very aggressive machining. That being said, the few times I’ve had to machine it, I’ve done it dry with no problems, but I wasn’t doing production.

Delrin, like most plastics has a much greater coefficient of thermal expansion than steel, so temperature must be closely maintained if tight tolerances need to be held. Also, Delrin is a crystalline material, and if not fully polymerized, heat can cause additional molecular cross linking, which will result in shrinkage. This shouldn’t be a problem with stock sold for machining applications, but could come back to bite you if doing secondary machining on injection molded components. The standard way to check for potential post molding shrinkage is to place the part in an oven at about 200*F for an hour, or an hour per inch of cross section after the material has come up to temperature, allow to cool, and recheck the dimensions. If it’s smaller, the original stock wasn’t fully cross linked. This same oven schedule can be used to normalize stock before machining if need be.

[FONT=&quot]Dennis[/FONT]

If your using carbide DON"T use the circular margin tools! I use the regular old up sharp carbide tools with good results.

If the whole world was made out of delrin it would be a better place.

I discovered that hot PVC attacks acetal (Delrin) like mad. I had a couple of pump motors with a PVC sleeves around the stators mounted inside acetal housings. The motors overheated, and when I opened up the housings, it looked like bark beetles had gotten after the acetal. All that was left was the white powdery filler.

Use Gh5 Taps To Get A Proper Thread Size.

Cutting delirn/acetal plastic, use sharp colbalt or carbide, 3flutes work the best with a high helix. remember to buy the material at least .200 thicker than you need for thin parts and take equal amounts off of both sides to keep it from warping, use the soft center meet.

as for speeds and feeds i run a haas VF2SS and cut all my plastics at 1200rpm, 100 to 400 ipm for .125 to 1" cutters, anything smaller i slow the feed only.

i'm a model maker and cut cut foam to titanium and hold all the pastic to a acrylic sub plate with double stick tape, and hot glue around the edge if its a bigger part. all you have to do to release it is squirt denatured alchol around the edges and let it seep in and it will pop right off. also use the cool air gun right on the haas, uses an m-code to turn it on, don't use coolant, as long as you take a fast feed for roughing and leave material for a finish on the floors of about .015 to .02" it will look like a babies bottom.

the double stick i use is permacel PO2 about $10 to $12 per 1" x 60 yards, if you need 2" double the price. if 1/2" divid by 2.

lenny

When I run Acetal/Delrin on the lathe, I have gone to using HSS inserts from AR Warner. Great surface finish. I have not noticed fumes from my turning experience, but Im also not hogging it off. I cant say much for milling, because I have only done a tiny bit, but just used HSS endmills.

From what I have learned, the keener edge you can get from HSS that you (supposedly - I have no way to know for fact - just know what I read) cant get with a Carbide edge really helps with the surface finish. Then again, I dont know how important that is in your op. For mine, apearance is 90% of it, so I focus on the best surface finish I can get.

I proof my parts dry so I can see and not get covered... but then I go to coolant, and actually aim the nozzel from under the tool (pointing from the bottom of the holder to the cutting surface - in my case, tool is cutting edge facing down, so the nozzle is on top pointing down) The way delrin/acetal wants to string, by running the coolant that way, the coolant carries the whole string into the chip pan so it doesnt wrap around the part.

I dont know what kind of tool life one would/should expect comparing carbide to hss... or if its much of a factor. But I did see a huge increase in surface finish going from carbide to HSS inserts.

Wade

yes on a lathe , you would use HSS because of the sharp edge you have, carbide doesn't have that. in mill you use ground solid endmills that have sharp edges not inserted endmills like on the lathe.

and i also have neve gotten fumes, unless i was burning the plastic from a dull cutter.

I would cool it with air. And the main purpose of the air is to get the chips away. Plastics will normally not overheat unless you fail to get rid of the chips.

Delrin will melt before it releases formaldehyde, so there is nothing to worry about if you cut it properly.

Len is right. For fine finishes and close tolerances, use HSS or cobalt. New cutters work best unless your regrinds are well done.

We do both milling and turning of acetal using the polished carbide inserts for aluminum cutting. They have a very keen ground edge and last forever in plastic.

Curtis