What's new
What's new

Milling Delrin? Speeds, feeds, coolant?

Edster

Diamond
Joined
Feb 8, 2003
Location
Illinois
I have a bunch of delrin jobs coming up. Just wondering what you guys use for speeds, feeds, and coolant? I plan to use endmills designed for aluminum, and standard drills and taps.

I'm programming the first job now. I'm using 1/2" and 1/4" SGS S-carb endmills. I've heard use high rpms with coolant and I've heard use low rpms without coolant. I've also heard large step over with a high feed.

If I could cut dry it would make cleanup a whole lot easier. Not sure how well drilling will work without coolant though. I've got a couple 6-32 tapped holes and a 1/16 hole. I'm envisioning lots of chips wrapping on the drills and tap.

Any advice appreciated! :cheers:
 
the way I cut DELRIN is slower than others suggest and books suggest....these setting are for dry but mostly i run with TRIM-SOL....wont hurt a thing....i also tap with trim-sol either flooded with machine or just a spray bottle....I run about 400 Rpms with a 2 flute cutter and aboot 10.0 inches per minute....if its 4 flute then I run maybe 250 Rpms and same feed...for roughing maybe .02 feed...finishing maybe 7.0....sometimes 12.0....if I run it wet I leave it roughly the same....why do this...because slower produces nice clean chips and no burr and no melting with great finishes...fast produces melting and huge burrs...as always I tell people to try slow speeds that I say....then fast like books of today say.....10 times better product slower as you will see for yourself...and then to deburr really nice....I rub with razor blade and or emery paper....lightly....oh ya....I tap it with machine all the way through at 100 RPMs...chip just spirals out or down thru hole...threads really sweet....if blind or small hole I tap by hand but maybe start with machine going .300 deep or so to start threads....my 2c

PS...drilling I go slow also....maybe a 1/2 drill at 400 or 300 also with heavy feed but a .100 peck....fast will bunch up like you said and extreme speed ball of chips on drill will mess up top surface of job by melting into it...peck
 
Uhhh, no. Delrin is by far the easiest plastic to machine hands down. Chips come off fragmented like cutting wood or brass. Run coolant.

UHMW on the other hand...:ack2:

Delrin can wrap up on a drill, or get stuck in ER collet slots, so you might program a chip break if available. Coolant or air blast can help clear them.

Regards.

Mike
 
I almost forgot but FINEGRAIN reminded me...when running dry....I hold the air gun open and aim at the cutter for entire operation thus ejecting chips with no ball up or melting
 
I have had the best luck with a higher spindle while milling with a light chip load for thin chips with A LOT of air blast. Looks like it snowed but it's easy to clean up. Drilling I sped up a little but not much to make sure the chips don't ball up on the tool.
 
IME this is a good guide

http://www.boedeker.com/fabtip.htm


That said -

Milling, when roughing and the job will take it, push the feed right up - 0.015'' Per tooth is not that high!

Turning 0.015 - 0.020'' / rev again is not that high!

IME Dubbed drill points -as you would for brass - help break up the swarf.

Oh yes - if a cutter's been used for anything other than plastic, DON'T use it.
 
To start with, do you know how to read? I mean do you know how to do a little research on your own. Or do you think we are your only ability to find your answers. At lease you might open a book about machining! Then you can, I guess read it. Think, in stead, how wonderful it is to find lots of answers for you right in the same book. The material people actually have information for you if you ask. I guess they still call them libraries. Might want take a trip if you're that interested, if not change occupations.





Drill like steel rpm with chip load of 3% of drill diameter. Peck if needed. The material is self lubricated.

Climb when milling.

Take it easy on it. It's only plastic.

Stanley Dornfeld.
 
Also, be careful when breaking out on thin sections. Tends to fracture. Make sure you have a good hold in a vise, if milling. Trying to only grip on .12 or something, it kind of squirts out like a watermelon seed.
 
To start with, do you know how to read? I mean do you know how to do a little research on your own. Or do you think we are your only ability to find your answers. At lease you might open a book about machining! Then you can, I guess read it. Think, in stead, how wonderful it is to find lots of answers for you right in the same book. The material people actually have information for you if you ask. I guess they still call them libraries. Might want take a trip if you're that interested, if not change occupations.

Uh... yeah... I know how to read. Do you know how to not be a jackass? Might want to do some research in the self help section of the library yourself. :rolleyes5:
 
1200 surface feet and don't look back using coolant on turning operations. Milling, how much spindle speed you got? Don't be a jackass about your milling cycles and let it rip. 50% step over at a minimum with high feed and coolant. Seriously, don't be scared Delrin has got to be the easiest to machine plastic across the board.
 
Turning has been smooth for me, milling the thing to watch for is how tight to tighten the vice..it is slippery stuff.
Use coolant if for nothing else nest removal.
Gary
 
If you're holding on to 1/4" of material I haven't found pulling the part out to be much of an issue. Delrin isn't as slippery as UHMW.

As stated before, sharp corners can chip out, but otherwise milling the stuff is like taking candy from babies. I'll use coolant if I want something to look really nice, but as with most plastics it'll swell when wet. Depending on tool size I leave .01-.02" for a finish pass, drill at 2.5% off drill diameter for feed and fairly slow at 120SFM, with an air blast. Also like many plastics, it drills small, so if you have a hole that HAS to be .250", ream it with a .251" or .252" with coolant.

12041760334_4d8a4f27f2_c.jpg
 
At lease you might open a book about machining!

Every book I've ever seen about machining is generally out-of-touch with modern metal-cutting, and written by some schmuck professor working in a lab somewhere it seems like.

And any "new" books on machining are going to be so rare and specialized they're certainly not going to be found in the library.

That's why PM is so great, it's up-to-date, factual, hands-on, hard-won advice from real machinists and shop owners out in the trenches getting it done every day.

ToolCat
 
To start with, do you know how to read? I mean do you know how to do a little research on your own. Or do you think we are your only ability to find your answers. At lease you might open a book about machining! Then you can, I guess read it. Think, in stead, how wonderful it is to find lots of answers for you right in the same book. The material people actually have information for you if you ask. I guess they still call them libraries. Might want take a trip if you're that interested, if not change occupations.

WTF ????? Lighten up man.
 








 
Back
Top