Drilling Delrin

[Slivers]

Hi All,

First post here, great forum, I've already learned things (and yes, I searched before posting this). Most of my experience is with hardwood, brass, aluminum, stainless, and titanium.

Here's my problem. I'm machining a part from natural white delrin, and it's my first time working with the stuff, nothing like the other materials. I need to drill a .625" hole about 3" deep through a 1" round rod. The bore has to be very smooth to accept a moving part with minimal friction.

What I'm getting is oversized, inconsistent, rough bores. I've varied the speed from less than 600 RPM to 3000 RPM (which should be correct at .008-.015 in/rev, right?). I'm using standard fluted IRWIN HSS drill bits, starting at 9/16", then increasing to 19/32" and finishing with a 5/8" reamer. I've also tried simply using a boring bar to finish the hole for the last 0.010 or so. All with the same, awful results.

Any suggestions?

[Eurisko]

Okay, I know very little about producing a nice finish on delrin.

I've worked with it. Drilling, tapping, milling, etc. The finish wasn't an issue. I probably used a shot of WD-40 just to keep it from squealing. Very easy to machine, taps well. Produces long, stringy chips.

Until a better response comes along, here's a link that might help...

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

Check out the troubleshooting section.

[djr76]

I make food processing equipment which in turn make 100's of different parts out of Delrin (Acetal). I would drill it one size under size and then use a bore bar with a .0156R tip insert and turn it to finish diameter .004-.005 per rev.. I never use any coolant or oils on Delrin, but I do blast air at the cutting edge to keep the chips inside the bore from welding.

[Geof]

Drill undersize using a brand new drill; possibly touch the cutting edges on a fine grinder so they have no top rake, like you would do for brass. Finish to size by boring and for best results in my experience use a HSS tool ground without any top rake but with a really sharp edge on a fine stone. I nearly always use coolant but you can get by quite well with just air.

[ALLtra Mach]

Take all those irwin drills and give them to a friend who isn't serious about machining. Then go buy some decent drills. If you get on MSC you can get a brand called Hertel, they are inexpensive and massively better tools than anything you get at A home improvement place.

As far as finish in delrin, Both answers are correct, very sharp tool, and coolant or air blast really unimportant, but you need something to keep chips/strings from welding.

[recordist]

If you don't need to have an exact .625 finish size, and can be allowed an extra few thousandths on the diameter -

Take a carbide insert and scrape ONE of the drill's flutes, right at the cutting edge, for the full length of the drill. I like to mark that flute with a marker, so I can return to the same flute to re-scrape later. This should be toward the OUTSIDE of the drill, actually raising a tiny burr...

This will give you a gorgeous finish - also will allow for a much straighter hole than possible otherwise.

LOTS of air and pecks, must get rid of the hot chips. Coolant may help, but it's not necessary.

[JohnnyTurn]

Forget about reaming plastic to a precision size. The hole will always shrink and you will be going in circles. A solid carbide boring bar could work for your aplication but you would need no more than a .005 Rad on the tip. You are also leaving too little of material for finishing. When you have to extend a BB out beyond 3:1 you must leave "something" for the BB to "bite" into.
.010 is not enough, it will chatter like crazy.

Try .025 to .030. Use coolant and a Spindle speed around 1000-2000 RPM with a feed of .003-.010. It depends if your making this part on a old beater or a newer machine. I would leave the finish boring as the last Op. when the rough thru hole is complete. Don't try to do this completely off the bar. You will get melt down.

JT

[gleas]

Lots of good ideas here but after 30 plus years of machining plastics, I have found that getting good finishes on bores sometimes requires a lot of trial and error. I would focus on the cutting point of your boring bar. Too sharp can also be a problem. We usually grind a sharp point, then just break the point with a diamond hone and try it, and repeat the honing until you get a good finish. There are no magic feed rates and rpm formulas for plastic. Sometimes fast works, sometimes slow. Keep the chips cleared or they will load up and burn the bore.

Hope this helps, -Greg

[John Welden]

I'd drill it and ream it. Should be no big deal. You may need an oversize reamer, the material pushes away and then comes back.

The thing you haven't mentioned is what kind of machine you're doing this on. What you're asking to do should be ridiculously easy unless you've got a sloppy machine and or set up. I'm guessing you're doing this on a lathe? The problems you're having sound like you've got a problem with your setup. Remember that rigidity is your #1 friend in the machine shop. All those little bits of slop can add up to a bad surface finish.