Subject: Re: Anyone machined Teflon?

From: [email-masked] (michael jensen)
Date: 5 Jun 1996 13:04:56 GMT

Boris Beizer ([email-masked]) wrote:

: >Has anyone had any experience machining Teflon?

: Indeed,
: >
: >If so, how does it cut?  

: Lovely.  Use really flat tools with extreme bottom rake angles.  About 15 Degrees
: top rake and about a 30 degree angle on the bottom (e.g., 60 bottom rake). Almost
: like a woodworking bit.  Really fine polish.  Use a fine grindstone, very fine, 
: then hand hone with India and/or black arkansas stone.  Lapped mirror finish is
: best.    

: >would also like to know recommended feeds
: >and speeds for turning a small teflon part on a CNC lathe.

: Almost doesn't matter.  It is self-lubricating and will cut at almost any feed
: and speed you want.  The trouble is getting precision.  At high speeds, you get
: wobblies on the surface.  It is very soft, distorts easily, and bounces back.
: You have to take that into account.  Sort of trying to get precision machining in
: American Cheese.   

     I agree, you want to radius the front edge of the cutting tool.  I have
found that HSS works better then carbide cutting tools.  The previous post
about lapped mirror finish is exactly right, the smoother you get your reliefs
the less distortion you will have in your finished parts.  Machine it 
at speed similar to aluminum or faster if your lathe can handle it.  
Do not smoke when machining telfon.  Burning telfons contain florines,
very bad for you.  The main key to machining telfon, very sharp 
cutting tools with a radius at the tip.

Best of luck

Mike J.

: >
: >Any replies by e-mail would be much appreciated.  Thanks.
: Boris Beizer

: -----------------------------------------------------------------------------------------------------
: Dr. Boris Beizer                                  Seminars and Consulting on
: 1232  Glenbrook Road                       Software Testing & QA
: Huntingdon Valley, PA 19006 USA
: TEL:     215-572-5580     FAX:  215-886-0144     Email:  [email-masked]

: Note:  After July 1, 1996, [email-masked] will not be active.
: Please update your directories and use the above address
: ([email-masked]) in the future.   Thank You.
: -----------------------------------------------------------------------------------------------------

--
Mike Jensen ([email-masked]) 
Chemistry Instrument Shop              
University of Nebraska - Lincoln
(402) 472-3542

---

From: [email-masked] (Boris Beizer)
Date: Wed, 05 Jun 1996 10:40:45

In article <[email-masked]> michael jensen wrote:

>     I agree, you want to radius the front edge of the cutting tool.  

Oh yes, I forgot to mention that.  

>I have found that HSS works better then carbide cutting tools.

I concur.  Forgot to mention that also.  Carbides need high pressure to cut
nicely and there's no way to get that kind of pressure cutting teflon.

> The previous postabout lapped mirror finish is exactly right, the smoother
> you get your reliefs the less distortion you will have in your finished parts.

Many years ago (1955), working as a technician in a hospital, I spent two days
making a set of cutting tools for teflon.  It took some fiddling to get it right 
and there was no guidance in the literature because teflon was so new at the time. 
Those lapped bits were so pretty that I put them in a nice box with molded in
foam.  So this MD, who needed to do a quick job on the lathe for an experiment
of his, not knowing how to sharpen tool bits, took my bits and used them on 
stainless.  What he didn't break, he burned.  Lesson: those bits are hard work
to get right.  Keep them under lock and key--they are a temptation because they
do look nice.   

> Machine it 

Cautionary note on that. If it's a big diameter and you run too fast, you
get standing waves (wobblies) formed on the work--okay, so maybe my lathe 
isn't tied down well enough and I have some vibrations here and there.
Generally, I found that for rough cuts, aluminum speeds
are great, but for finish cuts to precision I slow way down. 
 
Boris
Boris Beizer

-----------------------------------------------------------------------------------------------------
Dr. Boris Beizer                                  Seminars and Consulting on
1232  Glenbrook Road                       Software Testing & QA
Huntingdon Valley, PA 19006 USA
TEL:     215-572-5580     FAX:  215-886-0144     Email:  [email-masked]

Note:  After July 1, 1996, [email-masked] will not be active.
Please update your directories and use the above address
([email-masked]) in the future.   Thank You.
-----------------------------------------------------------------------------------------------------

---

From: [email-masked] (Boris Beizer)
Date: Thu, 06 Jun 1996 14:15:27

In article <[email-masked]> Ron Yost wrote:

>I've had trouble with little threads of Teflon wrapping themselves around the
>stock and clogging the cut - have to stop now and again to clean it all out. I'd
>thought it was caused by static electricity making the threads cling to the rod,
>but I suppose my bits aren't ground properly. Same thing happens with Nylon.
>
>Thanks a lot for the bit grinding and lapping info - I'm sure that's my problem!

That **is** yet another problem I forgot to mention.  If those are really thin
little threads (as it seems) then they are probably caused by the rough grinding
of your bit.  The swarf should come off just like for metal.
   For what it's worth, it's not static.  It's mechanical. Following your lead,
on a hunch, I just tried to see if lubricating with an anti-static spray did any good.
Other than the miminal cutting improvement due to lubrication, it didn't affect the
plastic's tendency to wrap around.  Tried it with lexan, teflon, nylon, and acrylic.
They all wrap and the softer the plastic the worse the wrap.  Lowered speed and 
coarser feed seemed to help.
   I never thought about this annoying little problem.  Any ideas out there?
How about trying something like a chip-breaker notch? Or maybe we need some
side rake?  Obviously, the ideal tool wouldn't have these problems.  Must be
a ***real*** soft-plastic machinist out there with the definitive answer.

Boris
  
Boris Beizer

---

From: [email-masked] (Peter Drumm)
Date: 7 Jun 1996 11:03:06 GMT

:->   I never thought about this annoying little problem.  Any ideas out there?
:->How about trying something like a chip-breaker notch? Or maybe we need some
:->side rake?  Obviously, the ideal tool wouldn't have these problems.  Must be
:->a ***real*** soft-plastic machinist out there with the definitive answer.

I saw plans for a tool for turning plastics in some magazine years
ago. It was a short piece of drill rod, drilled thru the center to
leave a ~1/16" wall tube. The top end was then countersunk with a 60d
c/sink to make the cutting edge, hardened and placed in a holder at
~15d back rake. The chip, or string, was supposed to go thru the hole,
and end up in the chip pan. I never did try this, maybe someday...

[email-masked]
Using Warp/Neologic News/PMMail/iLink2/WebEx
Wausau, WI. 44d 58m 00s N x 89d 36m 45s W
All opinions are my own, even if they are wrong!

---

From: [email-masked] (Clhuprich)
Date: 10 Jun 1996 15:31:56 -0400

For HSS or cast alloy tools or carbide, single point turning :
back rake angle : 0 deg
side rake angle : 0 deg
end relief angle : 20-30 deg
side relief angle : 15-20 deg 
side & end cutting edge angle : 10 deg
 
DOC is depth of cut
SFM is Surface Feet per Minute
IPR is inches per revoloution

   For .150" depth of cut (HSS) :
250-350 SFM
.010 IPR
  For .025" depth of cut (HSS M2 or M3) :
300-400 SFM
.002 IPR
  For .150" depth of cut (carbide) :
400-450 SFM
.010 IPR
  For .025" depth of cut (carbide) :
450-500 SFM
.002 IPR

  If the teflon is filled all the above is off -- I'm assuming unfilled
teflon.

  The above data is from the Machining Data Handbook, 2nd edition, 
1972, published by the Machinability Data Center, a DoD Information
Analysis Center, Cincinnati, OH

  From the 3rd edition, 1980, (now published by Metcut Research Associates
Inc.,  3980 Rosslyn Drive, Cincinnati, OH 45209 :

  For .300" depth of cut (HSS M2 or M3) :
300 SFM
.010 IPR
  For .150" depth of cut (HSS M2 or M3) :
350 SFM
.008 IPR
  For .040" depth of cut (HSS M2 or M3) :
400 SFM
.005 IPR
  For .300" depth of cut (carbide C2) :
500 SFM
.012 IPR
  For .150" depth of cut (carbide C2) :
550 SFM
.010 IPR
  For .025" depth of cut (carbide C2) :
600 SFM
.005 IPR

  For diamond tools :

DOC=.005-.015; SFM=1000-2500; IPR=.003-.006 
DOC=.015-.050; SFM=500-1000; IPR=.006-.012 
DOC=.050-.125; SFM=300-500; IPR=.012-.020

  Metcut was purchased/aquired by the Institute of Advanced Manufacturing
Sciences, Inc. 1111 Edison Drive, Cincinnati, OH 45216-2265  TEL. (513)
948-2048 FAX: (513) 948-2109

  The data is now available as a computer program --- and is being
integrated into some higher end CAD/CAM systems. If the hardcopy manuals
are still available they are well worth their cost. The above data
is only for one material and type of material removal process.

  I am not affiliated with any of the above companys --

Cliff Huprich
CAE/CAD/CAM Systems & Applications Engineer/Programmer

---

From: [email-masked] (Peter Brooks)
Date: 10 Jun 1996 18:01:07 GMT

I'm not a plastics machinist, but I've had much the same problem when turning
Delrin rod stock.  The best answer at the time was to rig the shop vac nozzle
as close to the cutting tool as I dared.  With the vac at full suck, the swarf
never got a chance to wrap around.

Pete Brooks

---

From: [email-masked] (Clhuprich)
Date: 11 Jun 1996 13:41:15 -0400

P.S. -- use an air blast on the cutting area to break up & remove the
chips. 
Cliff Huprich

---

From: [email-masked] (Clhuprich)
Date: 12 Jun 1996 18:36:38 -0400

Another method of chip control, if the part & tool geometry allow it,
is
to stop the lathe, advance the tool into the work at the tailstock end,
and then move the tool towards the headstock, thus scoring the stock.
   The chips may then break at the score as you cut -- of course this
cycle must be repeated for each pass but works well for the finish cut
on some materials.
   Do not score deeper than the final pass cuts --

Cliff Huprich

---

From: [email-masked] (Edward Haas)
Date: 12 Jun 1996 08:23:36 -0700

--A spray-mist unit helps blow the chip (not "chips": there will 
only be one big one and some dust ;-) ) off of a milling setup. For the 
lathe, a vacuum is good, although I like to supplement with one of those 
bamboo barbecue scewers, to hook the stuff out of the way of the chuck, 
etc. For a CNC setup, I would recommend programming in some pauses, to 
get a chip out in sections, so that it doesn't all run together and foul 
up the workpiece.
-- 
	"Steamboat Ed" Haas	:	Another proud member of 	
	COMING SOON		:	The Anti-Virus Vigilanties
	http://www.west.net/~steamer  	
		---Decks a-wash in a sea of words---

---

From: [email-masked] (David E.Hockin)
Date: Wed, 12 Jun 1996 09:45:55 GMT

Take care not to let the teflon get hot - it gives off toxic 
fumes if you do.

Dave.

-------------------------------------------------------------------
[email-masked]     | "my thoughts are mine alone, and not
			   |  those of the University"
G4UGT                      |
                           | But I wouldn't mind betting they've
                           | someone working on that already!
------------------------------------------------------------------

---

From: [email-masked]
Date: Fri, 14 Jun 96 22:25:45 PDT

Well, we make teflon washers for needle valve packing nuts.  They vary in 
sizes (1/4 to over 1")  and wall thinkness (up to 1/4") and we drill the rod, 
and part them with razor blades.   Cuts clean and pretty much burr free.  Best 
advice is to hone your turning tools to a super keen edge, to avoid pushing a 
burr.  Drills rarely have a problem if properly sharpened.   Turning speeds 
and feeds can be very high, as this stuff will not generate too much heat.  
Cut everything dry.

Thomas