Teflon Job Time Q please.

Hello, I'd like some CNC timing help / guide with a Teflon job

Material ;- virgin Teflon (PTFE)

Quantity 1000 plus.

Part ;- Machined from solid bar, a ''Cup'' , 3.290" OD (+/- .005'') with a 0.031" wall,(+/-.002") 1.290" deep (+/- .005") with a 0.130" Radius on the base wall corner, with matching internal rad of 0.099"

I'm thinking they could be bar fed and parted off??

Any help much appreciated.

Many thanks for your time.

Sami.

Never made anything out of teflon with that small of a wall on that large of a part, you can machine it 100 mph. You may need to put a plug in the i.d. to be able to turn it quickly and not collapse the bore.

I was doing some 6"+ diameter caps that had .25 walls and after I machined them the thin walled open end relaxed overnight about .045 larger. I worked with it and ended up machining the inside at a taper and undersized so it would relax straight. The OD was a little different but that didnt matter, just the fit on the inside.

Not sure if this will do the same in PTFE or not, I was using UHMW.

Charles

Bar feed will work. Ditto on an ID plug(and maybe slight pressure from tailstock to get the plug from falling out).

Sharp, positive (10 degree +) tools.

For that many I think they need to look at molding it, stuff moves a lot, and by a lot I mean way too much.

I'd make one, see how far off it is after parting it cause that will throw it a mile all over the place, make another one to compensate, give it a day to move, then see if you wanna make another one to compensate for however it went, give that one another day to see if it stays anywhere near tolerance, and go from there, probably starts all over with the next bar, and potentially even changes as you get further up a bar(heat in the spindle, humidity, stresses, etc). Running a 1000 in one shot would be, a lot of scrap if they are serious about its shape/size. Up side? I have a few drawings here for stuff with +/-.00005" all over and #8 finishes on 3" bronze... gonna need an engineering meeting for this crap. Sounds like a few of us are chasing unicorns these days.

As to bar feeding 3.5 or 4" bar, I can't imagine there's too many machines around doing it, kinda would be funny to see a 50hp machine doing teflon though, as long as I don't have the power bill

you can machine it 100 mph.

Click to expand...

I'M HIP!

Just ran a job of this for the first time yesterday. I kept cranking it up and up and up. 'Till finally it wasn't gunna make much diff in cycle time anymore, and just wear more on my machine. I was concerned with finding a "melt" point, but never did.

I imagine it's up there somewhere, but I didn't hit it. I was running 1300 SFM on a face mill and 400SFM with an endmill.

I don't know how turnings would break tho. ???


-----------------

Think Snow Eh!
Ox

Turnings will break if you hit it hard enough on feed.

having m/c'd a fair bit of it this year, I know the stuff squirms around like a hooker on a barstool, and the tolerance problems.

I was reckoning on a ball raced support plug from the tailstock before turning the OD,..... as I was also considering doing it in 2 hits.

Really I was thinking more of approx CNC cycle times, to get a rough idea whether it would be viable on a manual machine.

teflon..

I would start with 3.5" material if you can bar feed that dia. face it it then bore your inside feature then turn the dia. in 1 pass. had to do several thin wall parts in that fasion. then bring in a angled grooving tool to part it off

Well in material like this - tooling will make all the diff in the [known] werld.

Just hitting it with a 3/4 drill to start with and then open up in interp with a boring bar could take a few minutes to drop one off.

But - as you would know - if you made up a "drill" to your spec and plunged it and called it good - you should be able to knock that hole in there in seconds. Even on a W&S.

As for holding the tols - that would classify as "The devil is in the details" applies heavilly here.

One big drill (tool?) ran slow could very likely be the coolest means of running it as there would not be much "pushing" of the heat I don't think - like you would git in a multi-pass boring bar setup. And it would negate the chip issue on a boring bar.

A form tool on a cross slide and you don't have any ratts nests to worry about - other than maybe on the cutoff? You could prolly compete very well with a big CNC.


-----------------

Think Snow Eh!
Ox

My thanks to one and all,.......... the back story was I'd priced the job and owing to my experience of the nature of the material, at a conservative rate of 12/hour.

I understand there's another quote ''flying about'' which ''must'' have been worked on at least 30/ hour,......... it turns out from a CNC shop.

While I've been conservative - scaredily careful even I felt sure 2 mins a pop was crazy, and Ox's last sentence more or less confirmed my suspicions.

I think the job's been put back in the melting pot for another go-round, so all is not lost - yet.

Take Care

Sami

I prefer turning Teflon with very sharp ground tools, HSS or carbide, and using grooving tools as much as possible.
Dry machining the stuff could possibly create a dangerous situation if the tool melts in the stuff, as Teflon produces Hydrogen Cyanide around the melting point, pretty deadly stuff.

So as atractive as it looks to machine it 100mph, i take it a little slower and use coolant if i can.

And dont get the stuff in your cigarette.
Ive worked with a guy that had a chemical fever of the stuff, and he tought he was gonna die, he also warned me and i took his advice serious.

Limy Sami said:

Hello, I'd like some CNC timing help / guide with a Teflon job

Material ;- virgin Teflon (PTFE)

Quantity 1000 plus.

Part ;- Machined from solid bar, a ''Cup'' , 3.290" OD (+/- .005'') with a 0.031" wall,(+/-.002") 1.290" deep (+/- .005") with a 0.130" Radius on the base wall corner, with matching internal rad of 0.099"

I'm thinking they could be bar fed and parted off??

Any help much appreciated.

Many thanks for your time.

Sami.

Click to expand...

WOW! Tight! Ouch!

The material moves a bit. Rough and leave about .100" on both sides. Leave over night and see what happens. Maybe put it in the oven 200 degrees f. and then the refrigerator 40 degrees f.

Then cut leaving .020" on both sides and leave again. Notice the change if one exists.

The try to bring it to size. ???? I don't know?

Carl Edward Johansson of "Jo Block" fame raised and lowered the temperature 80 or so degrees f. several times to "Stretch and shrink" the moleular structure of Jo Blocks so they settled down.

***
Gage Blocks
Gage Blocks are the basic for all the measurement equipment in the metal workshop. Carl Edward Johansson is the developer of the first gage block. ...
Gage Blocks -
***

I wonder if that same process could "Settle" Teflon???

Leave room on the quote! Not many people can make this on size I would bet!

Best regards Sami,

Stanley Dornfeld I'd be curious to know how you wind up doing this.... Thanks.

Carl Edward Johansson of "Jo Block" fame raised and lowered the temperature 80 or so degrees f. several times to "Stretch and shrink" the moleular structure of Jo Blocks so they settled down.

Click to expand...

"Hydromat" (Switzerland I believe) made a note when they started making their transfer machines back in the mid 80's that they put the raw castings out in the snowbank for a yr to "age" them.

I wonder if they held to that routine strictly, or if mass production during the 90's cought up to the casting process ever?

Dry machining the stuff could possibly create a dangerous situation if the tool melts in the stuff, as Teflon produces Hydrogen Cyanide around the melting point, pretty deadly stuff.

Click to expand...

Just keeping some air flow throgh the werk zone should negate that eh?

How does this stuff react with coolant? Does it soak it up? If so - does that effect the size at all?

And dont get the stuff in your cigarette.
Ive worked with a guy that had a chemical fever of the stuff, and he tought he was gonna die, he also warned me and i took his advice serious.

Click to expand...

I may have done or tried some really dumb stuff in my day, but even considering sucking on something that was burning never sounded like a sane idea. ???


-----------------

Think Snow Eh!
Ox

Limy Sami said:

Hello, I'd like some CNC timing help / guide with a Teflon job

Material ;- virgin Teflon (PTFE)

Quantity 1000 plus.

Part ;- Machined from solid bar, a ''Cup'' , 3.290" OD (+/- .005'') with a 0.031" wall,(+/-.002") 1.290" deep (+/- .005") with a 0.130" Radius on the base wall corner, with matching internal rad of 0.099"

I'm thinking they could be bar fed and parted off??

Any help much appreciated.

Many thanks for your time.

Sami.

Click to expand...

Ok, one more thing...

I cut some nylon with standard tools. The burr created left another machining operation.

I remembered this guy who said, "When cutting nylon use a 15 degree relief on the tool."
It worked like magic! 16-8 finish. Really!

Teflon is maybe even "softer" than Nylon. Try 20 degree relief on the tool. It may cut the Teflon without rubbing the back side of the tool and "Burnishng or stretching" the surface making it longer and hence increasing the bore size.

I'd use the same surface feet, cutting speed, as steel. Because the material can't get rid of the heat of cutting.

I don't know if you want any back rake. That might pull the cut in and the size would be unstable there too.

Regards Sami,

Stan-

Thanks Stan,......... like I said I've been doing a lot of plastic this year - a new ''hook up'' and while like most machinists I've done the odd bit of nylon etc this has been an interesting new experience, and at 55, quite a steep learning curve.

OTOH I found you can get away with ''moves'' on plastic, that with metal would have the workpiece, tool and probably bits of machine whizzing past your ear at great velocity


To run through Stans points, which are aplicable to un filled plastics,....... filled are another ball game entirely.


''I cut some nylon with standard tools. The burr created left another machining operation.''

So did I, and it will . time for a rethink.

''I remembered this guy who said, "When cutting nylon use a 15 degree relief on the tool."
It worked like magic! 16-8 finish. Really!''

It sure does.

''Teflon is maybe even "softer" than Nylon. Try 20 degree relief on the tool. It may cut the Teflon without rubbing the back side of the tool and "Burnishng or stretching" the surface making it longer and hence increasing the bore size.''

20 deg is much better on Teflon, and rubbing tools do effect heat , surface and therefore size

''I'd use the same surface feet, cutting speed, as steel. Because the material can't get rid of the heat of cutting.''

So do I, because it does.

''I don't know if you want any back rake. That might pull the cut in and the size would be unstable there too.''

Careful with back rake, on the harder plastics it'll pull in allright, (just like brass) especially Delrin

Clearance clearance clearance, and sharp sharp sharp are the watch words, did I say sharp?.............. I'm talking as in 8 or 10X glass sharp - look at a ''standard'' cutting tool under a an 8X glass and chances are the edge will look like it's been chewed by a dog.

The smoother the surfaces the chip flows over, the better,............ forget about coated tools, they're not needed and are often not sharp enough.

Threading & tapping the softer plastics, including Teflon is a whole new ball game! and while I don't want to bore the ass off the PMers, if any want to know I'll reply.

Take care,. sharp end to the work.

Sami.

So Sami.. I guess I was on the right track. Thanks for the nice validation. I actually hadn't done it before. You give me more info for my "Toolbox."

It also sounds like you are way ahead of me on this. I hope you catch the job and have good results.

Best regards,

Stanley Dornfeld

I don't see how someone could do 30 an hour and still deal with the mess, even with a chip conveyor, your probably going to have to stop the machine every 5 parts or so for clean up.

Metalcutter said:

Carl Edward Johansson of "Jo Block" fame raised and lowered the temperature 80 or so degrees f. several times to "Stretch and shrink" the moleular structure of Jo Blocks so they settled down.

***
.

Click to expand...

Fun bit of trivia: There is not much molecular structure to speak of with steel. Other than the random carbide and inclusions it is 100% metallic bonding - no molecules at all.

Dimensional changes over time are frequently caused by the conversion of retained austenite into untempered martensite (which is less dense - thus takes up more space - thus causes movement). Temperature fluctuations can cause RA to convert. An additional temper cycle is very helpful too. The gold standard is cryo as a part of HT (after quench, before a full temper).

.. there ya go...

Carl Edvard Johansson (1864–1943) is the correct spelling. (Edvard instead of Edward)


His is quite a story, in the Moore Book "Foundations of Mechanical Accuracy."

Regards,

Stan-