Thread: New CNC - Trying to turn Teflon - Advice Needed

This post is really more of a materials question, and not so much of a "how do I get my CNC to do..."

A little background, I replaced an old boring machine that was turning a taper on a Teflon part. There is a steel rod going through the center of the Teflon, so hold it was never a problem. The boring machine just had a retro fit mist coolant system on it.

I replaced that machine, with a new CNC, which allows me to perform the turning, as well as the secondary operations, all in one (live tooling, drilling through the teflon and steel rod)

I've spent the past 1-2 weeks, playing with feeds and speeds, adjusting angles slightly, adjusting the OD's at the small and large end of the taper, still issues.

SO, here is the current setup

I am trying to machine a taper on some virgin teflon. (It might be 25% glass filled, but I don't believe so)

I'm using a CG5 insert from Circle Tool, with a .007" nose radius. Talking with Circle's engineering group, this is the correct type of insert. - This nose radius is larger than what we'd like, since the part only has a OAL of .380" or so, but, it's what we got for now.

I'm making a 6* taper, with 1 pass with flood coolant. 1400 RPMs @ .0015 IPR

I'm getting a great finish on the part, but when I assemble the part into the mating part, it will not seal. Some parts seal, others don't.

I'm making a light pass, a max of .060" cut at the start of the taper, coolant should be at room temperature, the shop is at a constant 72 degrees.

I know Teflon will creep/settle over time and with different temperatures. I have a very hard time believing I am heating the part enough with the drill through, then taper turn, to cause any significant change in the size of the part, especially with flood coolant.


The mating part is also a 6* taper (not teflon).

Basically this is a stopcock, where the teflon is the rotating part to open/close water flow. I am getting leaks at the top and bottom of the taper. I've been able to elminate a leak at the bottom by bumping the OD larger a couple of ten thousanths, but left the top alone.

I'm chasing my tail I think, because if I adjust the top OD now, I'll be basically back to where I was ratio wise originally.

My frustration is coming from that I am using a new machine, where my old machine was worn out and very slow. Now that I have my new fancy CNC, I can't get it....D'OH!

What I can't figure out, is that if I run a group, some leak, some dont.

The only thing I can think of is the coolant is chilling the part, then later when the part warms up, we are getting a larger part than intended? (or vis versa)


I've considered making 2 passes on the taper, but the old boring machine never did.

I believe my problem now lies that I am relieveing internal stresses in the Teflon, causing it to change size hours after machining. Almost that the part is SHRINKING...I would have thought the part would expand?


Anybody with any Teflon experience please give me your 2 cents. I've delt with a lot of plastics, Delrin etc, but I didn't expect to have to battle this Teflon this much...especially since nothing has changed, other than the machine.



FYI - The turning insert IS different than what we used before. I belive the insert now has a chip breaker (not needed) and that nose radius of .007" is rather large. Our old insert had a much smaller radius, if any, and no chip breaker. But I'm getting an amazing finish with the current insert, so I wouldn't thinking this the problem.

Thank you guys!

About the only way a .007" nose radius is too big, would be in threading. That is not the problem.

Jeff

Originally Posted by jdj

About the only way a .007" nose radius is too big, would be in threading. That is not the problem.

Jeff

Good to know!

I really shouldn't say this, so I don't get eaten alive, but I'm actually an engineer

I believe there's a difference between virgin Teflon and reclaimed. Do you know which it is?

IME the cutter has to be sharp that's SHARP as in 10X glass sharp,....... (I run HSS and hone with a fine Arkansas) if it's not SHARP I've found the tool sorta bulldozes material out the way, which then creeps back.

I keep the speed low too,........ about 150' min max to keep the heat out of the part as plastics are poor conducters.

If the parts thin I'd run 2 cuts, 0.060 is a lot to shift when the material moves so easily.

Did I say the cutter has to be SHARP

Originally Posted by Conrad Hoffman

I believe there's a difference between virgin Teflon and reclaimed. Do you know which it is?

Huge difference. Virgin is the biggest PITA. Glass filled is better to machine.

The print says the material is virgin, but I am contacting the supplier Monday to see if there is any amount of glass in it.

Is that similar to a DCGT type insert that have a very sharp edge and are polished?
Trying to search circle tool CG5 kinda showed me something different, that may not be good for plastics, unless google was wrong, no much info on them?

Teflon loves to move around, you should cut the taper last, with a small finish cut. If you're parting from bar, start parting it off but leave enough that it just hold on enough to take that little OD finish cut, then part the last bit holding it. Just that parting will change the stresses and shape.

Originally Posted by Limy Sami

IME the cutter has to be sharp that's SHARP as in 10X glass sharp,....... (I run HSS and hone with a fine Arkansas) if it's not SHARP I've found the tool sorta bulldozes material out the way, which then creeps back.

I keep the speed low too,........ about 150' min max to keep the heat out of the part as plastics are poor conducters.

If the parts thin I'd run 2 cuts, 0.060 is a lot to shift when the material moves so easily.

Did I say the cutter has to be SHARP

I know we've never honed our inserts but I do know we have special inserts for our plastics. We've seen that also, were the material just get's pushed away, I think that might be our problem.

I still have one of our old inserts, which is diamond coated. Nose radius is almost 0 I believe. No chip breaker, I believe that might also be a problem.

Do my feed and speeds look okay to you?

The wall of the Teflon is pretty thin, actually I think I said that wrong. I believe the wall is .060" thick, and I'm probably taking .030 of that at the max.

Originally Posted by SND

Is that similar to a DCGT type insert that have a very sharp edge and are polished?
Trying to search circle tool CG5 kinda showed me something different, that may not be good for plastics, unless google was wrong, no much info on them?

Teflon loves to move around, you should cut the taper last, with a small finish cut. If you're parting from bar, start parting it off but leave enough that it just hold on enough to take that little OD finish cut, then part the last bit holding it. Just that parting will change the stresses and shape.

I was wondering the same about that insert. Might look into a different one, or one from SECO. The insert has a gold color to it, and I know you don't want to use a coated insert to teflon. But we can't use HSS, everything is carbide.

I do cut the taper last, if I split it into 2 passes (if we think it's needed? wasn't needed before?), how much should I leave for a finish pass?

I tried looking up the exact insert we have, but I can't remember it correctly.

You want a aluminum style up sharp carbide insert. Or properly ground HSS. Theres no way your going to do what you want with a honed insert, its gotta have the upsharp - ground edge. Any honing and you can forget it. Normaly if its a tin coated insert the edges are honed so thats were your problem is.

Originally Posted by adama

You want a aluminum style up sharp carbide insert. Or properly ground HSS. Theres no way your going to do what you want with a honed insert, its gotta have the upsharp - ground edge. Any honing and you can forget it. Normaly if its a tin coated insert the edges are honed so thats were your problem is.

Thank you sir!

Can you recommend a specific insert? We typically only use Circle Machine Company inserts and SECO, since we can usually get them in 1-2 days.

Originally Posted by cold1313

I
I do cut the taper last, if I split it into 2 passes (if we think it's needed? wasn't needed before?), how much should I leave for a finish pass?

It usually takes a little trial & error. You don't want to leave too little, but not too much. With a sharp positive rake, you could probably leave .030-.040 for finishing.

Jeff

Originally Posted by jdj

It usually takes a little trial & error. You don't want to leave too little, but not too much. With a sharp positive rake, you could probably leave .030-.040 for finishing.

Jeff

I'm not taking more than .030-.040 off during the single pass right now. But since it seems the insert I have is possibly the issue, I'll have to look into something else.

I looked at SECO's site, but they have so many, I'm going to have to call them I think.

Originally Posted by cold1313

I know we've never honed our inserts but I do know we have special inserts for our plastics. We've seen that also, were the material just get's pushed away, I think that might be our problem.

I still have one of our old inserts, which is diamond coated. Nose radius is almost 0 I believe. No chip breaker, I believe that might also be a problem.

Do my feed and speeds look okay to you?

The wall of the Teflon is pretty thin, actually I think I said that wrong. I believe the wall is .060" thick, and I'm probably taking .030 of that at the max.

1400ft min @ 150' / min = app 7/16" dia ,.......... if those numbers line up you're about right for the parameters I use.

IMO that's a lot to take off a thin walled Teflon component in 1 cut when you're after the sort of accuracy you are.

I'll double check my numbers in the morning.

So, with my current (incorrect) insert, if I go to 2 passes, should that get me by until I can get a better insert in?

Or am I SOL until I have a different insert?

Got a diamond hand lap? . go at the insert you have and get a SHARP edge as in 10X glass sharp ,.......... IME Assuming you've sufficient clearance the angles are now here as important as the actual cutting edge.

I looked for your insert in Circles but couldn't find it,.......... chances are when you look at the edge under the 10x it won't be anything near sharp.

Originally Posted by Limy Sami

Got a diamond hand lap? . go at the insert you have and get a SHARP edge as in 10X glass sharp ,.......... IME Assuming you've sufficient clearance the angles are now here as important as the actual cutting edge.

I looked for your insert in Circles but couldn't find it,.......... chances are when you look at the edge under the 10x it won't be anything near sharp.

We've got some diamond wheels for our carbide etc, maybe those guys can sharpen this up for me

Originally Posted by Limy Sami

1400ft min @ 150' / min = app 7/16" dia ,.......... if those numbers line up you're about right for the parameters I use.

IMO that's a lot to take off a thin walled Teflon component in 1 cut when you're after the sort of accuracy you are.

I used this calculator Turning Speed and Feed Calculator

And got an RPM of 12,223RPM @ .012 IPR

Where as I'm currently at 1,400 RPM @ .0015 IPR which is around 82 SFM @ 1.8 IPM

So to get closer to your numbers (.260 cut diameter), I would need to run at 200ft min @ 147 IPM, which is 3,000 RPMs @ .050 IPR...which seems insanely high

Eh? say it's 1/4" @ 150' / min I got approx 2250

@ 100 ' /min = app 1500

I'd look to feed about 0.004'' (ISH) / rev - playing with the feed to get the best results.