<=16 RA finish -- mill or lathe?

[cnczoner]

Hi,

I need to create a part with a seat for an O-ring (under 3/4" dia). I made a polycarbonate prototype using my CNC-converted HF drill-mill, and it had a leak, so the O-ring manufacturer informed me I need to have a 16RA or better finish).

Is this achievable with a benchtop mill, which only does 1500RPM? And if so, what type of endmill should I use? I used a Maritool 3-flute, 0.25" HSS endmill with a 0.030" corner radius, but perhaps there is something better...?

Alternately, I have a 7X spindle speeder, and I can use a 3/16" endmill on it -- would the higher speed be better to get the 16RA finish?

Alternately 2, would it be better for me to use my (manual) lathe (Grizzly 10x22) to get the 16RA finish? I would like to avoid the secondary process, but if it gets me the required finish, I will.

Thanks,
-Neil.

[mactec54]

cnczoner

What size oring are you using & how much crush/compression do you have on it

[eartaker]

Using the lathe would give you the finish you want along with a perfectly round seat. If it is possible for you to place your part in the lathe I would go that route. If not try using a ball endmill with the dia. you need for the O-ring.

[cnczoner]

Not sure how much crush/compression, but the O-ring is a -015 (0.691" OD, 0.070" wall). It's not for a moving part, but rather a seal for a pressure sensor, that will see up to 150 PSI. The size is specified by the sensor manufacturer.

Very new to using a lathe, but I agree about getting it perfectly round. Thinking through this now, it think it could be relatively easy if I spend some time up front to make a jig etc, so that I can make the overall housing on the mill first, then easily position/align it on the lathe to cut that seat. I'm assuming I'd just get some type of insert with the correct radius for the O-ring.

Another thought -- could I do the same-ish thing with a boring bar/head in the mill? Not sure if those can go down to 0.691".

I need to do about 500 of these, so don't mind investing in the correct tooling.

[hoss2006]

would an 11/16 (.6875) reamer be close enough for you?
Hoss

[cnczoner]

Hmmm... that's actually *very* close, and I'd think it would work. Wasn't sure that this option existed (as the only reamer I ever used was a long one with a few steps for opening up wooden R/C airplane props a couple decades ago). But I'm looking at reamers now on mcmaster, and they have 0.691" reamers. What I'm not clear on is if the bottom is flat or if it has a corner radius, etc. However, will this give me a 16RA finish? I'm thinking it should as the mill would be held in one place while the flutes cut all parts of the circle the same way.

I'll draw up a diagram of how the o-ring sits when I get back later.

[pp7]

I've done O-ring grooving on both the lathe and mill. I get a better finish on my lathe. For the lathe, I predrill a starter hole and then use a boring bar to get the bore to the proper ID. I use a O-ring groove tool in my lathe to cut the groove. For the mill, I bore the hole with a boring head. For the O-ring groove, I ground down an old boring bar in the shape of the o-ring groove and fitted it in my boring head. I lock my Z and gradually increase the diameter of the boring head offset. I've never actually used a reamer, so I can't compare finishes.

[hoss2006]

Hmmm... that's actually *very* close, and I'd think it would work. Wasn't sure that this option existed (as the only reamer I ever used was a long one with a few steps for opening up wooden R/C airplane props a couple decades ago). But I'm looking at reamers now on mcmaster, and they have 0.691" reamers. What I'm not clear on is if the bottom is flat or if it has a corner radius, etc. However, will this give me a 16RA finish? I'm thinking it should as the mill would be held in one place while the flutes cut all parts of the circle the same way.

I'll draw up a diagram of how the o-ring sits when I get back later.

You can get a mirror finish with a reamer if you do it right with plenty of oil.
here's some guides.
Technical Tips - Reaming #8 especially
Reamers Guide
Hoss

[mactec54]

cnczoner
I'm still not sure how you are trying to make this as a .250 or .187 endmill would not be able to do this

You are looking at a Groove of .084 to .089 Groove Max width, for air/gas, & a depth of .050 to .054

A RA32 is normal, for a oring with that pressure, But the groove width & depth has to be right or it will never seal

Your Oring groove needs to look like this drawing

A reamer won't do what you need as it can't machine the bottom, the side finish does not matter so much, the bottom finish, width & the depth are what makes it work right

http://www.oringswest.com/

[cnczoner]

This is the design I did...


The O-ring manufacturer says I can use square corners ("CORNER") in the drawing, but in my last prototype, I also tried a 0.030" radius (using a corner-radius endmill). (Note that the O-ring has a 0.035" radius).

[mactec54]

cnczoner

The biggest radius that is allowed with that oring size is from .005 to .015, .030 is way to big

Looking at the drawing you would need to have max compression, of the oring to make it work/seal, & a square corrner does work but is not ideal

[ninefinger]

Is this sensor used on some standard type of equipment? Does it normally have a threaded connection? I ask because the -015 o-ring is a bit unusual and so is the sensor sealing surface shape - its not something that you see every day (compared to the normal run of the mill o-ring sealing types - BSPP, SAE o-ring boss, code 61/62 flange, metric ISO 6149-1, etc...) Did the manufacturer send a drawing of how it should be installed?

What controls the compression of the o-ring - over compression can cause a leak as easily as under compression.

Lastly, you do not mention at what pressure your prototype leaked but I think your pushing it with 150 psi and that design in polycarbonate....it could have deflected and that caused your leak. Lots of things to consider here.


Mike