Suggestions For Clearing Chips From O-ring Dovetail

[lerman]

I'm cutting a dovetail groove for a two inch diameter o-ring in 6061 aluminum. I found that the chips welded to the groove for the first 1/2 inch or so, until some clearance developed. The minimum width of the groove is .125, the speed was 2760 rpm (the max for my machine), the depth is .112, the tool is carbide with three flutes. I used a feed of about 3 ipm.

Any suggestions on how to do this better?

Thanks,

Ken

[mrainey]

Got a picture of the part and/or tool?

[lerman]

The tool is: http://www.internaltool.com/series51/index.htm EDP number 51-8020. The o-ring is a nominal two inch diameter. Photos will follow.

Ken

[mrainey]

Ken,

Without seeing the photo ...

Of course, the first and least-desirable thing that comes to mind is a separate roughing pass, which is expensive and probably not needed (don't know what your size and finish tolerances are, how well the tool cuts, etc.)

As an alternative, how about holding off a little and rough machining the first 1/2" to give the chips somewhere to go, then pulling out and taking the whole thing to size?

Feedrate is under .0004 per tooth - might be able to go up on that depending on the tool.

[lerman]

The problem is that because it is a dovetail that cuts to the desired profile, it can't be cut at partial depth.

I could do a rough cut for the first half inch with a 1/8 inch straight mill and then change to the dovetail cutter. I'd like to avoid that.

Looking at the attached file:

1 -- At the bottom is the entry point. I plunge .112 at 20% of the feed rate (3 ipm). I then mill out to the groove (the diameter is 2.123). I mill around the circumference. Then back to the entry hole and out.

2 -- Near the bottom, you can see an uneven area where the aluminum welded to the groove. Also, there are two areas where the edges of the groove have been destroyed.

3 -- The process that generated the part included my seeing that the chips were not clearing and turning on air and coolant at around the area things cleaned up. I then ran the program a second time to clean out the welded area. I later turned down the coolant and air and the chips cleared just fine with an occasional squirt of air.

4 -- It could be that the solution is to apply heavy air and coolant at the beginning. I'll also try turning down the feed to 1.5 ipm.

I don't mind heavy use of the air, but the coolant makes a mess. I have a system that mixes coolant and air that I'm using, but it tends to give way too much coolant. I'm going to add a regulator on the coolant line so I can increase the air without over doing the coolant.

Thanks for your ideas.

Ken

[mrainey]

I'm assuming the dovetail is there to keep the o-ring from coming out.

Since you have to make a full-sized entry hole anyway, any chance of doing it with a center-cutting end mill of the same diameter as your dovetail tool, then using the end mill to interpolate a little more of the circle to make some chip room?

Probably wouldn't be thinkable if you're making it for a customer, but sometimes for in-house stuff things like that can be worked out (after speaking with your friendly design engineer, of course.)

Or maybe plunge an 1/8" wide groove ahead of time? Easy and fast on a lathe or machining center, with a bit of creative tooling.

An air blast from the start sounds like a real good idea.

[lerman]

Yes. The dovetail is to hold the o-ring in place.

In this case, I am the customer -- in the sense that this is part of a product that we will be selling.

I could make a separate pass with a 1/8 inch endmill, but would like to avoid the tool change (since they are all manual on my machine).

Thanks for your help.

Ken

[Mcgyver]

On dovetails, i've always done/been told/read to end mill out the bulk of it and use the dovetail for the triangles - i've havn’t done a dovetail this small or via cnc but would guess the principal (the size of cut is excessive to the small part of the cutter) would hold.

as a good finish with an end mill usually requires separate cuts on each side, if the slot is only 1/8, you are going to be using some small cutters! Being cheap and not wanting to bust the cutters, it would take a bunch of passes to rough it out to .112 deep. I'd be inclined to do it in the lathe with a tool ground for trappening and then a couple bits ground to the the left and right side of the dovetail. Finish would be excellent, tooling is inexpensive and it might be quicker to machine. How may do you have to make?

[Geof]

Looking at your picture I would conclude that the function of the O-ring is to act as a seal; taking the place of a gasket between two parts. If these two parts are simply assembled and used the dovetail groove is redundant because it does not contribute to the integrity of the seal and assembly is quite simple with a parallel sided groove. Assuming that the dovetail is needed to retain the O-ring because the parts are frequently diss-assembled and re-assembled in normal use is it necessary to stay with a 1/8 cross section O-ring? If you change to a 3/16 section O-ring machining the dovetail groove would be possible with a first cut round the center of the groove, a second cut at a smaller radius to finish the inner wall and a third cut at a larger radius to finish the outer wall. Both the second and third cuts could be done at an increased feed and would produce a very nice finish.

[wizard]

Frankly I've never seen a doetail cut for face mounted O-Rings. One thing I would be concerned about would be the ability of the O-Ring to hold its shape and loose it's sealin ability due to migration into the corner of the dovetails.

Obviously not knowing more about the product this is pseculation. However if you are worried about retaining the ring, during assembly or whatever, I'd suggest that a little supper glue in one or two spots might do the trick.

Dave

Originally Posted by Mcgyver On dovetails, i've always done/been told/read to end mill out the bulk of it and use the dovetail for the triangles - i've havn’t done a dovetail this small or via cnc but would guess the principal (the size of cut is excessive to the small part of the cutter) would hold. as a good finish with an end mill usually requires separate cuts on each side, if the slot is only 1/8, you are going to be using some small cutters! Being cheap and not wanting to bust the cutters, it would take a bunch of passes to rough it out to .112 deep. I'd be inclined to do it in the lathe with a tool ground for trappening and then a couple bits ground to the the left and right side of the dovetail. Finish would be excellent, tooling is inexpensive and it might be quicker to machine. How may do you have to make?

[lerman]

My reference for o-rings is Parker O-rings: http://www.parker.com/o-ring/Literature/00-5700.pdf

Parker shows precisely the geometry that I'm using.

My application is for low pressure (1 PSI or so), where a screw on cap will be removed once every week or so.

So far, if the lots of coolant solution doesn't work, the mill an 1/8 inch starting groove first suggestion will be my next try. I'll probably mill down a helical ramp taking about an inch to travel to the full .112 depth. I'm reasonably certain that will work, since the original dovetail did fine except at the entry.

Ken

[psychomill]

I do thousands of these types of o-ring grooves and for many years. I always rough the groove first with a straight end mill, then finish the form with the dovetail. It repeats much better, nicer finishes (since many of these types of application require a really good finish for sealing) and doesn't eat up the tool (dovetail) as fast.

You can actually run the dovetail faster if you roughed it first.