What's new
What's new

Milling internal circlip grooves

Michael Moore

Titanium
Joined
Jun 4, 2004
Location
San Francisco, CA
Is there some sort of little saw or milling cutter that would be used to make a groove in a bore for an internal circlip?

I've looked through the MSC catalog and I don't see anything that seems specific for that application. The TruArc website doesn't show any corner radius at the base of the groove but it seems like you'd want some radius in order to reduce the chance of cracking from the corners (maybe that's not a significant concern).

I know that you could do this with a grooving tool in a boring/facing head but it seems like there must be some sort of production tooling that would let the mill do a circular interpolation to form the groove and then retract and leave the hole.

1" OD seems to be as small as the jewelers/slitting/slotting saws go. It looks like for a .056" groove (30mm ID hole) you might need to make two passes with a little bit of offset between them as many of the small saws are pretty thin.

cheers,
Michael
 
I do it with modified woodruff key cutters. I send a print to my tool grinder and he modifies one to suit the print. I haven't seen ready made tools anywhere so far, other than the automatic tools that plunge in and expand to a preset diameter.
 
Woodruff Keyway cutters are what I use. They are the easiest to come up with, and will get the job done quick.
They come in both carbide tipped, and HSS.

Doug.
 
If you have access to a surface grinder, a grinders vise and a 5c spindexer you can make one pretty easily from a woodruff cutter. Try to find one as close to size as you can get. The staight tooth ones work better for this method. What you do is stand them up in a v-block and surface grind thkns of the cutter a few thou over the high limit of the width of the groove.

After that is done put them in a 5c spindexer and relieve your grinding wheel as if you were going to sidewheel grind a slot. next put the indexer in a ginders vise or on a sine plate and tilt upwards approx 10 to 20 degrees. now set the bottom of the grinding wheel at the approx center of the cutter, bring the grinding wheel and cutter close together and eyeball it. now while spinning the indexer clockwise by hand feed slowly into the wheel. the whole purpose of tilting the indexer upward and grinding the face of the cutter is to creat a concave surface for chip clearance and so the cutter won't rub. you need to keep taking a little at a time till you get to the face width of your groove. i hope i've explained it clearly enough, if you have any questions just ask.

good luck
 
Sandvik has insert cutters for this, a solid shaft, and different inserts depending on the width of the groove.
Can also do thread milling with special inserts.
The insert has 3 cutting edges.

But I can't remember the name..

Horn has the same typ of tool, but at least here, Sandvik i cheaper.
 
I use lathe style boring bars with a grooving insert, like Top Notch, which are readily modified to suit custom widths. It is like fly cutting, but it is possible to feed quite aggressively because the arc of insert travel is typically a significant fraction of the bore size, so it blends in very well in interpolation.
 
You can use Thin-Bit round internal lathe tool holders and just interpolate from the known minimum bore of the holder. If you want radius in the bottom im sure they have it. They sell direct too witch makes it even that much nicer. Worst case situation you could also use a jewlers slitting saw with interpolation.
 
Michael,

Check out McMaster-Carr page 2471 "Narrow-Width Keyseat Cutters" smallest is 1/2' OD with a .02" width.

Hope that helps.
 
I think fmari mentioned something about custom key seat cutters in his thread about custom endmills.

I have made them in the past the way chip maker describes. It doesn't take much time and I usually have something in house I can modify. Of course this is assuming you have a grinder availlable.
 
Thanks for the info. I'm surprised that there aren't dedicated cutters for this kind of job, as I thought it would be a common industrial operation.

I've got a Narex boring head I can use. It didn't seem likely to me that commercial shops would do production stuff where they'd have to have an operator come over and operate a facing head for each groove, and the CNC controlled facing heads seemed like they might be fairly uncommon (and expensive). I also didn't expect to find that many people felt forced to modify/grind their own custom tooling to do this kind of thing.

It looks like a lot of those small woodruff cutters don't have much reach to them before the shank would start to interfere with the bore. They'd work for a circlip groove at the outer end of a bore, but if you need one farther in so there is a circlip on both sides of a bearing you might have some issues to deal with.

cheers,
Michael
 
Can you give some more specifics such as bore diameter/depth, groove dims, material? How many do you have to make? I had not thought of spinning a boring or grooving bar on center, then interpolating. Seems like a great solution to make circlip grooves with the cnc.

What would you imagine a dedicated cutter for this job would look like?

QB
 
I bet >25% of the woodruff cutters in my collection have had thier shanks ground down. I find them handy sometimes when the part has a side feature, like a notch, and I want to run the part from one side. Especially a whole strip of parts. They always seem to need additional clearance ground off the shank in this scenario.

As for being surprised they aren't a common stock item (someone may make exactly what you need) I can relate. I find myself many times saying "I can't be the only one who needs this" or "this has got to be a common tool" only to spend too much time looking for it, then, if I do find it, saying "whoa at that price I can find another way".

Keeps things interesting.

Gunnar
 
QB, here's a sheet with specs on what I think is a common series of TruArc internal circlips

http://www.truarc.com/pdfs/N5000 Series.pdf

A 30mm (1.181") bore would have a 1.255 +/- .004/005" OD groove that is .056 +4/-0 wide. So that would seem to be a cutter that is at minimum arbor diameter + 2x.037" x .056 thick. It seems like a 1/2" shank cutter with a 3/4" OD cutter would fit.

MSC shows a carbide slitting saw that is 3/8" hole x 1" OD x .031 or .062" wide for about $40. Robb Jack makes some carbide slotting saws that are 1/4" hole x 3/4" OD x .020, .040, .060 but at $100-150. Their 1/4" hole arbor is 1/2" OD and they want $200 for that.

Dave, those Harvey Tool cutters seem to be what there is, but it doesn't look like they'll cut grooves much past the outside opening of the bore.


I'd thought that these kinds of grooves would want a radius on the corners but maybe that isn't standard practice. Most radiused grooving inserts that I can find in the catalog seem to start at about .118" width.

cheers,
Michael
 
NJ Gunnar,
This is exactly one of the reasons why I will have a Keyseat cutter customizer. I've had many reasons to modify keyseat cutters, this is one of them.
 
circlip cutters

Hi All:
I make my own cutters too, but I grind them from solid carbide for small sizes (under 1/2 inch diameter) and use broken 1/8" shank milling cutters in a bar made from an ejector pin cutoff for larger sizes.
I make them 2 flute and grind them with a diamond wheel and a spin fixture in the surface grinder.
I can make a cutter almost as fast as I can order it...certainly much faster than I can source it if it's an oddball.
2 flutes have always worked best for me.
Cheers

Marcus
 
Those woodruff cutters are Huge compared to what you need somedays.
I took an old 5/16 reamer, and cut off almost all the flutes, lengthwise.
Then ground down the remaining flutes to make a Snap ring cutter to go into a 9mm bore.
I think the width of the groove was aroung .020" IIRC.

This was for the snap rings for the axle shaft on a set of roller lifters, for a CAT 3208 block, running alcohol, and three turbos.
The lifter bodies were 7075, and those cat lifter bores are huge. So, some hollow body aluminum roller lifters worked out pretty good.

I'm surprised there is not a standard solution to this problem.
 








 
Back
Top