What's new
What's new

Need source for 60 degree included tapered end mill

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Hey guys I need a couple of square end tapered carbide end mills about .125 small diameter, 60 degree included angle, 6mm to 10mm shank inch sizes ok. I have a RFQ pending with Harvey Tool and will talk to Conical Tool tomorrow to see what they have. MSC has one in stock but it is $223 and I'd sure like a cheaper option. Can't use a chamfer tool it has to end cut.

Anybody know of other good sources?

Thanks!
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
As a hack, I've ground the ends of good single-flute countersinks to make them end cutting, at least linearly. If you get stuck you can try this route, and if need be use an 1/8" endmill to establish the narrow path before starting the countersink.

I like MA Ford's for this sort of use. Not the multi-flute, just the single.
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
As a hack, I've ground the ends of good single-flute countersinks to make them end cutting, at least linearly. If you get stuck you can try this route, and if need be use an 1/8" endmill to establish the narrow path before starting the countersink.

I like MA Ford's for this sort of use. Not the multi-flute, just the single.

That's a good idea. Thanks.

If I can't find a cutter I think my work around will be a 1/8 square end mill. Since this is on a CNC screw machine I can move around and do what i need to do. I've done this part before with a woodruff type cutter down the center and then at the two angles on the side. Just want a better solution. Two diametrically opposed grooves down the length of a 5/8-18 thread in 304ss, so nasty burrs. Gotta rethread and recut the grooves a couple of times to get the burrs to an acceptable point.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
That's a good idea. Thanks.

If I can't find a cutter I think my work around will be a 1/8 square end mill. Since this is on a CNC screw machine I can move around and do what i need to do. I've done this part before with a woodruff type cutter down the center and then at the two angles on the side. Just want a better solution. Two diametrically opposed grooves down the length of a 5/8-18 thread in 304ss, so nasty burrs. Gotta rethread and recut the grooves a couple of times to get the burrs to an acceptable point.

From what you're describing, if you have two powered spindles try a roughing and finishing endmill. I bet you'll get better burr control this way than with a tapered endmill.
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Shaping the cut rather than milling

A 60 degree carbide insert seems like a logical starting point. Just cut off the corners.

This was one of those "why didn't i think of that" moments.

Since you say corners and not corner I assume you mean use an on-edge insert and make a holder so you have a 3 flute rotary tool. With machinery at hand I don't think I can make a tool holder and grind the insert good enough to get all 3 (or even 2) corners cutting together.

Milland said:
So using it like a broach? I think burr control would be painful, and cutting would be slow.

You got me thinking though. I can use tool holder laying on the side and grind one corner of the insert. Then shape the feature in. It is not deep and do this sort of thing quite a bit, usually for internal features. And I can grind one corner precisely. No coating on the tip not the best but will work. No heat generation to speak of.

Thanks for the ideas guys!

Have to calculate time but don't think it will be that much slower than 4 endmill passes, two to get the .130 groove width and 2 more for the angles. Along with possibly 4 more passes 2x to deburr. Thread, shape, rethread, reshape, rethread, reshape, rethread. Might be able to eliminate some of those passes but way better to come off the machine with no hand deburring reqd. The reshaping passes will be 1x not 4x. Think I can handle the shaping burrs ok.
 

gbent

Diamond
Joined
Mar 14, 2005
Location
Kansas
If I understand what you are doing correctly, get a woodruff cutter (wheel cutter for your usage) custom made with the side angles included. Simple to do, and the larger diameter of the woodruff will run circles around trying to cut with a 1/8" end mill.
 

DDoug

Diamond
Joined
Oct 18, 2005
Location
NW Pa
I smell something frying in the kitchen.

The mod has deleted all the post's from the spammer, but as you quoted said spammer, the links are still active.

spammer still wins.

You get maybe 12 hours to edit/delete your post's I would suggest you doo so now.
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
If I understand what you are doing correctly, get a woodruff cutter (wheel cutter for your usage) custom made with the side angles included. Simple to do, and the larger diameter of the woodruff will run circles around trying to cut with a 1/8" end mill.

Yeah for sure!

The Harvey tool I had quoted at $273 each min qty 3 pcs is that type of tool, 3/8 diameter x 6 flute. Can't hold a big woodruff cutter in this machine. Can't swing the $$$. No local tool grinders that can mod a tool that small and it's not an easy one to make. As I said waiting on a special end mill quote it should be substantially cheaper, I hope.

The last time I made these parts about 7 years ago used a 1/8 x 3/8 carbide woodruff cutter. Two passes down the middle to get root width of .130 then a pass on both sides to get the angle. It's just a pain to get everything just right in the corners. Still a pain with a 1/8 square endmill but the tool is a lot cheaper. I never mentioned quantity is only 150 pcs so tooling cost... yeah.

Really looking to balance tool cost versus final part integrity. This customer is very picky and will not tolerate any mismatch at the root of the groove.
 
Just to clarify - cut is a pocket? So a regular 6o deg cutter with the corners trimmed, on an arbor won't work? Even though a woodruff cutter will?

From your description of how you did it originally with a straight side woodruff? It sounds like you can tilt the spindle or the work? If so, a 60 deg dovetail cutter is pretty cheap. again, knock the corners off square to the 60 deg shape, and tilt part or spindle to use for one (or 2) pass cutting.

smt
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Just to clarify - cut is a pocket? So a regular 6o deg cutter with the corners trimmed, on an arbor won't work? Even though a woodruff cutter will?

From your description of how you did it originally with a straight side woodruff? It sounds like you can tilt the spindle or the work? If so, a 60 deg dovetail cutter is pretty cheap. again, knock the corners off square to the 60 deg shape, and tilt part or spindle to use for one (or 2) pass cutting.

smt

Not sure if I can find a double angle circular milling cutter small enough to modify. Really prefer carbide and arbor shank can only be 1/2 diameter max.

The dovetail cutter is a good idea will look into that. Since two passes required the flat width not so critical and a local guy can modify. I might even be able to do that in house.

Thanks!
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Well all things considered I'm gonna use a modified threading insert and shape the grooves. Main reasons for not getting a special cutter are cost and lead time.

I'll post back when I get the parts done. Thanks for all the ideas!

Greg
 

gbent

Diamond
Joined
Mar 14, 2005
Location
Kansas
What is the material given you think you need carbide for only 150 pieces? HSS is much easier to grind. I see that as a 1-hour project with a surface grinder and whirly gig.
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Material is 304SS. Burrs are a big issue with the groove passing through the thread. That is why carbide is my choice. Any slight cutter dulling will make tons of work later. And I have no way of modifying a cutter in house. Don't trust local cutter grinders to get me a cutter that cuts on all flutes. Their history doesn't warrant it.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
3/8 diameter x 6 flute.... Two passes down the middle to get root width of .130 then a pass on both sides to get the angle.

Just trying to get a view/idea of the tool.

QT OP[Don't trust local cutter grinders to get me a cutter that cuts on all flutes.]

If you could sketch the part or cutter you might give Special Drill and Reamer In Michigan a call.

They were my main source back when I was ordering /designing special cutters.

Have a sketch of the part feature or the cutter that you can fax, so not wasting their time.
(248) 588-5333

QT op *[MSC has one in stock but it is $223 ] you might reference that tool/cutter so everyone knows what will work.
 

guythatbrews

Cast Iron
Joined
Dec 14, 2017
Location
MO, USA
Shaping worked fine

Parts are done now. The shaping worked great.

I could have saved about 45 minutes using a square end mill. A lot of attention and extra programming time required with this method to blend the 30 degree side walls with the floor of the cut and the parts maybe not quite so nice. Cutters of course cheap.

Could have saved about 1.25 hours using a 60 degree included angle end mill with .130 minor diameter. Cutters were $130 each minimum 3 pcs so $390 total.

Used a topnotch ntp3r insert ground to .130 tip flat at a cost of $130 for holder and insert and about a half hour to grind.

So shaping was the way to go for 150 pcs with last time I ran the parts over 5 years ago. The topnotch insert will hang in there for maybe 1000 pcs I think.

Maybe someday will run big enough qty to justify a custom milling cutter.

Thanks for all the ideas!
 








 
Top