1/32" End Mill

[Travis_Buchanan]

I'm trying to mill a pocket roughly .33" deep with .015 radius in corners.  I roughed leaving .002 on the walls with a 3/6", then roughed with a 1/6" leaving .001 on the walls.

 

The 1/32" end mill is a 3-flute with 3/8" of cutting length. https://www.mscdirect.com/product/details/62778147

 

With the 1/32" I am cutting .005 deep, 22k rpm, 20imp, about .0003 fpt.  I keep popping these end mills like crazy.  Only the 1/32" ones.

 

Any advise?  

[Colin Gilchrist]

A couple things come to mind:

1. MSC sucks for supplying good quality tools. They say "Accupro" on that listing, but who knows where the tool really came from. When you buy tools this small, it is really important (and difficult) to grind the proper rake and clearance angles into the flutes. I used to get some .01 diameter endmills, and would have to inspect them under a microscope. I would reject 2 out of 3, because I could visually see that the grind was crap.
2. Driving any long tool into a corner where the corner radius = tool radius is a recipe for disaster. 20 IPM IN THE CORNER? No way, no how. You are going to need to slow down about .02-.03 before you hit the corner. I wouldn't be going into that corner faster than 1-2 IPM. Then you can accelerate back out of the corner.
3. .005 deep with a .032 diameter cutter is just wasting time. I'd step down .03 per pass. (You are only taking .001 on the wall, with a .032 tool)
4. Have you thought about a .03 diameter Endmill? That would allow you to swing a .001 arc in the corner. (what kind of tolerance do you have on that .015 CR? Can you get away with a .002 cutting radius, using a .03 diameter tool?
5. Get a Harvey Tool (.03 diameter, .375 flute length) for this:  http://www.harveytool.com/prod/Square-Miniature-End-Mills/Miniature-End-Mills/Browse-Our-Products_255/Miniature-End-Mills----Square-Long-Flute_52.aspx

Good luck!

[Colin Gilchrist]

Another thought would be to drill the corners out with a .032 Carbide Drill, prior to cutting the pocket. That would help immensely. I say Carbide Drill, because it will produce a much straighter hole...

http://www.harveytool.com/prod/Miniature-Drills/Holemaking---Threading/Browse-Our-Products_275/Miniature-High-Performance-Drills---Aluminum-Alloys_260.aspx

[Travis_Buchanan]

Thanks for the replies, the corner radius is actually .5mm or .0197"  After inspecting the part it looks like the endmills are breaking when they hit the floor of the pocket. I am going to add a thou or so to the tool length and keep it off the floor.  It is worth a shot.  I will keep your tooling recommendations in mind for the next time, I just got to get this part out the door now. 

[Guest]

Also, check tool runout. Even .0005" will give you troubles on a tool that small. 

[gcode]

I've never tried dynamic milling with a tool this small, but I have used dynamic paths in titanium using a 1/16" end

to clear out corners with excellent results. I would think dynamic milling would work equally well with 1/32" tools

[nickbe10]

I think Colin et al covered just about everything I can think of. Harvey is a good company, excellent and consistent quality. Another one to look at is Mikron, they also do great thru coolant small drills.

[Colin Gilchrist]

1 hour ago, nickbe10 said:

I think Colin et al covered just about everything I can think of. Harvey is a good company, excellent and consistent quality. Another one to look at is Mikron, they also do great thru coolant small drills.

+1000!  Mikron makes great stuff. I really like their Crazy Drill line of products too.

[nickbe10]

37 minutes ago, Colin Gilchrist said:

I really like their Crazy Drill line of products too.

Have you tried the Crazy Drill Cross Pilot? Its worth watching the vid on the site.....totally outrageous. We do our wirelock holes with these, drill on the angle from both sides with the pilot and then a Crazy drill cool to join the dots, up  to 12D deep in Inconel and 15-5. We reduced our time from 5 min to 10 seconds.......including tool change. Watching the thru coolant shoot through the bottom when it breaks out at 11 - 16 ipm with a .047 - .075 diameter drill never gets old.... 

[Oppiz]

Have spoke to the engineer of the part?  Possibly that small of a radius isn't necessary and was over looked in the design.  I run into that quite often.

[Travis_Buchanan]

LOL, I did talk to the designer of the part, he bumped the radii up to .5mm up from .25mm.  Acted like I was a sub par machinist/programmer for not wanting to do .25mm radii in the corners at .33" deep.  I think run out is my major issue, I'm going to tool this up in heat shrink next.

[Colin Gilchrist]

You could always broach it I suppose. Engineers these days are spoiled by additive manufacturing. Soon undercut, square corners, will be the norm...

Like G-Code mentioned, Dynamic would probably work pretty sweet on this. You can get a .03 Endmill with .375 of flute length. I'd do a .006 stepover, leaving .001 for finish, and then run a full depth finish pass, stepping over .0006, and make a few passes on the wall to size.

For my geometry, I'd take the wireframe, and break it about .05 from the corner. That way you can use "Change at Point" to slow the cutter down before the corner, and speed it up after the corner is cut...

Do you have a 5X machine? The other option is a very small Tapered Ball endmill, and tilting the part to get some clearance. Then you can just surface machine the material left in the corners. Harvey has a .015 diameter Ball endmill, with a tapered neck. You'd need about 10 degrees of clearance to pull it off. But then you can give him a .01 corner radius, no problem. (Could even do .008 CR...)

[crazy^millman]

2 hours ago, Colin Gilchrist said:

Do you have a 5X machine? The other option is a very small Tapered Ball endmill, and tilting the part to get some clearance. Then you can just surface machine the material left in the corners. Harvey has a .015 diameter Ball endmill, with a tapered neck. You'd need about 10 degrees of clearance to pull it off. But then you can give him a .01 corner radius, no problem. (Could even do .008 CR...)

Colin he works for Onsurd Routers so I will go out on a limb and say yes he has access to a 5 Axis machine.

[Travis_Buchanan]

I am cutting this part on a 5ax machine.

I dialed in a tool/holder and now have about .0003 runout.  I'm ashamed to tell you what it started out at.  I am using an extension so it takes a little work to get it dialed in.

I am going to try this part again on Monday.  I have not had a lot of experience with tooling this small, so I'm learning, just like every other day

[Leon82]

You may want to try a stub flute long reach endmill.  Harvey has a wide selection

[JMahon]

I do this fairly regularly... I'd try to slow the sfm to around 100-150 and .0001-.0002" per flute feed.