Cutting a deep rectangular pocket...

[Spencer in NH]

I have a project where I need to cut a pocket about an inch deep with a .065 radius in the corners. The dimensions are .42 x .17-in.

If I use a 1/8-inch end mill, that's about an 8:1 length-to-diameter ratio. Not sure how to approach this. I need a surface finish of at least 32.

I suppose I can remove most of the material with a 5/32 endmill and then just deal with the corners.

The material is nominally 6061-T6. Machine has 10K RPM and is tight.

Any help would be appreciated.

Thanks.

 

[Kyle Smith]

One approach that works well is to buy the shortest length of flute endmill you can get and then relieve the diameter of the endmill by 0.005". You only cut with the first 0.050" or so anyway, this gives you the most rigid setup possible and removes all the side load.

Another option is EDM and polish.

 

[RJT]

Or use a CNC EDM, orbit and forget about polishing. It can be milled, but I would go as deep as I could with a standard end mill first, then use Kyles suggestion, using solid carbide tooling. Keep the chips out by using a small air blast of spraymister.

 

[Matt@RFR]

Harvey Tool PN 34708 should do what you need. I think I would swiss cheese the pocket with a 1/8" drill to within .005" of all four walls, then have at it with the Harvey endmill. Maybe leave .002" on the walls for a cleanup pass. You could also get a slightly smaller tool with the same reach and have a larger radius in the corners so you're sure it won't chatter there.

 

[Spencer in NH]

Thanks guys.

EDM is not an option here.

Matt, that Harvey Tool looks good. I'll give them a call.

I'm still open to ideas...

 

[Matt@RFR]

Matt, that Harvey Tool looks good. I'll give them a call.

Just in case you go that way, Lakeshore Carbide is a distributor for Harvey.

 

[Spencer in NH]

That's interesting. I thought Lakeshore made their own product.

 

[Matt@RFR]

They do, but they are also a Harvey distributor. Just trying to give you an easy way to buy if you use Lakeshore already.

 

[Heinz R. Putz]

If possible, I would get back to whoever designed this and explain to them the problems involved in doing a pocket like this with a really small corner radius.
Hopefully the guy that designed this had no idea how difficult and time consuming this is and he may not need the small corner radius.
If he still does. drill the corners to depth, use a little larger endmill to mill it down using a repeat sub, then use the small endmill to clean up the overlap in the corners.
I recently did this as part of a training job with a .125 radius about 1" deep on a pretty good size pocket, I got the designer to change it to a .1875 corner and it worked OK.
Good luck: Heinz.
Sorry that I do not have this example on my website, its a little too unusual, but there are lots of other good examples.
www.doccnc.com

 

[Rossco]

Deep pockets I normally plunge rough the corners out first then pocket. Then clean corners with smaller endmill.

 

[John Welden]

If you've got a relieved endmill, it should go fine, especially if you can program it with a HSM tool path.

Run the same speeds and feeds you would normally use, but take a light depth of cut.

 

[cmailco]

I've used the Hanita long-reach 2-flute 'Javelin' end mills for these types of jobs with good results. That said, there's not a lot to pick from when it comes to 'reach' type end mills in anything under 1/4" diameter, especially with non-ferrous geometry.

There are a number of ways you could machine this pocket, though none of them are that productive at 10k rpm. Working with what you've got, I'd start by drilling a 5/32" hole in the center of the pocket. Use the best (lowest TIR) holder you've got and drop the 1/8" tool in the pre-drilled hole.

If you can build a toolpath that maintains constant engagement angles ('morph', 'spiral' type toolpaths) then this whole thing is relatively easy. You can use .125-.250 axial, 20-10% radial respectively with a .085 radius in the corners to minimize the arc of engagement on corner entry. After pocketing to depth, you can either pick the corners out like... [ ] or pick them up as you finish the walls. Reduce corner feed by 30%. You don't need much wall finish in this type of pocket; .001-.002 is adequate and I'd finish those at z-levels just short of the flute length, say, .2" (to get a small overlap) or something divisible by the total depth.

Not the most descriptive process outline ever but you get the general idea.

Silly engineers and their pockets...

 

[Spencer in NH]

Great info! Will report back. This is a proto, but I'm afraid there's no alternative for redesign for technical reasons. This is a little chunk of microwave waveguide, and it's pretty constrained.

I'd tell the engineer what I think of his design, but I wander around talking to myself too much already.

Thank you for your wisdom.

 

[John Welden]

If you can build a toolpath that maintains constant engagement angles ('morph', 'spiral' type toolpaths) then this whole thing is relatively easy. You can use .125-.250 axial, 20-10% radial respectively with a .085 radius in the corners to minimize the arc of engagement on corner entry. After pocketing to depth, you can either pick the corners out like... [ ] or pick them up as you finish the walls. Reduce corner feed by 30%. You don't need much wall finish in this type of pocket; .001-.002 is adequate and I'd finish those at z-levels just short of the flute length, say, .2" (to get a small overlap) or something divisible by the total depth.

Are you sure about a .125 - .250 DOC with a 1/8th inch 2 flute endmill an inch deep?

 

[-Chris-]

deep pocket milling

I agree with all said a relived shank with a short flute length small depth cuts and try doing a finish pass at each depth cut you might be suprised at how good the finish will come out Chris