[rustyolddo]

Most of my work is aluminum at depths less then the cutters DOC. I've got job to machine from 304 stainless. It's simple enough, a square pocket .1875" corner radius. It has to be machined through a 1.75" thick block of stock. I plan to rough it out with a .75" or 1" EM then go back with (a) finish pass(es) to clean it up. I'll have to use a .250" EM to get the corners clean & chatter free.

First question, what is SOP when cutting pockets, slotting etc. greater than the tools DOC?

Is it ok/normal if the shank rubs the part? Or are reduced shank EM's mandatory?

I could machine to the tools DOC then step over and continue until I reach the finished depth which will leave the pocket stair stepped. Doesn't solve the problem with the finish pass.

I could also pre-drill the corners with a little offset which would leave less material to remove with the .250" EM.

I could machine the part from one side then flip it, and machine from the other side, at least for roughing, I'd have to finish it without flipping to avoid mismatch error.

Simple everyday operation for most folks, but it's bugging me.

[Cmailco]

Most of my work is aluminum at depths less then the cutters DOC. I've got job to machine from 304 stainless. It's simple enough, a square pocket .1875" corner radius. It has to be machined through a 1.75" thick block of stock. I plan to rough it out with a .75" or 1" EM then go back with (a) finish pass(es) to clean it up. I'll have to use a .250" EM to get the corners clean & chatter free.

First question, what is SOP when cutting pockets, slotting etc. greater than the tools DOC?

Is it ok/normal if the shank rubs the part? Or are reduced shank EM's mandatory?

I could machine to the tools DOC then step over and continue until I reach the finished depth which will leave the pocket stair stepped. Doesn't solve the problem with the finish pass.

I could also pre-drill the corners with a little offset which would leave less material to remove with the .250" EM.

I could machine the part from one side then flip it, and machine from the other side, at least for roughing, I'd have to finish it without flipping to avoid mismatch error.

Simple everyday operation for most folks, but it's bugging me.

Ok, the fastest way to do this might not be feasible because I don't know your tooling situation and what you have at your disposal. Lots of variations on this though:

1. Use a hi-feed mill and ramp-pocket the whole thing.

Like I said, lots of variations dependent on the size of the pocket and tooling. You could just ramp-pocket, but the width of the pocket needs to be such that the tool covers the pocket without leftover stock in the center.

In a case where leftover stock is unavoidable, pre-drill (inserted drill) or helical interp the center slug out, then proceed with ramp-pocketing routine.

Once the pocket is roughed, mill the corners out with a relieved end mill. It needs to "reach" 1.75" but we sure as hell don't want or need that much flute length. There is a specific technique for doing this, called "slicing" but whether or not you can do it is dependent on your CAM software... or whether or not you HAVE CAM software. I cover this technique very briefly at my blog but you can probably find a bit more information on the web, if you look for it. Basically, we need to "rest mill" the corners out.

Rest mill far enough from the corners so that the finishing tool doesn't hit the corner. In other words, if you want to use a 3/4" end mill, you will want to rest mill back from the corner at least 3/8"... I typically add another .025" for insurance.

1. Ramp-pocket with or without center clean-out
2. Rest mill the corners
3. Finish the walls

I don't particularly like working with 304, it can be a bit of a challenge because it's gummy. TiAlN coatings sure do help though, and making sure you take finish passes that are deep enough to get below the work hardened layers from previous passes.

edit: By the way, the corner cleanout can be done a number of ways: 1) Use a 1/2" first, then go in with the 1/4", 7mm, etc.. 2) skip the 1/2", use a standard length 1/4" first, then switch to relieved 1-3/4" reach tool or 3) use combination of 1 & 2.

Best regards,
Chuck

[rustyolddo]

Thanks for the input. Very! informative blog as well, I skimmed it and will go back and read further. I use OneCNC that has HSM tool paths & rest machining and this will be done in a VMC. If I understand you correctly, using a reduced shank EM for the finish operation would be the key.

[Cmailco]

Sorry for the late reply Rusty, somehow I missed this post on my last trip through.

To answer your question: Yes, use a reduced shank tool for the corners with 3-4 flutes, variable helix, .015-.02 radius; your typical grind hi-performance end mill specifically designed with stainless work in mind. Using a variable helix type will allow you to get the corner radius with a 5/16-3/8 diameter tool and that gets you into 'stocked' tooling from Destiny Tool. They have a variable helix 4 flute (DVH4240815RC) that fits the bill nicely: 3/8", 1/2" LOC, 1-7/8" reach, 4" overall length, with a .015-.02 corner radius. At near 5:1 length/diameter, you may have to reduce the feed & speed by 15-20% but this should make for a nice quick cornering process either way.

DESTINY TOOL - online cataloge and shop

Frank is a great guy to deal with. Really knows his tools well; they're his designs. I'd go with whatever he recommends, might even steer you more towards the 3/6 (6-flute) they offer since you have good tool engagement angle control within your CAM system.

Good luck,
Chuck

[universalfab]

If your work hardening the material your failing and it happends to the best of us from time to time. If your messing around with dull endmills or endmills your don't know are sharp enough, get a new one. Stainless is expensive to work with. It eats up alot of tools, it takes longer to machine, and the material itself is fairly expensive. Your going to want much lower feeds and speeds for stainless the aluminum, work hardening happens when your rpms are to high and your feed is to low. It also depends on your machine, rigidity is a must.