2mm radius corners in 1.75 deep pocket milling strategy help

So I have a part that will be 7075 aluminum and has quite the deep pocket. The pocket is over 3” deep but it’s a through hole and the only way I can figure I can do it is half from each side. So from each side I will have to go 1.75” deep. The pocket has 2mm radi on the corners and is about 3/8 tall by 1” wide. I was thinking of drilling the corners out but now I’m thinking I will drill a hole to plunge a 1/4 tool in do as much as I can then come back with a 5/32 endmill and finish the walls and corners with small stepdowns all the way.

Is this how you would do it? Or would you try to predrill the corners with the right drill?
Give me your suggestions on how to do this cost effectively.


Now the caveats. I’m limited to 3 axis and 7000rpm. I would also like to keep cycle time reasonable and avoid breaking the endmills. I’ve found them both from Melin and Harvey and they are $40 a pop. Also need to hold better than .004 on this. This needs a time effective strategy as I need 150 parts.


Also I have normally just done chamfers or used a corner rounding endmill but I don’t have one needed for this part can a 3D contour with a ball nose produce a decent radius quickly?

Would you recommend Harvey tool or Melin? I can get the Melin shipped for the price of the Harvey before shipping $39 for a 5/32 stub flute extended reach 3flute 1.875 reach endmill.

I think I would broach it. Send it out if you have to. That will be way too fiddly with a 5/32" endmill at nearly 10xD. If you can't do that for some reason, definitely drill the corners first. Then I might look to drill a 5/16" hole through and use a larger endmill (1/4" ish) to rough everything in and finish the majority. Then set up a shaping tool in the spindle and nip the corners. Does your spindle have a rotation lock?

That's not a pocket, at 3/8x1 over 3" thru.. That's a rectangular hole..

If it wasn't a ton of them, and you had a wire EDM kicking around, maybe
that would be the way to go..

But 175... Broach.. You can probably have one made for fat money..

Or you can "redneck" it.. I'd probably get it sort of close with a
5/16 or a 1/4" endmill.. Then I'd make a broach to finish it out.

Its aluminum, so you can take a decent size bite per tooth, granted its
not as easy as with 6061, but you can still take a heck of a bite in 7075.

Tool steel if thats your thing.. I'd make it out of 17-4 since I have a bunch
of it, and I can heat treat it in house easily...

You could even make a broach bushing, and then make your broach out of some HSS
blanks, take out one corner, or one end at a time... I've done that before in
hardened 4140 (35C) and been reasonably successful.

Another "redneck" solution, shape it right on the VMC... YES, use your VMC as
a shaper, I've done it..

I think almost anything would be quicker and cheaper than trying to mill it, that's
going to be a bitch and a half.. Getting it to blend nicely from both sides isn't
going to be the easiest thing either.

Even if you have to fab up a broach to take a cleanup pass, 3" is a long push and you want to remove as much as you can in any way possible. I think you're going to have to flip the part. To accurately locate it when flipped, you need a finished pocket for some depth on the first side so that you can make a centering pilot fixture that you can dial in on so you know for sure where the bottom of the partially finished pocket is.

I think I'd try drilling and reaming the corners first. Drill out most of the center mass with a couple of larger drills. Then mill the pocket down to 1/2 or 3/4 inch depth to finish if you can, you want to shorten the broach depth and chip load as much as possible. If you can finish mill the pockets on both sides to 3/4" depth, then you've only got to push the broach through an inch and a half of material, which is conceivable. Still need to make a broach as long as a keyway broach though, quite an undertaking in itself. But with the radius corners already done, you should only have a little ramp to remove from 8 locations near each corner.

I'd ask the engineer if all this fuss is worthwhile or whether he could redesign the thing with full radius ends to the slot.

Ooh, you are going to have quite the fun on these parts with 7k RPM . I passed on the job, and I have 16k RPM.

Broach would be nice, but expensive for the shape required. It's more complex than just a rectangle. Predrill, then have at it with a 10xD 5/32" neck-relieved Harvey.

The other part has all sorts of little fillets that you are going to have to 3D contour anyway, so might as well just suck it up and 3D contour the partial corner rounds.

It's gonna take a helluva long time at 7k RPM.

Regards.

Mike

Finegrain said:

Ooh, you are going to have quite the fun on these parts with 7k RPM [emoji5]. I passed on the job, and I have 16k RPM.

Broach would be nice, but expensive for the shape required. It's more complex than just a rectangle. Predrill, then have at it with a 10xD 5/32" neck-relieved Harvey.

The other part has all sorts of little fillets that you are going to have to 3D contour anyway, so might as well just suck it up and 3D contour the partial corner rounds.

It's gonna take a helluva long time at 7k RPM.

Regards.

Mike

Click to expand...

Haha yea well I haven’t quite taken it yet. The other part is easy enough to 3D contour. But you are right it will be a lot of contouring. My only saving grace is that these will be bead blasted. So I might be able to get a little more step over in and still have them come out good.

Because of the shape the only way I’m getting a broach is if I make it myself otherwise it would make the job not worthwhile. And I don’t think I could make it myself.


For blending there are slots that come down through the part and one in the middle so there is no problem there.

I guess I’ll be talking to the customer about changing it see if I can get 1/8 in the corners. If I could get that how doable do you guys think it would be?

In the end these parts are a nightmare to machine and I could make them much cheaper and presumably still function the same purpose but it’s about what the customer wants right? Not what I want to machine.



Edit forgot to mention.
Recommended speeds and feeds from Harvey actually put me at right around 7000rpm for that tool as in 7075 they want 250sfpm. Unless I read the chart wrong but I think that’s right. Now the 3D contouring is another story I’d be using 16k if I had it.

Ianagos said:

Edit forgot to mention.
Recommended speeds and feeds from Harvey actually put me at right around 7000rpm for that tool as in 7075 they want 250sfpm. Unless I read the chart wrong but I think that’s right. Now the 3D contouring is another story I’d be using 16k if I had it.

Click to expand...

I have no idea why they would recommend such a low SFM, even if it is 7075. I run a 1/2" EM at 16k in 7075, and it cuts beautifully and lasts a long time.

Chatter is a whole 'nuther ballgame though, and that is one area where running 10xD is going to take some trial and error.

Regards.

Mike

Ianagos said:

I guess I’ll be talking to the customer about changing it see if I can get 1/8 in the corners. If I could get that how doable do you guys think it would be?

Click to expand...

Better, but then the mating part will have larger partial corner rounds that need more time to 3D contour.

Regards.

Mike

Finegrain said:

Better, but then the mating part will have larger partial corner rounds that need more time to 3D contour.

Regards.

Mike

Click to expand...

Very true no winning with this part I see why you passed. Oh well I think I can make the part just not easy. I may give the broach idea some more thought. Just making a broach isn’t something I’ve ever done before.

Hi lanagos:
From what you're describing, these would take under 20 minutes apiece on a wire EDM if you can accept one pass precision and finish (+/- 0.002" and 32 microinch).
Do you think you can mill them faster?
Is it worth it to you to do all the screwing around necessary to make them on the mill?

Slotting them with a broach on an old fashioned keyseater will be by far the fastest; at a guess under 5 minutes apiece, certainly under 10 minutes apiece but you need to be able to get the broach through first, so you'd have to knock enough of the meat out to get a broach in and eat the cost of the broach.

Sinker or wire EDM cutting them will require the lowest upfront cost if you already have the machine.

Milling will give the shittiest outcome and might well be the slowest too.
Milling might not even be possible.

If you can mill them at a price competitive to the wire you'd get $6000.00 for the job.
Your call if it's worth the risk of taking it on and not being able to complete the job for 6 grand.

I'd be looking to farm it out if at all possible, and if not I'd quote for the risk and hassle factor.

Treating the mill like a CNC shaper as others have said also works, but you'd have to make the tool and it's hard on the spindle bearings if you get too cocky with your DOC.

Have them wire cut and save yourself lots of pain!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

implmex said:

Hi lanagos:
From what you're describing, these would take under 20 minutes apiece on a wire EDM if you can accept one pass precision and finish (+/- 0.002" and 32 microinch).
Do you think you can mill them faster?
Is it worth it to you to do all the screwing around necessary to make them on the mill?

Slotting them with a broach on an old fashioned keyseater will be by far the fastest; at a guess under 5 minutes apiece, certainly under 10 minutes apiece but you need to be able to get the broach through first, so you'd have to knock enough of the meat out to get a broach in and eat the cost of the broach.

Sinker or wire EDM cutting them will require the lowest upfront cost if you already have the machine.

Milling will give the shittiest outcome and might well be the slowest too.
Milling might not even be possible.

If you can mill them at a price competitive to the wire you'd get $6000.00 for the job.
Your call if it's worth the risk of taking it on and not being able to complete the job for 6 grand.

I'd be looking to farm it out if at all possible, and if not I'd quote for the risk and hassle factor.

Treating the mill like a CNC shaper as others have said also works, but you'd have to make the tool and it's hard on the spindle bearings if you get too cocky with your DOC.

Have them wire cut and save yourself lots of pain!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Click to expand...

If I could wire them I would but I don’t have an edm. If I take the job on I’ll get a few quotes from wire guys but there are other features that are not conducive to wire so if I pay 6k to get the wire done I won’t have much left to pay for my time and machine for the rest of the parts. Gonna have to get a quote on a broach it seems. I may try making one from 4340 or something of the nature and mill out with a 1/4 tool then run the broach through to clean up the corners.

Anybody have any insight on broach design? Or can make one in 3 days haha?

Hi again lanagos:
Making a broach:
First you have to decide if you're going to make a multi-tooth broach or a shaper cutter: the two require some significant differences in your approach.
Second, if it's a broach is it a push broach or a pull broach?

For the width to length ratio of the slot, it's not a broach in my opinion, but a glorified keyway cutter and the mill will be used like a shaper.
So you need room in the slot to get the cutter down and it needs to be enough room so the cutter has some stiffness since it's cantilevered out from one end and will just bend or break if you make it too skinny.

To make it you need to mill it out of a hardenable tool steel like A-2 or S-7 and then harden it and finish the cutting edges with a grinder or a slip stone.
Alternatively you can grind or wire cut it from a hardened blank.

Next you need to decide if your cutter will travel diagonally into each corner in turn or if it will traverse the length of the slot and cut two corners at each pass.
Obviously the cutter design will be unique to the strategy you choose.

Designing the shape is a bit tricky since you need to minimize the forces that will want to push the tool tip sideways when you make each cut.
Your top rake (or front rake) will govern that to a significant extent...too little and it will bend back out of the cut and snap; too much and it will dig in and snap.
The top rake determination is kind of empirical; a common starting point is 5 degrees.
Everything else on the cutter requires clearance and 5 degrees is a pretty good starting place for that too.
Remember that ideally, the cutter will have room to back away from the cutting face a few thou on each back stroke.
Remember also it needs to be as stiff as you can make it which means short and wide.
Thin is OK so long as it's WIDE (just like a parting blade on the lathe)

Next you need to program it; lots of hand coding here.

Last is to make a holder, set it all up and clench your sphincter as you push the big green button for the first time.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

So I milled a test part today and it worked out fine but now I need to get faster with the 3D contouring.

As of now I’m using 2 flute and 3 flute ball nose endmills. But do you guys think a 4flute Kyocera ball nose (it’s 5/32 if that matters)
With a high polish will let me run some faster feeds since I am limited in rpm?

Also will be running some long tools would set screw holders be recommended? As of right now I use almost exclusively collet holders.

Hi lanagos:
Glad to hear you were able to mill them after all; so all my hand wringing turned out to be just so much bullshit as is often the case when you solicit free opinions on the internet on how to do something.

So here's yet another opinion:
With the ball cutters, the four fluters will theoretically let you jack up the feed rate and preserve the chipload per tooth, but in aluminum that's not usually what limits you; it's the finish you hope to get.
In the real world, my experience is you can get way better time gains by increasing the size of the stepover than you can by jacking the feedrate to the max for the spindle speed you've got.

The cutter geometry will limit how much you can push it; go above an upper chipload limit and the finish turns to crap, because at the microscopic level there is always one flute hanging down a micron or two more than the others, so it's really actually a one flute cutter, not the four flute cutter you're thinking it is.

So absent the ability to run up the spindle speed, you can maximize your finish quality by minimizing the cutter runout, and by increasing the ball cutter diameter to the max that can run the job, so you can jack up the stepover to the max.

Part of minimizing runout is excellent toolholding; in my free opinion on the internet, setscrew type holders are not excellent...they're piss-poor.

This goes double in my opinion for long stickouts: you want short flutes, as big a shank diameter as possible, (even if you have to buy die-mold cutters with tapered shanks) and a solid circumferential grip which means no general purpose ER collets; you want dedicated collet sizes closely matched to your shank diameters so the grip is as close to circumferential as possible.
Shrink fit holders are another good option; the chatter resisting abilities of the circumferential grip are well known; that's why you can see them getting away with some outrageous stickouts on 5 axis work...they spent lavishly on great tool holding and it's often shrink fit.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

That sounds like something coming from Xometry...

implmex said:

Hi lanagos:
Glad to hear you were able to mill them after all; so all my hand wringing turned out to be just so much bullshit as is often the case when you solicit free opinions on the internet on how to do something.

So here's yet another opinion:
With the ball cutters, the four fluters will theoretically let you jack up the feed rate and preserve the chipload per tooth, but in aluminum that's not usually what limits you; it's the finish you hope to get.
In the real world, my experience is you can get way better time gains by increasing the size of the stepover than you can by jacking the feedrate to the max for the spindle speed you've got.

The cutter geometry will limit how much you can push it; go above an upper chipload limit and the finish turns to crap, because at the microscopic level there is always one flute hanging down a micron or two more than the others, so it's really actually a one flute cutter, not the four flute cutter you're thinking it is.

So absent the ability to run up the spindle speed, you can maximize your finish quality by minimizing the cutter runout, and by increasing the ball cutter diameter to the max that can run the job, so you can jack up the stepover to the max.

Part of minimizing runout is excellent toolholding; in my free opinion on the internet, setscrew type holders are not excellent...they're piss-poor.

This goes double in my opinion for long stickouts: you want short flutes, as big a shank diameter as possible, (even if you have to buy die-mold cutters with tapered shanks) and a solid circumferential grip which means no general purpose ER collets; you want dedicated collet sizes closely matched to your shank diameters so the grip is as close to circumferential as possible.
Shrink fit holders are another good option; the chatter resisting abilities of the circumferential grip are well known; that's why you can see them getting away with some outrageous stickouts on 5 axis work...they spent lavishly on great tool holding and it's often shrink fit.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

Click to expand...

I use sized collets and actually ordered some tecknics high precision collets for the job.
I get that with the flutes there is a threshold I can only increase the stepover so much until the step over gets too much and also ruins the finish.

It’s all a compromise of what I can do. I’ll just have to experiment and see what I can get away with I bought a bunch of different cutters. I always do that for a job then I end up just using one and the rest sit.

Shrink fit is not in the budget as I would have to buy a shrinking machine and what not.


I don’t know what xometry is but it’s not that.


Some of the cutters I bought were 3 flute designed for stainless and metals like that so hopefully the work ok in 7075. For my test part I necked back a tool myself so if I have to I’ll just neck back aluminum specific tools myself.