Milling deep narrow pocket in stainless. Tool suggestions?

Tichy · Sep 27, 2019

I'm milling a 24mm*10mm*71mm xyz pocket in 304 (or as we Swedes call it 2333.) Last time around was a disaster. Now I need to make 150 of them. (Or to be exact, just 8 of those, then the others are a bit wider pockets (12 and up) and a little easier.)

What's my best option? Any suggestions welcome. We'll obviously buy the tools needed, or I will scream and /ragequit.

Rick Finsta · Sep 27, 2019

I'll take a shot. I'd use a high feed mill to rough it, and come back with a 5-flute to finish the floor and walls; probably something with a stubby flute length and reduced neck.

Biggest problem I've had with pockets like that is getting the chips out.

Finegrain · Sep 27, 2019

I would drill/ream the ends of the slot, so that whatever endmill you end up using isn't getting buried at each end of the cut. That actually gets you most of the 24mm width already. After that I guess I would just step down with first a normal, then a necked endmill. Pull up a few thousandths short of each of the slot ends.

Regards.

Mike

Tichy · Sep 27, 2019

Rick Finsta said:
I'll take a shot. I'd use a high feed mill to rough it, and come back with a 5-flute to finish the floor and walls; probably something with a stubby flute length and reduced neck.

Biggest problem I've had with pockets like that is getting the chips out.

I may have been unclear. It's a hole. Straight thru the bit so no pocket. Could you link me to a suitable high feed mill with 10mm or less diameter? I find jack squat.

Finegrain said:
I would drill/ream the ends of the slot, so that whatever endmill you end up using isn't getting buried at each end of the cut. That actually gets you most of the 24mm width already. After that I guess I would just step down with first a normal, then a necked endmill. Pull up a few thousandths short of each of the slot ends.

Regards.

Mike

What I created was this:

1, predrill 10mm holes at end of slot as you suggested to half length.

2, solid carbide rougher to open up the same.

3, turn part. Make customized material stop to angle position it (with a plateau that goes into the pocket.

4, repeat steps 1,2 for other side.

5, finish cut.

I'm set with the material stop. (using a 4 jaw chuck.)

However I can't find a 10mm mill (or less, my preference would be going trochoidal/skimming) with that reach. We don't have one.

By the way the 10mm slot is new. The previous order the smallest was 12.

The thought about normal+necked seems good. I'll just have to research the options. I'm taking time with the strategy on this, I know we'll make lots.

Is my logic sound?

Mtndew · Sep 27, 2019

Tichy said:
Could you link me to a suitable high feed mill with 10mm or less diameter? I find jack squat.

Garr Series H45 high feed end mills, I've used them before with excellent results.
They also offer metric for you backwards people

GARR TOOL - Search Results

G00 Proto · Sep 27, 2019

I think you would be way money ahead to water jet that feature.

MattiJ · Sep 27, 2019

Water jet or wire edm comes to my mind also if the hole is so deep that you need to mill it from both sides.

Extra long reduced neck 3/8" = 9,5mm end mill?
Helical Solutions - 4 Flute, Square - Variable Pitch, Reduced Neck
Enough reach even from one side but I have feeling that these need some babying..

Toms Wheels · Sep 27, 2019

Does the part need to be made from solid?? Mill 24 x 71 x 10 groove, couple minutes. Driil tap some holes to fit a cover.

Rick Finsta · Sep 28, 2019

Seco 10mm x 70mm:
980TL100-MEGA | Secotools.com

We've used their inserted high feeds (down to 3/4" diameter) and they rip.

That said, if it is straight through I'd also probably get quotes for water jet, or do it in a 4th axis from both sides. The high feed will not leave a nice wall finish (in fact it will look really bad LOL) so you would need to leave stock for a cleanup pass around the periphery.

pablo.casiano75 · Sep 28, 2019

Are the pockets close to each other? Thin walls in between? If you have thin walls in between yeah it can be tough. I had a part like that before and ended up using a thin wall pocket feature that mills .050 at a time as a depth of cut and got a very nice finish on the walls with no tapper. I believe I left no more than .050 on the sides so it has something to cut as it spiraled around to the final depth. Leaving too little causes issues also. But yeah the posts everyone shared are good options too. 5fl endmills is the way to go.

Sent from my iPhone using Tapatalk

chowming · Sep 29, 2019

So if I'm hearing this right your making a thru slot .3937 wide .9449 long 2.7953 deep.
Lay out the edges on the top of the part drill a 5/16 hole at starting end. Use a carbide 5/16 5 flute endmill (5 flute for the center mass of the endmill) move over a 1/32 or 1/16 and plunge thru. So you'll be cutting cressent moon steps. Repeat the copping step all the way to the end. Now you have a5/16 slot thru in the right place. Now ith a shorter 5/16 end mill cut the slot shape and remove the peaks or the un even Ness left by the copping process. Switch to a longer endmill and clean up the lower part. Stay like .01 to .005 a side small during clean up walls process (you could flip it over and dial in the lower and use a shorter endmill). Then finish it from one side or from both sides.

Sent from my SM-N950U using Tapatalk

Edit typos (it's hard typing on this phone)

Tichy · Apr 1, 2020

Rick Finsta said:
Seco 10mm x 70mm:
980TL100-MEGA | Secotools.com

We've used their inserted high feeds (down to 3/4" diameter) and they rip.

That said, if it is straight through I'd also probably get quotes for water jet, or do it in a 4th axis from both sides. The high feed will not leave a nice wall finish (in fact it will look really bad LOL) so you would need to leave stock for a cleanup pass around the periphery.

Love that tool spec. I'll try to sell it to management next round of these. Seco's expensive but hell they make quality sh*t.

dian · Apr 2, 2020

first time i hear about 5-fluted endmills. what is the advantage? center mass? you mean a thicker core as compared to a 6-fluter?

Milland · Apr 2, 2020

Tichy said:
Love that tool spec. I'll try to sell it to management next round of these. Seco's expensive but hell they make quality sh*t.

Could you clarify something? When you said "pocket" in your first post, it implied a flat bottomed, five-sided feature (i.e. not a through hole). But a lot of people suggested though approaches (waterjet, wire EDM).

So which is it, with a bottom or through? Very different methods to take dependent on that.

TeachMePlease · Apr 2, 2020

Milland said:
Could you clarify something? When you said "pocket" in your first post, it implied a flat bottomed, five-sided feature (i.e. not a through hole). But a lot of people suggested though approaches (waterjet, wire EDM).

So which is it, with a bottom or through? Very different methods to take dependent on that.

Check post #4. He clarified it's a through slot, not a pocket.

Milland · Apr 2, 2020

TeachMePlease said:
Check post #4. He clarified it's a through slot, not a pocket.

Thanks, hadn't noticed that.

gbent · Apr 2, 2020

Tolerance? Surface finish? Drill a starter hole and finish it with a shaper. Could also walk it lengthwise plunging with an end mill.

Search

Largest Manufacturing Technology Community on the Web

Search

Milling deep narrow pocket in stainless. Tool suggestions?

Tichy

Aluminum

Rick Finsta

Stainless

Finegrain

Diamond

Tichy

Aluminum

Mtndew

Diamond

G00 Proto

Hot Rolled

MattiJ

Titanium

Toms Wheels

Titanium

Rick Finsta

Stainless

pablo.casiano75

Aluminum

chowming

Plastic

Tichy

Aluminum

dian

Titanium

Milland

Diamond

TeachMePlease

Diamond

Milland

Diamond

gbent

Diamond

Similar threads