What's new
What's new

Narrow slot roughing tactics

Cole2534

Diamond
Joined
Sep 10, 2010
Location
Oklahoma City, OK
I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.

Would you guys HEM this with an undersized tool, run it traditionally with an 1/8" rougher, or something else?

The job was priced with a traditional slow movin path in mind so if that's the best way Im covered but I feel like there's a more efficient method.

Thanks, Cole

Sent from my SM-G973U using Tapatalk
 
What about drilling the bulk of material out with a drill about .010 under then come back with a 3MM make a roughing then finish pass?

I hate those small deep slots, Not so much they are difficult they just take too long.
 
I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.

Not much of a 304 machinist, but I have a project with a 1" diameter, .125" wide, .125" deep slot in 17-4PH. The bigger challenge is that I need .5" of tool stick-out to get to the top of the feature.

Went with the Helical HEV-C, a 5 flute chipbreak rougher and it worked amazingly well. Plugged my cut into the Helical Milling Advisor and ran the book numbers (4k something RPM, 8IPM). Worked beautifully! The chip breakers really make keeping the slot clear, which is just about the most critical thing to all this.

Same Milling Advisor says your parameters would be 7460rpm at 24IPM taking that slot in .125" deep passes. I would pre-drill and plunge between levels (my setup chattered like the dickens on helical entry, so I drilled a hair undersize and plunged slowly between passes).

The Harvey is a great tool!
 
At +.01" tolerance I would use a .125" tool, with 3/8 LOC and a TiAlN coating or similar, and a slight corner radius ideally (.01 to .015"). Drill a start hole, then enter that and go around .021" at a time. Make sure you slowly plunge into the last couple of depth to cut your way in. Make darn sure you are getting the chips out. If my math's right this would end up being around 20 minutes of cutting.

I'd be afraid of breaking drills off in the part and being screwed so I wouldn't feel great about chain-drilling, personally.

If you have the power and rigidity, I wonder how a shop-made trepanning tool might do.
 
I don't like chain drilling, but a 3mm cutter followed by a 1/8" is a good idea.

I spoke with Helical and they suggested the HEV series. I think that's what I'll try.

As for coolant, I'll be using Trim 690xt at about 10% concentration and doing whatever I can to clear the chips. Now I understand the desire for servo driven coolant nozzles.

Sent from my SM-G973U using Tapatalk
 
Iscar EC-E7 2 millimeter seven flute end mill, you will not find a better tool, go for a trochoidal path and chances you break it are slim to none. You'll save time with predrilling yes.
 
I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.

Would you guys HEM this with an undersized tool, run it traditionally with an 1/8" rougher, or something else?

The job was priced with a traditional slow movin path in mind so if that's the best way Im covered but I feel like there's a more efficient method.

Thanks, Cole

Sent from my SM-G973U using Tapatalk

.
1) usually dont use same size end mill as the slot that is usually rough slot leave material on sides and bottom then take finish cut to improve surface finish and slot size consistency
.
2) 304 usually have short tool life and sudden tool failure rate is higher. usually have to be cautious about not damaging the part. little end mills in 304SS often dont finish long slot like that. i wouldn't be going 24ipm feed either. going by tool history data on 1000's of previous jobs. obviously part cost and risk of part damage from sudden tool failure need to be considered
.
3) often roughing end mill has chamfered corners for longer tool life and the finish end mill has smaller corner chamfers to make a more square corner slot. usually square corner end mill dont last very long roughing in 304SS
.
4) tool stick out length problem most important factor. usually stickout length over 3 dia and especially over 4 dia tool flex can be a problem. .125 dia that 0.5 stickout is very long length. .093dia end mill thats .36 stickout is long
 
I might consider plunge cutting with the 3mm, or even a 3/32 mill.
Drill a start hole, and then switch to the mill and just program a "bolt hole pattern" with like 100 or whatnot holes in it - so that you are only taking .06 (?) at a time.
That would seem to be the strongest use of the tool and the programming would be almost a one liner!


----------------------

Think Snow Eh!
Ox
 
I would also stay away from chain drilling. I rode that wild bull once. Thought I could get a 8 second ride and ended up on the arena floor spitting poop out of my mouth.

Ox's idea has some good legs with a tool that is happy end cutting. Do you have TSC? Not sure if the Guhring Diver is available in 3mm but with TSC that could be mint.

I would also be keen to go with a ramp down play



I have no earthly idea why I made a rodeo themed post.
 
Last edited:
I would also stay away from chain drilling. I rode that wild bull once. Thought I could get a 8 second ride and ended up on the area floor spitting poop out of my mouth.

Ox's idea has some good legs with a tool that is happy end cutting. Do you have TSC? Not sure if the Guhring Diver is available in 3mm but with TSC that could be mint.

I would also be keen to go with a ramp down play



I have no earthly idea why I made a rodeo themed post.
Me neither, but yee haw.

Sent from my SM-G973U using Tapatalk
 
I might consider plunge cutting with the 3mm, or even a 3/32 mill.
Drill a start hole, and then switch to the mill and just program a "bolt hole pattern" with like 100 or whatnot holes in it - so that you are only taking .06 (?) at a time.
That would seem to be the strongest use of the tool and the programming would be almost a one liner!


----------------------

Think Snow Eh!
Ox
Yeah, that idea could be meritable. And yes the code would be only one line if you wanted :D (G16 G91 Y3.6 K100)
 
I have nothing of value to add....

Buuutt... 1/8" is a big tool at current job! Now 'roughing' a .010"x.030" deep slot with an .007" endmill is where it's at LoL

aluminum though... :leaving:
I'll see myself out hehe :stirthepot:
 
High Feed Mill

I would ramp in quickly with a high feed endmill like above, may need to relieve the shank a little to get that deep.

Hardplates, you're my man. I like this approach a LOT. It keeps the coding simple for my old VMC and with its .120" diameter it's a perfect roughing tool.

Thank you!

I emailed Carl at Lakeshore to see what he recommends for speed/feed/DOC, I'll reply with his suggestions.
 








 
Back
Top