Need help with machining a part

gear cutter · Mar 29, 2014

I am having trouble machining some parts from 304SS. The part is 1.062 OD X 2.06 inches long. I need to machine a bore .875 ID X 1.875 deep with a boss at the bottom of the bore at the bore center. The boss is .280 OD X .437 long. I have drilled and bored to the finish ID up to the face of the boss. Then i have tried to mill the material away around the ID of the bore and the OD of the boss. I am not doing something right here. All I am doing is breaking endmills. I am machining the parts on a Okuma Genos L 200 M with live tooling. The endmills are accupro .250 OD with .500 flute length and factory relieved shank. I have 100 of these to do. Any help would really be appreciated. Thank you. Tim

reedeprintice · Mar 29, 2014

A video of what is going on would do it justice . How much are you taking per cut ?

Atomkinder · Mar 29, 2014

Are you milling this groove? Seems a long-ish way to stick and end mill down along the bore. I would try something like a facing groove tool first (not necessarily this one, just an example): Grooving Tools | MSCDirect.com

AARONT · Mar 29, 2014

feeds, speeds, doc, are the endmills coated/uncoated, how many flutes? Try starting around 150sfm and .001 chipload.

gear cutter · Mar 29, 2014

I do not have a way to get a video. Sorry. I have tried taking from .06 to .125 so far.

michiganbuck · Mar 29, 2014

Feed, speed, chip load per tooth, direction of cut, ridged holding of part and set-up, quality of holding cutter, rotation direction of cutter, quality sharpening of cutter, chip load and removal of chips, cutter bumping other than part, coolant missing job, chatter or vibration, spindle bad, bump in rapid, program error, decimal point wrong.

gear cutter · Mar 29, 2014

AARONT said:
feeds, speeds, doc, are the endmills coated/uncoated, how many flutes? Try starting around 150sfm and .001 chipload.

4 flutes, carbide, .03 corner radius, coating is AITiN.

gear cutter · Mar 29, 2014

michiganbuck said:
Feed, speed, chip load per tooth, direction of cut, ridged holding of part and set-up, quality of holding cutter, rotation direction of cutter, quality sharpening of cutter, chip load and removal of chips, cutter bumping other than part, coolant missing job, chatter or vibration, spindle bad.

150 SFM 3IPM. Ihave tried to cut that by 50% no luck. Part is rigid, holding flush with soft jaws.

NodecoMachine · Mar 29, 2014

Increase ur feed a bit and make sure there's plenty of coolant. I imagine it's making plenty of noise at what you are feeding now.

wheels17 · Mar 29, 2014

A custom cutter styled after a rotabroach? .875 endmill with the center missing.

Akzle · Mar 29, 2014

cant drill a blind hole and use bar stock for the boss?
How deep are you trying to go? Instead of doing the full .437, do more passes at .1 or .05, whatever is going to work.?

ostie01 · Mar 29, 2014

Instead of milling, Just remove most of the material by plunging with your end mill.

Just take a finish pass after that.

Your end mill break because all the chips get stuck at the bottom.

Jeff

gear cutter · Mar 29, 2014

NodecoMachine said:
Increase ur feed a bit and make sure there's plenty of coolant. I imagine it's making plenty of noise at what you are feeding now.

Didn't work. A lot of noise yes. Then SNAP.

gear cutter · Mar 29, 2014

ostie01 said:
Instead of milling, Just remove most of the material by plunging with your end mill.

Just take a finish pass after that.

Your end mill break because all the chips get stuck at the bottom.

Jeff

I have thought about drilling holes around the boss and then milling. The only problem is I only have 1 live tool holder to work with.

gear cutter · Mar 29, 2014

Akzle said:
cant drill a blind hole and use bar stock for the boss?
How deep are you trying to go? Instead of doing the full .437, do more passes at .1 or .05, whatever is going to work.?

Customer said no. They want the part machined from one solid piece.

MK Proto · Mar 29, 2014

Can you helical ramp it down at 2-5 degrees (c rotation), on the center line the come back and do the same thing for the od of the boss and the id of the part. Get coolant in there to flush out the chips.

Cuda · Mar 29, 2014

wheels17 said:
A custom cutter styled after a rotabroach? .875 endmill with the center missing.

I like that idea! Iscar may make a face grooving tool to do it, sometimes if I'm in a hurry and need to just get it done I'll go old school for short run jobs like this and get out a chunk of HSS and make my own grooving tool, run it at 20 FPM with coolant and it works fine if you know how to properly grind it.

ostie01 · Mar 29, 2014

gear cutter said:
I have thought about drilling holes around the boss and then milling. The only problem is I only have 1 live tool holder to work with.

Just drill with your end mill and finish with the same end mill

Jeff

michiganbuck · Mar 29, 2014

Any chance the end mill shank above the cut is interfering with part side or pinching chips between cutter shank and part side? Perhaps .030 reduced diameter shank above flute length.

You said...
"The endmills are accupro .250 OD with .500 flute length and factory relieved shank" That sounds like you should be clearing any shank problem.

*or coolant pressure or direction of coolant not flushing out chips.

David Carlisi · Mar 29, 2014

Try using a .75 annular cutter to get some of the meat out of there.

Need help with machining a part

Cast Iron

Stainless

Titanium

Stainless

Cast Iron

Diamond

Cast Iron

Cast Iron

Cast Iron

Stainless

Aluminum

Cast Iron

Cast Iron

Cast Iron

Cast Iron

Hot Rolled

Hot Rolled

Cast Iron

Diamond

Stainless

Similar threads