I need advise milling Haynes 230 and 233

[laminar-flow]

We have a project to mill some round pockets in some Haynes 230 and 233. We managed to get one completed using a .1875 Ø 5 flute carbide end mill for steel and although we managed to get a part, the end mill was suffering and basically ruined.

On the .1875 Ø end mill we were running 50 SFM, spiraling in and circling out with a .020 radial depth of cut, .025 axial depth of cut, .001 chip, and 5 ipm. Does that sound about right? We are not in a hurry so we could slow it down if needed.

If there are recommended end mills, I'd like to know what they are and where to get them.

Thanks for looking.

 

[Milland]

Dry, coolant, MQL? What machine, how short was the tool in the holder? I'd plan on using a tool for each pocket, use the preceding tool to rough, finish with new tool, which becomes the new rougher.

At least 3/16" cutters are dirt-cheap. But you could try checking out hard-milling specialty cutters to see if they're better for your needs.

 

[D Nelson]

Are you using dynamic tool paths? At full depth of cut?
Don


Sent from my iPhone using Tapatalk Pro

 

[laminar-flow]

Haas TM1, flood coolant, end mill held in ER16 collet quite short. Pocket is about 1"Ø and .230 deep. We were spiraling in with shallow depths of .025. Figured that if we spiraled to full depth and then took a full length of cut, it would not allow a big enough chip to get under the hard material. Round piece held tight in a Northfield air chuck so that is quite rigid.

 

[plastikdreams]

Rough with an end mill with radiused corners then finish with a square end mill. Haynes will rip the sharp corners of a square endmill off very quickly.

 

[laminar-flow]

We need a bit of a radii on the end so no points. Speeds and feed look OK? How about the other parameters?

 

[D Nelson]

Haas TM1, flood coolant, end mill held in ER16 collet quite short. Pocket is about 1"Ø and .230 deep. We were spiraling in with shallow depths of .025. Figured that if we spiraled to full depth and then took a full length of cut, it would not allow a big enough chip to get under the hard material. Round piece held tight in a Northfield air chuck so that is quite rigid.

.025 is not a shallow cut for a .1875 Endmill ramping in to hard materials try .005 per loop then dynamic maybe 5 percent step over maybe 4 percent step over. That’s what I would try. descent rpms and feed
Don


Sent from my iPhone using Tapatalk Pro

 

[laminar-flow]

We were cutting 0.020" radial depth of cut, so you are recommending 0.005" Radial depth of cut? I thought that would be too much into the hard layer from the previous pass but hey, I'll try it. What about each level?

 

[plastikdreams]

The key is not getting the material hot, air blast is highly recommended, also good coating. AlTiN does very well with niCrWMo superalloys and is still cost effective. I'd go with a 20-25k depth and step over 5-10k. With 1.000 size I'd be looking at .500 cutters or bigger, variable flute as well.

Airblast keeps the chips out, cools the cutter, and doesn't create thermal shock. With these materials chip evacuation is key recutting chips will destroy cutters.

Spiral down to your depth and helical cut to your finish, -.010 then do a ramped finish. You should be able to step over .030-.050 on your rough. I'd feed 5-10 ipm and 3500-4000 rpm. Then adjust from there.

I recently did a .500 deep open ended slot in custom superalloy, it was .5625 wide and 1.000 long, I used a .500 cutter with air blast with a little koolmist, .050 depth cuts then a full depth pass .038 radial on either side with a spring pass...hand cranked on a Bridgeport. You should be fine on a tm1.

 

[laminar-flow]

Ok, just bought some 1/4" 4FL SINGLE END STUB LENGTH HARMON-I-CUT CARBIDE END MILL .020" CORNER RADII from northbaycuttingtools.

Getting the blanks ready on the lathe today. I'll be milling them Mondayish.

Disk is 1.375 Ø and .3 thick. Pocket is .880Ø and .250" deep.

Thanks for all the help everyone and any more ideas would be appreciated.

 

[plastikdreams]

Ok, just bought some 1/4" 4FL SINGLE END STUB LENGTH HARMON-I-CUT CARBIDE END MILL .020" CORNER RADII from northbaycuttingtools.

Getting the blanks ready on the lathe today. I'll be milling them Mondayish.

Disk is 1.375 Ø and .3 thick. Pocket is .880Ø and .250" deep.

Thanks for all the help everyone and any more ideas would be appreciated.

I would have gone much bigger on the end mill size...did you see my response?

 

[laminar-flow]

Yea, but a .500 end mill is quite costly and we have another project that we might end up needing a .250. We only have to make a few more parts out of this material.

 

[D Nelson]

If the price of a 1/2 inch Endmill bothers you your definitely in the wrong game
Don


Sent from my iPhone using Tapatalk Pro

 

[TeachMePlease]

Yea, but a .500 end mill is quite costly and we have another project that we might end up needing a .250. We only have to make a few more parts out of this material.

I bet one .5" endmill costs less than the machine time you waste messing around with a 1/4".... Or the 3x 1/4" you snap trying to get those last few parts out the door...

 

[laminar-flow]

Shucks, I used advise in stead of advice in the subject. To late to correct it.

 

[D Nelson]

I bet one .5" endmill costs less than the machine time you waste messing around with a 1/4".... Or the 3x 1/4" you snap trying to get those last few parts out the door...

Nobody thinks that far out. Running materials like that and worrying about Endmills is crazy.
Don


Sent from my iPhone using Tapatalk Pro

 

[plastikdreams]

If done right that .500 end mill will go on to other jobs. It's not rocket surgery, bigger end mill bigger cut, more contact area. I don't cut superalloy stuff every day but I work in a foundry that casts parts from it. Sometimes we have to mill it, it's tough stuff but done right it's not hard on cutters. For example, I put holes in .250 waspaloy plates. I use a .25 cutter and plunge straight down, usually 15 or 20 pieces one at a time. I still use that cutter on aluminum and steel with good results. Again on a Bridgeport, your speed and feed is critical or you will burn that cutter on the first plate. And it's a 3 flute square TiN coated only.

Right tool and right knowledge for the job...anyone can cut steel or stainless, when you step up to the big leagues you better have both or its gonna eat you alive.

That said, I'd still run that cutter to the bottom, step over .020-.03 on a helical interp. And finish with a tight ramp. Keep the cutter engaged, don't go in and out of the cut. And keep the chips out, I can't stress this enough.

 

[laminar-flow]

After retiring one .250 end mill on one part...

I put the blank in the Monarch used an old carbide end mill as firs an end mill to plow the hole in the middle, then used it as a boring bar and roughed out the pocket leaving about .020" on the surfaces. Then back in the Haas TM1 and finished with another new .250 end mill. Took about 10 min in the Monarch since I could really plow it out, and 25 min cycle in the Haas. The chip was increased to .0018 and used 60 SFM. The end mill held up for the rest of the 6 parts. The Haas with its ball linear ways lacked rigidity for this small job, but I rarely machine these nickel chrome alloys. A non ball way machine would be much better. Thanks for all the help.

 

[Mtndew]

Yea, but a .500 end mill is quite costly and we have another project that we might end up needing a .250. We only have to make a few more parts out of this material.

A 1/2" end mill is around $50 give or take from most manufacturers.
How much are you paying for yours?

 

[laminar-flow]

The ones I bought were short 4 flute for tough alloys. Also, the Haas would have made too much noise with a .5 end mill. Nice job and a good customer made happy.