Help milling stainless

[Leigh @ Kodiak]

We have some pieces of 304 stainless with a flame cut profile that is prooving to be quite the challange. To make matters worse, a crappy flamecut left as little as .062" extra stock on the profile at the top of the profile, and as much as .25" extra at the bottom.

 

I am using an Iscar 1.25" 90deg mill, and we have a choice of IC328 inserts, or IC928 inserts. I have already tried many combinations of speed, feed, and depth of cut, all of which work OK, but the tool life is not great at all.

 

Any recommendations anybody might have are very much welcome. We need to find the right ballance between cycle time and tool life here, and I am having a tough time!!

[crazy^millman]

Switch over to a 3/4 carbide varamill run 3/4 depth of cut .004 per tooth chip load at 220 sfm dry with plenty of air. You can run it wet just increase the feed by 10%. If you are running inserts had you tried them dry???

 

HTH

[Leigh @ Kodiak]

unfortunately we don't have time to wait for special carbide endmills to get here. We are already running our inserts dry, with air

[MultiAxGod]

It's the flame cut what made em hard. You won;t get a combination that will give you good tool life because of this. The money saved for the cheaper flame cut has now cost you in inserts, so the company didn't save a penny and the parts will probably cost more overall now to make. If you have to do more, get them waterjet cut. No material distortion, case hardening, jagged edges, etc. Tool life will increase dramatically.

Good Luck. I hate flame cut material. It should only be used for +/- a football field, finish cut, farm parts.

[Andy]

We also find that flamecut materials work great for jobs you dont have to machine!

[crazy^millman]

quote:

---

special carbide endmills

---

Standard off the shelf endmills. You can keep wasting inserts and time or get a tool that will do the job and do it quick and efficient that if your choice, but if you are running it dry and getting these results you would be better getting a 2" corncob rougher and taking it in one pass at about 3 to 5 imp at about 200 rpms than your current method. It some purchasing guys is making decisions about getting good carbide endmills to do the job have them price out a corncob rougher they are now about $150 to $200. They run slower and take more time costing more money so where do you save and how do you get ahead staying with something that is not working at is going to keep giving you the same results???

[strabe]

I agree totally with Multiax. Nothing you do is going to help much from here on out. It might get a little better where there's more material but who knows? I would definitely get the boss over to see the expense related to trying to machine flame cut material so the same mistake isn't made again. Sorry for the bleak outlook.

 

Good luck.

 

Ken

[jbrooks]

Try conventional milling instead of climb milling. That may help. Jeff

[bhyde]

I used to cut flame cut 304ss and we used high speed roughers and didn't climb..Conventional cut seemed to help with tool life. Don't know if this will help with inserted tooling but made a huge difference on hss.

 

Bill

[produca2]

I was having a similar problem with stainless steel recently. I was using .125 "precision ground" blanks saw cut into 8"x8" squares. I was making oval shaped thru-pockets with a 6 flute AL-TiN coated 1/4in endmill. My first run of 10 parts went O.k. with a spindle speed of 6061rpm's, and a feed rate of like 23 ipm. Like I said 10 parts went o.k., minor issue with tool life.... About a month later I was asked to change the configuration of the holes, and went right back to work with the same speeds and feeds on the same kind of material, and was breaking endmills after the first plunge started into into its toolpath! I got it to where it would do 1 or two pockets perfectly and then randomly break the e.m. again!--- ??? So tried al kinds of configurations of feed and speed with nothing working AT ALL! And after breaking 27 endmills at 32.00 each I was done wasting money.I eventually had to crank my spindle down to like 735rpm with a 1.7ipm feed rate and the same tool has cut 10 parts front and back.....but it takes all day to finish 1part I have no idea what happened where, and I am just grateful that I am in a prototype/individual part making position and not on a time is money time table!

[Matthew Hajicek - Singularity]

Produca2, my guess would be that something is different about the material. Could it be a different hardness?

[produca2]

I ordered the same material I ordered the first time, and that did cross my mind. I was wondering if the "precision gringing" process caused the hardness to be inconsistent between each piece of material. I would think not, but I cant seem to find any rhyme or reason for that peticular scenario!

[Guest]

+ a million to conventional cut.

other than that large cut slow and easy may be

the only way to make time in this??

it will take patience.

 

ds

[Leigh @ Kodiak]

STATUS REPORT

We had the Iscar rep come in and take a look at things, and he provided us with a new tool that has tangentaly mounted inserts, using their new "SUMO CUT" 805 grade...

 

Everything is looking ok so far on our test cuts, but we had to avoid the inside corner radius's( radii?) and pick them out later with another tool.

 

Will report back later after we are done the run, but our current parameters we are using are .39" deep, .08 radial cuts, at 1000 RPM, and 35IPM. I did ask the rep about conventional milling, but he said it's not such a great idea in stainless....something to do with the gumminess of the material.