What's new
What's new

Light cuts in 304 stainless

gehodgin3

Plastic
Joined
May 11, 2015
I'm machining 304 stainless plates that are 12mm thick and I have to remove .6mm step from the corners (kind of like a pocket) that is 38mm x 75.5mm. I keep burning the corners off my cutters every 3 or 4 parts. I'm using 5/8 carbide endmills with 7 flutes, 3/4" loc and ALTiCrN coating.

SFM 325
IPT .001
RPM 1986
FEED 350
Flood Coolant

Any help would be greatly appreciated
 
I'm assuming your programming your feed in mm per minute?

Sent from my Moto G (5) Plus using Tapatalk
 
I'm suspecting RPM too high and feed too low, but I'd also use a 1/2" cutter for this job unless I was making a lot of them and had to optimize the process.

How are you holding the cutter and the workpiece, and on what machine? A few pictures would help.
 
Machinability of 304 plate can vary quite a bit.

We do a lot of sheetmetal (many parts in this thickness range) and some of them require machining. There's one job that repeats every so often and it is either a piece of cake, or bitch. We use a facemill (45° lead) to mill a wide shallow slot. Batch of 20-25 parts usually.

Sometimes we do the whole job rotating inserts twice. Sometimes we have to rotate inserts every. single. part. 304 sucks. Played with speed and feeds a whole lot without much effect on that part. Seems to me it can depend on the material mostly.


Your feed is probably a bit slow, but SFM isn't anything crazy. Might be a little much if you are using very large step-over.
Could double or triple the feed at least, maybe more depending on machine and rigidity of setup. Try lowering your SFM and upping the feed.
 
I like to have a roughing and finishing endmill when I’m machining difficult materials. Maybe leave .05 mm on the floor and walls for the finish tool.
 
Yes we are programming in mm per minute. I'm holding a 5/8" endmill that is 3" total length and 3/4" flute length with an er32 collet in a Cat50 holder. The parts are machined on a fixture that is blocked up off the table due to the fact that they get 2 ports and 4 through holes. We use the 5/8" endmill to machine the ports as well as slots on the parts. There is a roughing op and a finishing op, both with 5/8" endmills. The roughing op is done with 5/8" endmill with a .06/in radius. Here lately I've been running anywhere from 16 to 40 parts a week on a JohnFord DMC 2100. As far as machinability, 304 is so aggravating to machine because the 300 series stainless has the highest tolerance of chromium and nickel. This is why one batch of parts cuts like butter and the next is impossible to machine. I am using about a 60% stepover. I was running the feed at 500mm per minute but was also spattering endmills. I have ran this part at slower speeds and feeds with great success but was taking way to long (almost 3x as long). I just got some different endmills with a nARCo coating hoping this will make a difference as well. I will get some pics when I get back tomorrow. Thanks for all the advice so far.
 
I just got some different endmills with a nARCo coating hoping this will make a difference as well. I will get some pics when I get back tomorrow. Thanks for all the advice so far.

That's a high-temp coating, might be worth trying it at higher speeds and feeds but with an air blast, no coolant. Just for the facing, if the hole making is working OK with current parameters stick with them.
 
I'm machining 304 stainless plates that are 12mm thick and I have to remove .6mm step from the corners (kind of like a pocket) that is 38mm x 75.5mm. I keep burning the corners off my cutters every 3 or 4 parts. I'm using 5/8 carbide endmills with 7 flutes, 3/4" loc and ALTiCrN coating.

SFM 325
IPT .001
RPM 1986
FEED 350
Flood Coolant

Any help would be greatly appreciated

I acutally think your parameter are off and you are rubbing instead of cutting. Im using YG V7 plusA endmill and their 6 flutes line suggest the follwing number.

SFM 348
IPT 0.0024
RPM 2127
IPM 20.77
Flood coolant.

Stainless is a pain and will eat your tool if you don't feed hard enought.
 
Me, I'd call Imco endmills and get their recommendations. They've never steered me wrong in the past, working on some decidedly "tough stuff" Plus, they're really good endmills. I use them exclusively on hard / tough stuff daily.
 








 
Back
Top