Realistic Feed and Speed for 304SS

Milling some 304SS blocks. I'm using a CNC Knee mill with a 4000 RPM 5 HP spindle. Tooling is 3/8 and 1/4 4 flute uncoated carbide in 3" GL ER20 Collet holders. HSM Advisor is telling me to cut at roughly 107 SFM and 8.3 IPM for facing (.375 EM, .25 WOC, .03 DOC) and 107 SFM and 23 IPM for adaptive clearing (.375 EM, .03 WOC, .25 DOC). The 1/4 I'm using to mill a .265 wide channel using proportionately scaled feeds and speeds.

Since HMS Advisor says these are the starting numbers, is this still a good ball park?

Jay Fleming said:

Milling some 304SS blocks. I'm using a CNC Knee mill with a 4000 RPM 5 HP spindle. Tooling is 3/8 and 1/4 4 flute uncoated carbide in 3" GL ER20 Collet holders. HSM Advisor is telling me to cut at roughly 107 SFM and 8.3 IPM for facing (.375 EM, .25 WOC, .03 DOC) and 107 SFM and 23 IPM for adaptive clearing (.375 EM, .03 WOC, .25 DOC). The 1/4 I'm using to mill a .265 wide channel using proportionately scaled feeds and speeds.

Since HMS Advisor says these are the starting numbers, is this still a good ball park?

Click to expand...

A little conservative IMO. Go for it. I would use a bigger Collet though ER20 is a little guy.

R

Seems like a very low SFM unless there are some complicating factors.

I just did a couple hundred 304 parts at 200 SFM, and got the whole batch done with one set of AlTiN-coated endmills.

Regards.

Mike

OK, I see you are using uncoated endmills. Why?

I second the uncoated comments, you want coated, makes a really big difference in tool life and the slicker coating really helps the cutting. Larger than ER20 would be good for the 3/8" tool, thats just fine though for the 1/4" tool. May wel lbe just fine though if thats all you need from the 3/8" tool DOC wise.

HSM tool paths can work really well in stainless, you will get way way better tool life too using more of the flute than your 30 thou.

Speed and feeds though in 304 are the crap shot, as material goes if frequently varies and whats fine in one part is way too much for another. It pays to be slower than fasster generally in 304 and with increasing speed, the difference between gaining speed and tool life can be a real cliff edge. even a small increase in RPM can take you from a nice long reliable tool life to failure with in a part. The sweet spot can be very narrow in this material.

That sounds pretty reasonable to start with given the uncoated tools and assuming you don't have good/any coolant given that it's a knee mill.

Jay Fleming said:

Milling some 304SS blocks. I'm using a CNC Knee mill with a 4000 RPM 5 HP spindle. Tooling is 3/8 and 1/4 4 flute uncoated carbide in 3" GL ER20 Collet holders. HSM Advisor is telling me to cut at roughly 107 SFM and 8.3 IPM for facing (.375 EM, .25 WOC, .03 DOC) and 107 SFM and 23 IPM for adaptive clearing (.375 EM, .03 WOC, .25 DOC). The 1/4 I'm using to mill a .265 wide channel using proportionately scaled feeds and speeds.

Since HMS Advisor says these are the starting numbers, is this still a good ball park?

Click to expand...

.
.
304 SS can vary depending if cold rolled or cold worked or if annealed with sfpm easily varying 200%.
.
length of tool sticking out of tool holder can easily effect tool life 200% or more and this influences max ipt feed and max DOC and or WOC
.
end mills with more corner radius are better for roughing out material and can easily last 200% longer. tool life with 304 is not unusual to be 20 minutes or less
.
coolant or some oil on surface can increase tool life easily 200%
.
some cheap steel has slag or hard spots in it. if hard spot big enough it will easily wipe out tooling in seconds. you can be milling ok then bam there goes the end mill