[brento]

I am trying to cut 303 stainless steel using a 3/16 TiN HSS end mill. It is currently running at 1400 rpm, 11 ipm, 0.02 depth of cut. As can be seen, it is stepping the cut. Through a process of elimination, I believe this is being caused by the tool flexing. I am looking for advice on how to fix this problem, whether my rpm or ipm are wrong, and what is a reliable way to calculate these as I am entirely self taught, both in machining and CAD/CAM, and the learning curve is steep.
Thanks.

[DMF_TomB]

the most important factor when using a end mill is how long it is and how far it is sticking out of the collet
.
a 3/16 end mill sticking out 3/8" is 8 times more rigid than one sticking out 3/4"
.
basically if sticking out 3/4" the depth of cut is reduce by 1/4 and feed reduced by 1/2
.
the rule is 2x longer then it is 2x2x2= 8 times less rigid
3x longer then 3x3x3= 27 times less rigid

[brento]

The end mill is sticking out approximately 3/4 in. Does this mean I should be running at 5.5 ipm and 0.005 depth, but still at 1400 rpm?

[DMF_TomB]

The end mill is sticking out approximately 3/4 in. Does this mean I should be running at 5.5 ipm and 0.005 depth, but still at 1400 rpm?

3/16 dia end mill
2 flute ?
stickout length 3/4"
milling 303 SS with
machinabilty rating 0.78 cubic inches per minute per hp
70 sfpm
1426 rpm
max depth of cut 0.036"
max Feed 4.1 ipm
chip thickness 0.0015"
coolant ? cutting oil can help. chips can stick to cutting edge and to flutes or clogging flutes can put addition pressure on a end mill
rough power calculations
0.035 hp
0.028 cubic inches removed per minute
end force 7.6 lbs
torque 0.71 inch pounds
this is calculated 50% of maximum safe end force assuming no chip sticking or flutes clogging problems

[Delw]

what kinda machine are you using?
3/4 is too long but it will work. what brand endmill are you using, thats looks like crap. so either your machine is junk or your endmills are.

fake edit, just reread, your using HS endmills go with carbide 3/4" on a hs endmil in 3/16 dia is like stiring icecream with a 8" plastic straw

[brento]

Thank you, DMF tomB for the info. Those numbers were very similar to what I had calculated. Was running it at 5.5 ipm and broke the endmill. Will try your speed. Out of curiosity, how did you come to your ipm and depth calculation? Is there a better endmill type with a diameter between 1/8 and 3/16 when cutting 303 stainless steel, who is a good vendor and brand?

[Delw]

endmill brands to some are like the ford chevy argument

I only use GARR endmills and sometimes harvey tool endmills, garr makes a kick ass little 1/8 and 3/16 coated 4 flute carbide endmill that works great on 303 and 15-5ph.
I get all my endmills from the tool crib in phx az. and have been for 15+ years.

[DMF_TomB]

Thank you, DMF tomB for the info. Those numbers were very similar to what I had calculated. Was running it at 5.5 ipm and broke the endmill. Will try your speed. Out of curiosity, how did you come to your ipm and depth calculation? Is there a better endmill type with a diameter between 1/8 and 3/16 when cutting 303 stainless steel, who is a good vendor and brand?

i use an Excel spreadsheet that does the math. it also opens with the free Open Office Calc program. it takes info like
1) SFPM
2) diameter of flutes
3) number of flutes
4) machinability rating of metal being cut with examples given of common metal types.
5) Coolant use
6) End mill stickout length from collet
7) tool holder length
8) tool holder shank diameter
9) end mill shank material (carbide is stronger than steel)
10) end mill shank diameter ( important if shank dia smaller than flutes)
11) cutter efficiency, rough end mills and coated end mills need less hp to cut same amount of metal, examples are given
.
it takes the date and crunches the numbers, basically doing hundredths of mathematical formulas in a split second. the first 2 rows calculate end milling parameters on a constant hp load and 2nd on constant force load on end mill tip. these change based on machinability rating thus why you can take a higher depth of cut with aluminum compared to Stainless Steel
...3rd row is ball end milling
4th row is Side milling or high depth of cut and partial width of cut
.
Excel file is in a zip compress file / folder attached. it might seem complicated if you are new to machining. double check any suggestions with your own formulas and calculations.