single pass on 304SS 5/16 thick

[dingo0722]

I am profile cutting a small part with an outside profile of about 6 inches. The material is 304SS. I have all the drilling and chamfering of the part down but am struggling with cutting the part out of the stock. Currently I am drilling all the features into the stock plate. Then I secure the part each piece prior to cutting out with screws through the drilled holes into a board below. I am profile cutting the part out using 1/4" HSS 2 flute running at 1300 RPM and a feed of 1.25ipm with 4 passes. I am getting tooling failure after cutting out 6 pieces. The stock material hold 11 pieces. I am entering each part off the stock material and side cutting the whole time. I was thinking of going with a roughing endmill to pick up the pace, do a single pass cut and hoping to get the tool to last longer. Is this possible? any help and thoughts would be much appreciated

-Dan

[metalworkz]

Hi Dan,
Do you think the material is work hardening?

[dingo0722]

I have run into that. I have found that running a carbide endmill I could never get the speed and feed correct which caused the part to work harden and destroy the tool.
with the HSS, the tool will cut for a while then rapidly fail. I suspect this is a speed/feed issue that I just haven't been able to figure out.

[xclr82xtc]

make several passes, and chnage the code so that every few passes it changes the z to use a lil different spot on the tool

[dingo0722]

I changed the code so the tool starts off the part in stead of plunging on the part. This made a big difference but still getting premature tool failure(premature as far as I am concerned)

[Shane123]

use a niagra fine tooth roughing endmill, leave about .01 on your xy surfaces, then come around and clean that with your carbide. the cheaper fine tooth roughers have larger teeth than the niagra, hence why i suggest using niagra brand if possible. if you have clearance, use a 1" or 3/4" diameter rougher, seems to last longer. 99% of our work is stainless, and i finally got the purchasing staff to order 303 whenever possible to save on tooling. 304 is soooo inconsistent on plate. use a 4 flute finisher if possible, keep your chip load down.

[Shane123]

if you do go with the niagra, speed of around 750 for either of the 2 recommended diameter cutters. feed of 5 - 6 ipm, your tool will let you know what it likes.

[jamesu229]

Check out how we run 17-4 stainless. these cutters should do well slotting in 304 also

YouTube- HIGH SPEED MACHINING(REALLY HIGH!!!)

[djr76]

Originally Posted by Shane123 use a niagra fine tooth roughing endmill, leave about .01 on your xy surfaces, then come around and clean that with your carbide. the cheaper fine tooth roughers have larger teeth than the niagra, hence why i suggest using niagra brand if possible. if you have clearance, use a 1" or 3/4" diameter rougher, seems to last longer. 99% of our work is stainless, and i finally got the purchasing staff to order 303 whenever possible to save on tooling. 304 is soooo inconsistent on plate. use a 4 flute finisher if possible, keep your chip load down.

what this guy said,

1 pass for rough, 1 pass for finish and flood the crap out of it to cool and flush chips. Id go with a .500 rougher since you will be able to run it faster than a .75 - 1.00 diameter endmill and finish it with a .250 carbide.

[Shane123]

Originally Posted by djr76 what this guy said, 1 pass for rough, 1 pass for finish and flood the crap out of it to cool and flush chips. Id go with a .500 rougher since you will be able to run it faster than a .75 - 1.00 diameter endmill and finish it with a .250 carbide.

havent had the best luck with .5 diameter, what speed/feed you running? i know the .75 and 1.0 will do full radius cuts fairly easily, but the .5 seems to wear itself out on me. i must be running it too hard or not hard enough.

[djr76]

Originally Posted by Shane123 havent had the best luck with .5 diameter, what speed/feed you running? i know the .75 and 1.0 will do full radius cuts fairly easily, but the .5 seems to wear itself out on me. i must be running it too hard or not hard enough.

I run 304 on the slower side. For hss fine tooth roughers, 30-50 sfm .001-.002 ipt. with flood coolant. So for .500 diameter hss rougher, 350 rpm is a good starting point.

[dingo0722]

Originally Posted by djr76 I run 304 on the slower side. For hss fine tooth roughers, 30-50 sfm .001-.002 ipt. with flood coolant. So for .500 diameter hss rougher, 350 rpm is a good starting point.

350 RPM. I am way above that and that could be my problem. I am running around 1200 at 2.5IPM. I have some 3/8 Colbalt roughing endmills on order I will give them a shot at a lower RPM and same feed which will be with in your 0.001 to 0.002 parameters for a 4 flute