Reply with QuoteHi Dan,
Do you think the material is work hardening?
single pass on 304SS 5/16 thick
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
Similar Threads:
Hi Dan,
Do you think the material is work hardening?
Regards,
Wes
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.
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
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)
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.
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.
Check out how we run 17-4 stainless. these cutters should do well slotting in 304 also
[nomedia="http://www.youtube.com/watch?v=E3AqIZURMbI"]YouTube- HIGH SPEED MACHINING(REALLY HIGH!!!)[/nomedia]
Originally Posted by Shane123
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.
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
that is certainly your problem , you also need to uphold a heavier chip load or your going to burn up and dull your tool . for that type of material you would be best off using coated carbide endmills or better yet coated carbide variable flute end mills , you'd be able to run at much higher speeds and feeds with less tool wear and less deflection
A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........
I would love to run a carbide, but I find them so unforgiving. Its like go-nogo, and with the HSS/Cobalt I can dial them in. Maybe its just my junior statis running machines.
Dingo, after running this cut through G-Wizard, I came up with a couple of things to think about:
First, as others mentioned, your rpm is definitely wrong for an Cobalt (HP HSS in G-Wizard) cutter in this stainless. I wouldn't go as slow as 350, but about 900 rpm versus 1200 would be a lot better.
As a rule of thumb, if the cutters wear out too fast, its surface speed. If they break or chip, its too much feed (too much chipload). Although, see my note below about rubbing for an exception!
Second, as work hardening goes, the recommended feedrate at 900 rpm would be about 1 IPM, normally. This is with a 1/4" Cobalt endmill. However, that will vary due to chip thinning if you are cutting less than half your cutter diameter in terms of width of cut.
That brings me to my third point. On a 1/4" HSS endmill, with a 1" stickout from the tool holder, if you cut more than about 18 thou in that stainless, you will get more than a thou of tool deflection. That's heck on your cutter life too, especially for brittle carbide. If you're cutting more than that, the deflection may be contributing to your problems and even causing a little chatter.
But let's say your width of cut is actually 18 thou. That's well into chip thinning territory. Your real feedrate for a recommended chipload of 0.0005" actually needs to be 3.9 IPM and you were running about half that. With any material, this can lead to rubbing and more tool wear. With stainless, rubbing = work hardening. And most peeps think running less feed was babying the cutter.
Okay, last point. If you did all this with a 1/4" carbide, you should be running at 2900 rpm, 3.9 IPM at 166 thou width of cut. I don't know if you need that much or not. If less, you can pick up the pace. 80 thou width of cut and you can run nearly 7 IPM. The bigger cutters mentioned can be even more aggressive since they're much more rigid.
Cheers,
BW
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html
thanks for the worms! baby bird is hungry! honestly, great advice, im still wet behind the ears on milling and love to know all the tricks. i have some ss 303 i will need to mill full radial cuts, 1 1/2" depth total and 3/4 wide thru 2" round cylinder barrels for ears. i been using the 1/2 in niagra fine tooth with coating, going 1/4 in deep per pass. seems like when i tried to hollow it out with drills before hand, i would get weird results on the cutter when it broke thru, so i have been staying in the cut to remain predictable on wear. i might have to try less baby-ing and being more aggresive. thanks for the advice bro.
