endmill for 3/16 1018 profile

[timmydabull]

looking for a good endmill in the 3/16 size for profiling 3/16 thick 1018,also some reccomended feeds and speeds.

havent had much luck with sandvick 3 flute garr 3 flute or fullerton 4 flute.

tried runing .0012 chipload and tools wont last long.

any help would be appreciated.

thank you
tim

[HuFlungDung]

Can you rough with something larger so that the 3/16 does not have so much to cut?

Are you currently roughing full diameter full depth in one pass?

There are several possible scenarios that might help out, but if you are breaking tools consistently, it is not likely to be the tools' fault.

[timmydabull]

i have the parts nested so that 3/16 is the largest tool that will pass in between parts.

1018 is .1875 thich and i have tried .090 depth of cut and .060 depth of cut with no success.

roughing with a bigger tool may certainly take the stress off the small cutter i didnt think about that.

im pretty sure its not the tools fault.lol

please let me know what you reccomend.

thank you
tim

[HuFlungDung]

Endmills under 1/4" are not great for roughing because of a strength deficiency. Frankly, I'd re-nest the parts at about .28" minimum seperation so you can rough without damaging surfaces that need to be finished later. But that is just opinion.

I'd then look for stub length serrated roughing endmill, 1/4" or 6 mm dia. C1018 can be a bit gummy, and a serrated tool will help break up the chip. One place I know of to check is at maritool.com and look in the roughers area. They have them down to 1/8" but my gut tells me you don't use the teeny weeny ones unless someone forces you to do so

Use a good airblast to clear the chips out of the groove to avoid recutting. If you are not running super fast, you could use coolant, I suppose but at the risk of premature edge cracking, especially in deep grooving situations, it is very difficult to predict how continuous the coolant flow is in the cut. TiAln coatings can stand heat quite well anyways, so I'd try air blast first.

Leave a thin joining skin at the bottom of the initial roughed grooves so the parts stay in position, then go in with your 3/16 and profile each side of the groove to finish the parts off.

[timmydabull]

i will take your reccomendation.

thank you very much

tim

[OKUMAN]

I have very good sucess with the Iscar Finishred EM.Very strong em.I would say you could run about 2500 RPM with a feed of somewhere in the range of 12-15 IPM @ full depth.

[timmydabull]

Originally Posted by OKUMAN I have very good sucess with the Iscar Finishred EM.Very strong em.I would say you could run about 2500 RPM with a feed of somewhere in the range of 12-15 IPM @ full depth.

thank you for the speed and feed reccomendation

tim

[timmydabull]

roughed with 1/4 variable helix rougher and finished with 5 flute finisher.

both at .200 depth of cut and 2500 rpm at 12 inches a minute.

harmonics are great and finish is WOW

thank you working mint

tim

[timmydabull]

thank you guys for the advice on this job.

really made a big difference.
tim