milling question

[Rick46]

I have a electrode( 4 x 5 x 5 ) I need to cut. The center of it is a clearance pocket about 4 inches deep and roughly 3 x 3 square. I was told to day to use a 1 inch cob cutter to remove this center clearance area out of the graphite instead of using a .500 in diamond cutter at high speeds and feeds and fairly large depth of cut.

 

cutting recomendations for the cob cutter were about 1 inch deep 700 rpm's and maybe 40 inches a minute if it would take it..full stepovers as well of the cutter diameter.

 

what are thoughts on this, is this a good idea or bad.. electrode will be fixtured up with (4) 5/16 mounting screws and 4 dowel pins of 3/8 diameters..

[Leigh @ Kodiak]

If I was programing this, it would be the method that you prefer. I don't know what a chunk of graphite that size goes for, but I would be wary of breaking it.

 

Solid carbide would probably be fine to use if you don't plan on doing this type of work often.

[Rick46]

yeah its a one time deal set of 4 electrodes.. but Im worried of breaking the carbon myself.

[TR Mfg.]

Either way would probably work. With only 4 parts to do I wouldn’t use the cob cutter for fear of cracking the material.

[mold100]

corn cob in graphite, BWAAAAAAHAHAHA go with your method first cut depth like .02 to keep a sharp edge after that its on .25 - .300 DOC 7500 rpms 120 ipm to get it out of there, plunging with center cut endmill.

[MAKINOPAT]

No way would i use the corn cob going 1" deep. definately use the high speed method. It could easily break the graphite around the screws and throw the trode right off the fixture especially going that depth of cut and feed rate!

[shazam/TPP]

+1 mold100

[Rick46]

@ mold100 what are u recommending for a 3 or 4 flute ball endmill with 4 inches of flute with inches of length hanging out of a holder ?? speeds,feeds, stepovers, and depth of cuts.. im wanting to a prove a point to a co-worker and looking to get the best results possible just to see the look on the face of this guy no into the high speed machining processes..thanks a bunch..

[Rick46]

or even a 3/8 6 flute elat bottom with three inches of cut.I have those option of course the 3/8 would leave me stock to still remove from the botton of pocket but just curious of a good way of approaching this.. thanks and to anyone else that wants to chime in on this matter.. thanks again..

[mold100]

Rick U don't need a ball mill, I prefer a bullnose, but I run a little differant, I run a .25 bull nose with a .02 corner rad at 9200 rpms and 130. ipm with a .1 doc, 70% step over.

finish wall at each step down. This feeb I use and my cutter is in a shrink fit sticking out 2" in a HSK32 holder.

[Rick46]

oh I dont have and bullnose endmills.. just millstar inerts with 1/32 and 1/16 rads..from 1/2 up to 3/4 inch..the holders are mainly collet holders with a few solid ones HSK 63 series. I do have some solid carbide endmills and diamond coated endmills but no rads on them and our shrink fit system dosent work had a command shrink fit system but it no longer heats up and they want us to ship it to them so they can look at it but no gurantees and its like a thousand dollars do ship it there or something crazy.. I forget but it was up there.. I am pressing the issue for a new system so we can use our shrink holders once again.. love those things.lol.but back to the carbon basically all I have is diamond coated extended length ballnose up to 1/2 inch.. and regular length solid carbide with altin coating up to 3/4 inch.. then I already mentioned the millstar stuff..