Chris, 6061 is very gummy in the annealed state. Try to get your stock in the T6 condition. In T6, it cuts a lot like 2024, provided you don't heat it so much that you anneal it.
Your question asked for speeds and feeds for carbide. My experience is that there is so much surface heating with carbide, that you can do as well with high speed steel. Especially since you only have mist coolant. Try 320 sfm at (30*dia) ipm as a start. Depths of .5*dia to 1.5*dia. for roughing. In most applications, a two flute mill will work best. It has more clearance to get the chips away from the cut. If the chips impact, they will fuse and break the cutter or spoil the part. Four flute cutters are OK for light side milling or shallow end milling, where there is no danger of impacting the chips. If working with rolled stock, try to take the same amount of material from each side. To minimize warpage, you may have to rough both sides of the part, reflatten the blank, then finish. If maximum strength is required, you should re-heat treat the part after roughing. Leaving a .010 web to hold the part together works fine. I've done it many times. Best results are obtained if the last cut on the last side is at least .050 deep. This way you have .060 holding until the last 1/2 diameter, and you can reduce the feed there. Some cutter manufacturers offer end mills especially ground for aluminum. They have sharper edges and higher relief angles. They cut a lot better than general purpose end mills, and last longer. The greater relief angles are necessary for higher feed rates. At high feed rates, standard mills may drag the heel of the cutter and overheat the material. Galling will occur. Also, the heat treatment of the material will be changed. Gene Bowen ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
