tooling question

[CASTLEVILLE]

I have to cut a pocket 2.5in deep in some 6061 and I can't seem to get rid of the chatter. What endmill and speed and feed should I use? I am doing this on a bridgeport series 1 so I can only get to 4000 rpms on the spindle. Some of the corners have a radius of just over .5in so I can't go to big of a endmill dia. wise. I have tried a couple different endmills from .5 to .75dia 2flt and 4flt and 3in LOC HSS. Ran rpm's from 1500 to 3000 and feed from 7 to 20ipm. Nothing seems to work so any help will be much appreciated. If I didn't give enough info let me know.
Thanks Eric

[JDenyer232]

Originally Posted by CASTLEVILLE I have to cut a pocket 2.5in deep in some 6061 and I can't seem to get rid of the chatter. What endmill and speed and feed should I use? I am doing this on a bridgeport series 1 so I can only get to 4000 rpms on the spindle. Some of the corners have a radius of just over .5in so I can't go to big of a endmill dia. wise. I have tried a couple different endmills from .5 to .75dia 2flt and 4flt and 3in LOC HSS. Ran rpm's from 1500 to 3000 and feed from 7 to 20ipm. Nothing seems to work so any help will be much appreciated. If I didn't give enough info let me know. Thanks Eric

Go to the largest endmill you can use, use an extended endmill, the ones with a relief cut into the shank, with a flute length of say 3/4"
but with a cutting reach of 2.5" these types of endmills work great in deep pocketing. 3&4 flute mills are more rigid, but have less clearance for chip evacuation, I would go with a 3 flute as its a good balance between rigidity and chip evacuation ability. Try running at 1530 rpm at 18 ipm with a .075" depth of cut. This speed and feed will give you a chip load of .004" and require a 1/3 of a hp, with losses and heat generation the machine will actually be using roughly twice that amount. I would climb mill on the finish passes, and flood it with coolant, you gotta get those chips out or you will be recutting them which is not what you want to do. Sure it's gonna take you longer to pocket it out but I think the surface finish will be nice. To make a shorter cycle time I would use a roughing endmill first to hog out as much as you can, then use the extended mill for a finish pass. I would go with a cobalt hss roughing mill and a carbide mill for the finish, carbide won't flex like hss, but you can't beat carbide around alot as it will chip or break, not likely to happen at moderate feeds and speeds with shallow doc's. You can also drill out the corners to reduce the side loads generated once the endmill tries to go around the corner. You will need to adjust the feed and speed until it sounds good, a noisy endmill is one that is gonna leave chatter marks. Hope this is of some help.

[kacheric]

There are a couple of important factors to consider when attempting to eliminate chatter, an important one that was not mentioned is end mill helix angle. Many companies offer 3 flute high helix cutters that do a very good job of eliminating chatter. They do this by converting much of the cutting force to axial where things tend to be more rigid. Another thing to consider is generating a radius in the corners. If you use a cutter that produces the exact corner radius it will have 90 degrees of contact when hitting the corners and that is sure to cause chatter. By sweeping even just a small radius, maybe .030" you will eliminate this momentary high contact that causes chatter. A final comment would be use your feed and speed override knobs and explore, sometimes just a small adjustment will find the systems stable cutting condition.

Eric

[CASTLEVILLE]

thanks guys, I guess I need to order some endmills today.

[JDenyer232]

Originally Posted by kacheric There are a couple of important factors to consider when attempting to eliminate chatter, an important one that was not mentioned is end mill helix angle. Many companies offer 3 flute high helix cutters that do a very good job of eliminating chatter. They do this by converting much of the cutting force to axial where things tend to be more rigid. Another thing to consider is generating a radius in the corners. If you use a cutter that produces the exact corner radius it will have 90 degrees of contact when hitting the corners and that is sure to cause chatter. By sweeping even just a small radius, maybe .030" you will eliminate this momentary high contact that causes chatter. A final comment would be use your feed and speed override knobs and explore, sometimes just a small adjustment will find the systems stable cutting condition. Eric

All good points, with the higher helix mills work holding becomes more important as a high helix mill will try and lift the part even more than a standard helix mill.

[Geof]

New cutters often chatter badly but they settle down when the extremely sharp cutting edge has been dulled a little.

A drastic way to do this is to wad up some Scotchbrite firmly and stroke it down the cutting edge. Be really careful you don't cut through the Scotchbrite into your fingers if you do try this.

A less drastic way if you have many pieces is rough them out using the new cutter leaving enough material to clean up the chatter later. Just put in earplugs and ignore the chatter and hope that it goes away as the tool dulls.

[ImanCarrot]

If he's going to use a carbide on the finish cut would it be better without coolant? I've heard others say that carbide can handle heat fine, but hates going from hot to cold and will chip on the cutting edge. Soz for asking, just curious.

[Geof]

Originally Posted by ImanCarrot If he's going to use a carbide on the finish cut would it be better without coolant? I've heard others say that carbide can handle heat fine, but hates going from hot to cold and will chip on the cutting edge. Soz for asking, just curious.

For machining aluminum coolant or some form of cutting lubricant is almost essential. You do not encounter the same cutting edge temperatures on aluminum as on steel but you can get adhesion of the chip to the tool which can cause jamming.

[JDenyer232]

Originally Posted by Geof For machining aluminum coolant or some form of cutting lubricant is almost essential. You do not encounter the same cutting edge temperatures on aluminum as on steel but you can get adhesion of the chip to the tool which can cause jamming.

Pretty much what Geof said, because this is a pocket it will be full of coolant, you wouldn't have to worry about thermal shock as the cut is not an interupted one. Using a 2inch indexable 4 insert face mill on steel with coolant could crack the carbide inserts as each insert gets extremely hot, and is then cooled rapidly as it leaves the cut, this type of cut would be called an interupted cut. Hope this helps.