Deep Pocketing Aluminum

[John H]

Hi All,

I had asked this question once before and did not realy get a good answer,Maybe I just did not explain correctly.So Iwill try again. I have a 4.00 thk. x 5.375 x 7.125 aluminum block(6061)I need to machine a 3.500 deep pocket ..03 rad between floor and walls,need a 125 finish.What I am using is a multi-master .750 Dia. 3 flute head mounted to a 4"lg. bar to rough out the pocket,Depth of each cut is .250 dp. and I am ramping in.Feeds 33.00ipmand rpm is 4500. leaving .010" on the walls and .005" on the floor.Forgot to mention the pocket has .500 rads in the corners.then I come back with a 1.00" dia. 3 flute Dataflute endmill to finsh. I did try indexable end mill ,But way to much chatter.Can anyone give me some advise on speeds feeds and if this is the process to use?

Thank You in Advance,

John

[HuFlungDung]

Hi John
Well your problem is largely a matter of experiments carried out in the past, and how they panned out.

I would use an Iscar insert mill because they are quite free-cutting. The shank is also massive all the way down to the tip, as opposed to a fluted mill with 3.5" of flutes. I would use the special grade of polished insert with sharp edges to assist with the free cutting action and chip flow.

I might use a shorter endmill to begin with until it has gone as deep as it can. It may work well at .125" DOC, maybe 125 ipm feedrate.

I would likely use a depth of cut of about .06" and 100 ipm feedrate for the 4" long roughing mill.

Its critical to allow the tool to sweep the corner to reduce the engagement angle. After roughing, I would plunge machine the corner radii within .005 of finish. This would be an effort to clear most of the material from the corner so that the finisher will not run into a big bite, where the engagement angle suddenly skyrockets. I would want to prevent a chatter pattern from starting, if at all possible.

For finishing, I guess there would be little option but to go with a solid carbide finisher. Probably knock the rpm down to 1200 rpm and maybe 25 ipm to try obtain silent cutting. Those corner radii are going to give you trouble with instant chatter if you use a 1" finisher. This is because the engagement angle of the tool suddenly rises to 90 degrees as the tool enters the corner. So I would beg the designer to permit a larger corner radius, say .525" If he won't hear of it, then maybe go with a smaller diameter finisher....25mm maybe or 7/8" if you could find one.

[InspirationTool]

Are there any other ways of dealing with the engagement angle issue on corners?

I'm having a similar chatter issue on one of my parts. The chatter is acceptable, but not great.

I tried pre-drilling the corners, but the end mill was rather unhappy with the interrupted cut.

Thanks!

-Jeff

[HuFlungDung]

If you use a long, fluted tool, it might work to circle grind the flutes to a smaller diameter starting about 1/2" from the end, and all the way up to where the shank enters the holder. This will restrict your depth of cut to less than 1/2" per pass but will prevent too much cutter contact, which decreases the cutting pressure and gives rise to chatter.

[ctate2000]

Educated and experienced guess... I would use endmill smaller than the corner radius and interpolate the radius. This will minimize the flute engagement and put more load on the tool. I would cut center away leaving .250 or so on the wall. Then set up finish pass to traverse the pocket in a continuous move from top to bottom moving in Z all the time to put some axial load on the tool. The axial load will help stabilize the tool and combat chatter. The .03 radius is best acheived by grinding the corners of the finish tool to .03. The more you load the tool the less likely you are to get chatter. I would move fast and keep only the corner of the tool engaged no deeper than the .03 radius. Give it all the RPM you can muster and feed it heavy, say .010/flute. By staying on the radius you can maintain the finish requirement and the chip load will add some load to the tool. Clear as mud.

[little bubba]

I'll second what ctate2000 said, load the tool for the finish pass. I've been bitten many times with long overhang tools and chatter. All the things you think of doing naturally are wrong, less RPM, less feed and less finish allowance. The RPMs/SFM doesn't seem all that important, but feed rate and finish allowance are key. What I do now is keep the SFM where its at, and increase the feedrate and the finish allowance, it really stabalizes the endmill and it will leave a nice finish.

As for the corners, a .5R and a 1" endmill do not mix, especially at that depth. I would want to go as big as possible on the endmill, but that combo could kill you. Depending on the tolerance of your pocket, one thing I might try is to plunge the corner with the 1" endmill, then run the finish with a larger R(maybe .530 or so) so that it never even touches the corner. You may have a small cusp, but depending on the tolerance of the pocket, you might be OK.

This is one of those situations, where when you hit it, you're going to feel like a hero.