Residual Stress Management

[TheePres]

Has anyone heard of RSM, nonsequential balanced machining, and harmonic feeds and speeds?. Had a tooling engineer mention above terms concerning machining of thin wall/floor aerospace parts using 7075 alum. One of his claims is, all odd feeds and speeds seem to provide better results ex: 4011RPM instead of 4000RPM, 55.5 instead of 54 IPM etc....

[Michael Reynolds]

Unless he's talkin' about a constant variable(ing) speed and feed, sounds like hokus pokus to me. BUT there is a chance I speak out of tern...

 

Mike R.

[Finecut]

Its more then that. Chip load, cutter geometry, speeds and feeds

For high speed machining in aluminum 3 flute is better then 2. Harmonics (or when that sweet spot of cutter slapping the wall is pushed to the point that the part vibrates or sings) for a 3 flute is much higher. This equals a faster feed rate and rpm. Its all still based on chip load.

 

MMSonline.com has some info on this.

 

Now for the bad part. Not all parts can be run the same way. Some experiments will have to be done to get the best feeds and speeds. Part geo

plays a big role in how to program for the best results.

 

Thin walls and thin floors can be tough. 7075 will stress relive more when you get below .1 thickness.And tool wear on this material is more then fun to deal with

 

Tips from my experiance:

 

A small radius on the cutter if allowed , for finish.

Final pockets and /or floor routines, work from inside out

all walls ( for thin ones ), work all to the same z height as you step down

If you can find the harmonics , note it and stay above or below

Flipping a part several times to keep the flatness is sometimes needed. ( Yea its sounds dumb and time consuming, but it works )

 

Hope this helps

 

Finecut

[cadcam]

I have read and actully seen them come out to Haas factory and do this.

I still am not complety sold on it.

Some of this we as machinst are all ready doing by the way it sounds and adjusting at the machine.

 

And the guys that were showing us still did this to.

But there is some truth behind it.

[johns]

One of the variables is that every machine has a harmonic range, it vibrates in time to the spindle speed or even the axis servo motors. Alot of times, the machine builder can model this and add some ribs or adjust casting thickness to move this value out of the operating range of the machine. The more common harmonic vibration that we see is due to the part and spindle (tool) within a certain range. if you're taking a .1 cut in a 2" block, it won't show, but if you get to thin ribs or sections it can effect size and finish dramatically. For thin ribs, it is always best to finish cut in steps, doing each side of the rib at the same depth and stepping down. Here's a trick from an "old guy", keep a lighter and some wax handy. Add a few blobs along a thin section to dampen the vibration.

Harmonics in the extreme case can cause so much vibration that stress cracks can occur. Aircraft people don't like this! If you use a stethoscope to listen to the mat'l being cut, and experiment, you can actually hear the difference as speeds and feeds are changed.

I agree with Finecut that 3 flutes are better. In the old days, we used Strassman or Cresscut mills for roughing to prevent vibration and tool breakage, but all I see now is carbide tooling.

I showed one shop I was at how to reduce roughing by 50% by going full depth with a Strassman in one pass at 4 ipm, rather than multiple steps with carbide at 16 ipm.

[Guest CNC Apps Guy 1]

But with that 4 IPM comes stress, heat, poor chip evacuation, etc... of course, 16IPM is barely moving anyway but still, heat and stress are big contributors to part warpage, and the dreaded chatter. I'm doing a part right now out of 7075. Starts out at a good 75lbs when all is said and done about 5 lbs will be the final weight. there are only two standing walls and a .125 floor and a few .09 floors. How I am approaching it is one depth at a time and finish at that depth. I do this because it offers the most support for the walls and pockets. BTW my feeds will be in the 400 -600 IPM range on a Mori Seiki SH-630 HMC.

 

JM2C

[TheePres]

Thanks all for your suggestions, will incorporate on my current project. It involves a 8"x30"x240" block of 7075. The thickest wall is at .250 and floors down to .08 at points. My most ambitious project to date. How do you manage feed rates as high as you state?. Must be on 10,000+ spindles, Im limited to 4000RPM.

[johns]

James, the feed rate example was for stainless, I forgot to mention that. I used an air blow with coolant fed into the air stream for chip evacuation and the standing features were to the middle of the block, so the depth cut was from the outside of the block.

For TheePres, consider having the CNC work done on a high speed CNC, especially if you have a number of parts to do.

[gary dunn]

i would think that if you took less than half the diameter of the cutter, you would throw the chips out instead of trapping them in the flutes for a rev and that would eliminate both heat and some of the vibration caused by temporarily trapped chips. what do ya'll think about that ? as far as cutter geometry, has anyone tried those SGS

Zcarb endmills ? 2 of the flutes are cut on one angle and the opposite 2 are cut on a slightly

different angle. those cutter work well, especailly in hard steel (52RC approx). i would be interested in hearing opinions on those also.

[TheePres]

Im very much interested in taming this "xxxx" material, had a job once making wing skins, using 3/4" plate, about 4ft. x 8ft. Ran on vacumn with only 4 bolts at corners, (counterbores only left about .25 thickness). After completion, operator released vacumn valve, causing part to fold lengthwise ripping at bolts and cracking into 2 seperate pieces.

I found this article, you all might be interested in. R.S.M.