Flatness problems on 6061-T6 aluminum

Cha0ticBliss · Nov 18, 2021

Does anyone have any tips or tricks on maintaining tight flatness requirements on 6061-T6 (or T6511) aluminum?

Parts are generally around 12"x 12" and at least .100" thick on the majority of the part. Most have pockets and or ribs so lapping is not an option for most. I normally see .002-.003" flatness on a part this big, but have been no-quoting several jobs lately that call the same flatness on a part twice as long.

I've seen that dull cutters or aggressive cutting can definitely induce stress, but beyond that it seems like a each lot of material behaves differently. Some hardly move after machining while other lots can bow 4 times as much with the exact same process.

I spoke with a heat treater and they suggested heating the raw material to just below the tempering temperature to relieve any internal stresses so will probably give that a go, but am open to any other suggestions!

Mtndew · Nov 18, 2021

How are you cutting the thickness currently?
Can you order Mic6 plate?
Typically we would have to find a way to clamp the part without forcing it flat, then mill/flip/repeat as many times as it takes to get the desired flatness.

Finegrain · Nov 18, 2021

Can you clarify "at least .100" thick on the majority of the part"? Do you mean a 1" thick (for example) part with pockets having .1" walls and floors?

Regards.

Mike

Larry Dickman · Nov 18, 2021

lot of variables here, you didn't give a whole lot of info.

What side of the world did the material come from?
You say T6511 (bar) You'll have better luck with plate
How are you finishing? Face mill? Try having the OA thickness blanchard ground.
Rough the parts, have them cold cycled, then let them sit in the corner for a week.

charlie gary · Nov 18, 2021

Here's a few of thoughts based on very little info given.

Buy material thicker than your finished part, with at least .1" extra on each side. Then make sure your part comes out of the middle of this material.

Use sharp cutting tools. The more stress you impart into the material, the more it will warp. I've successfully machined 24" x 24" x .5" fixture plates flat within .002" by facing with a 1/2" sharp corner end mill. I started with 3/4" plate. When I tried the same parts with a 4" face mill, they warped a lot.

As previously mentioned, don't force the material flat when clamping and expect a flat part to come out of the machine.

Machinerer · Nov 18, 2021

Non-coated tools can help. As was said before, origin of material can make a difference. We had a run of parts that were running great, then we got an order of material from a russian company, for a cheaper price and profiles and flatness went to hell. Went back to Alcoa material and all was well. As was also said, fixturing is key. Hold the part on 3 points if possible, and make sure to clamp over those points, without deforming the material.

Cha0ticBliss · Nov 18, 2021

Mtndew said:
How are you cutting the thickness currently?
Can you order Mic6 plate?
Typically we would have to find a way to clamp the part without forcing it flat, then mill/flip/repeat as many times as it takes to get the desired flatness.

I'm held to the customer's requirement for 6061-T6

Cha0ticBliss · Nov 18, 2021

Finegrain said:
Can you clarify "at least .100" thick on the majority of the part"? Do you mean a 1" thick (for example) part with pockets having .1" walls and floors?

Regards.

Mike

Sorry for the limited info, was just trying to avoid a TLDR post where folks may not want to take the time to read through a page of info.

For the part I am working on right now:
-90% of the part is .100" thick
-There are several thru holes and threads. 15% of the part consists of pockets (approx .5" x 2" x .04 deep) with floor thickness of .060".
-1" from the perimeter of the part there is a rib that is .050"thick x .100". The rib runs along 3 sides of the part.

Since one side of the part is not supported by the rib, we generally see the most distortion in that general area.

Cha0ticBliss · Nov 18, 2021

Larry Dickman said:
lot of variables here, you didn't give a whole lot of info.

What side of the world did the material come from?
You say T6511 (bar) You'll have better luck with plate
How are you finishing? Face mill? Try having the OA thickness blanchard ground.
Rough the parts, have them cold cycled, then let them sit in the corner for a week.

All of our material is DFAR compliant but the cert doesn't show what country it came from. (cert says material was melted in US or another DFAR compliant country)

Seems like it is sometimes a toss-up between bar or plate. I the past I always was under the impression that plate was always better. We ran a basic flat 16"x4"x.250" cover recently out of bar and plate that were both the same original thickness. The plate stock yielded .035" flatness while bar was closer to .006"

We generally finish with 3/4 coated endmills or 1.5" Korloy insert cutters. May try smaller .500" uncoated end mills for finishing and see if that yields better results.

What do you mean by cold cycling? Put in freezer overnight?

Cha0ticBliss · Nov 18, 2021

charlie gary said:
Here's a few of thoughts based on very little info given.

Buy material thicker than your finished part, with at least .1" extra on each side. Then make sure your part comes out of the middle of this material.

Use sharp cutting tools. The more stress you impart into the material, the more it will warp. I've successfully machined 24" x 24" x .5" fixture plates flat within .002" by facing with a 1/2" sharp corner end mill. I started with 3/4" plate. When I tried the same parts with a 4" face mill, they warped a lot.

As previously mentioned, don't force the material flat when clamping and expect a flat part to come out of the machine.

Agreed, I've been considering skimming .100" off both sides, let it sit for a week or two, then machine op1 and op2 sides.

I have had the most luck centering the part inside of the blank but ignoring the ribs while doing so. Seems that if the main "floor" of the part is on center, even though there may be ribs sticking out of one side of the part that are closer to the edge of blank, the net part comes out flatter when the main floor of the part is on center to the blank.

If there is a lot of stress within the blank and assuming I'm not inducing stress with the milling, the only solution I can think of is to rough both ops, let it distort to where it wants to be. Then clamp op1 without distorting, finish op1. Then go onto op2. In theory that would be a good way to go but in practice clamping a flimsy part firmly enough to avoid chatter and without distorting the part is fairly challenging and not to easy to get the repeatability I'm hoping for.

Cha0ticBliss · Nov 18, 2021

JBethell said:
Non-coated tools can help. As was said before, origin of material can make a difference. We had a run of parts that were running great, then we got an order of material from a russian company, for a cheaper price and profiles and flatness went to hell. Went back to Alcoa material and all was well. As was also said, fixturing is key. Hold the part on 3 points if possible, and make sure to clamp over those points, without deforming the material.

Luckily the customer's spec on the material prevents us from getting anything from Russia, but not sure exactly where the material is sourced. (Cert says melted in US OR dfar compliant country)

Most of the parts I work on are too thin to mount on 3 points. Having a 4 point mount + 1 in the center to avoid vibration might be an option. Would need to adjust the heights of the mounting points for each part however.

Larry Dickman · Nov 18, 2021

Cha0ticBliss said:
What do you mean by cold cycling? Put in freezer overnight?

parts get frozen/ heated for several cycles.

Machinerer · Nov 18, 2021

Cha0ticBliss said:
Luckily the customer's spec on the material prevents us from getting anything from Russia, but not sure exactly where the material is sourced. (Cert says melted in US OR dfar compliant country)

Most of the parts I work on are too thin to mount on 3 points. Having a 4 point mount + 1 in the center to avoid vibration might be an option. Would need to adjust the heights of the mounting points for each part however.

Sorry, by mounting on 3 points, what I meant was, 3 solid, coplanar points, then i'll usually use adjustable supports/rest buttons to support the part as needed for rigidity or vibration dampening.

Orange Vise · Nov 18, 2021

Cha0ticBliss said:
I spoke with a heat treater and they suggested heating the raw material to just below the tempering temperature to relieve any internal stresses so will probably give that a go, but am open to any other suggestions!

So that's going to be somewhere in the neighborhood of 350F. Not really that hot, and you could do it in a household oven.

It could help, and wouldn't hurt to try, but your best bet is to Blanchard or surface grind after machining.

Blanchard is not expensive and most shops will hold +/- 0.001 as a standard tolerance, hitting both sides. Just need to establish a good relationship with a local Blanchard shop.

EmGo · Nov 18, 2021

Cha0ticBliss said:
Agreed, I've been considering skimming .100" off both sides, let it sit for a week or two, then machine op1 and op2 sides.

You've considered skimming both sides of rolled plate ? Who the hell taught you to cut metal ? They missed a few lessons.

gustafson · Nov 18, 2021

Cha0ticBliss said:
I'm held to the customer's requirement for 6061-T6

I think I would be tempted to make a part from Mic 6, and if it is just run it and ship it[not saying it will be] and bring it in, say:
'This one is 100 bucks a piece, this one is 50 bucks a piece, which one do you like?"

Sometimes you get thrown out of the office, sometimes you win loyal customers for life.

Vcmt · Nov 18, 2021

I would buy the stock from TCI metals they double disk grind the stock and guarantee .001 flatness.

I bought 12 aluminum plates 6061, 16 inches square .5 thick I put them on my surface plate and they were within .0003 flat.

The part may warp after you machine it but is nice to start with a flat piece.

MaxPrairie · Nov 18, 2021

Vcmt said:
I would buy the stock from TCI metals they double disk grind the stock and guarantee .001 flatness.

I bought 12 aluminum plates 6061, 16 inches square .5 thick I put them on my surface plate and they were within .0003 flat.

The part may warp after you machine it but is nice to start with a flat piece.

Grinding is a form of stress relieving so he might be okay getting them double disked.

Kalispel · Nov 18, 2021

6061-T6 material can heated to reduce machining stress. The optimum temperature is 290 degrees C (555F) where distortion is reduced by 60% with a corresponding loss of 20% of its yield strength. Heating above 300 degrees C can further reduce distortion but strength falls off quickly. Reheating below 240 degrees C has no benefits.

Just a moment...

jwmelvin · Nov 19, 2021

Kalispel said:
6061-T6 material can heated to reduce machining stress. …

Just a moment...

Thanks for the reference.

Flatness problems on 6061-T6 aluminum

Plastic

Diamond

Diamond

Titanium

Stainless

Cast Iron

Plastic

Plastic

Plastic

Plastic

Plastic

Titanium

Cast Iron

Titanium

Diamond

Diamond

Plastic

Hot Rolled

Aluminum

Aluminum

Similar threads