What's new
What's new

Warpage on T6061 plate part

MiamiCNC

Plastic
Joined
Dec 2, 2019
Location
Florida, USA
I'm getting my butt kicked on this part and hope someone can give useful advice. Making a part from T6061-T651 plate. Part is approx 15x18 inch rectangle. Has a raised center section 0.6" thick approx 1/3 the width down the center, with lots of slots (kinda like a maze). This is flanked by two flat wings 0.4" thick. The bottom is flat, and the profile is on the top side. There are no thru holes, so the part is machined from larger sized stock which is bolted to a subplate along it's periphery. The raw material is 1" thick T6061-T651 that I happened to have from an old job, sitting under the Florida sun for a couple of years. My problem is that the part warps about 0.015 along the periphery (thin wings warp up toward the pocketed side), and I can't figure out a way to prevent the warp (tolerance 0.005 flatness). Here is my order of operations:

  • Face the flat side of the part, leaving about 0.020 for a later finishing op.
  • Flip it over and machine the top side. The perimeter contour is machined, leaving tabs.
  • Part flipped back over and flat side is faced.
  • Equal amounts of material are removed from each side of the plate.

Also tried taking very little material off the flat side (0.005), removing the bulk of material from the top side, with same exact results.

Don't know if this problem in inherent to the geometry and material? if the problem is that my material has been sitting out in the sun for a couple of years? if the material is too thick and thinner plate (less material removal ) would be better? My work holding? would cast aluminum be better?, or is it just that I am a shitty machinist.
 

barbter

Diamond
Joined
Oct 27, 2007
Location
On Tour...
If your stock is initially not flat, and you bolt that down and skim it, when you unbolt it, it will probably bow back....
Your OP1 - Face the flat side of the part, leaving about 0.020 for a later finishing op.
Is the mtl dead flat after doing this?

Ultimately if the section of the job is similar between both sides, you have to concentrate on getting the OP1 flat IMHO.
And the size of the part is large enough to hold/suck the centre with vacuum - incase there's a risk that the centre is lifting on your OP2?
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
  • Face the flat side of the part, leaving about 0.020 for a later finishing op.
  • Flip it over and machine the top side. The perimeter contour is machined, leaving tabs.
  • Part flipped back over and flat side is faced.
  • Equal amounts of material are removed from each side of the plate.

Also tried taking very little material off the flat side (0.005), removing the bulk of material from the top side, with same exact results.
Order of operations look fine, what we don't know is HOW you're clamping the part after the 1st operation.
It would need side pressure, like in a vise.
 

MiamiCNC

Plastic
Joined
Dec 2, 2019
Location
Florida, USA
If your stock is initially not flat, and you bolt that down and skim it, when you unbolt it, it will probably bow back....
Your OP1 - Face the flat side of the part, leaving about 0.020 for a later finishing op.
Is the mtl dead flat after doing this?


Checked a piece of stock and damn if there isn't a nice 10-15 thousand warp. At least now I know the issue. Feel like a dumbass. I will flatten the stock and rerun the part. Let you all know the results.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Pretty much the same as everyone said if you lay the part on a surface plate and see a .015 bow, and then clamp it down flat the bow will/may come back after you machine it, and then un-clamp it.

In grinding we put a shim under the bow and grind one side flat. Sometimes just take part of the take and see what that does. Some bigger parts need flip-flops. A .015 bow may need over .030 to machine/grind flat.

Dull, or wrong rake angle cutters can put stress in a part to cause some change in flatness.

Stress already in the part can be relieved and make a seeming falt part have warps after machining that releases the stress.

Sometimes you may be stuck with a straightening operation. (.6 part is not easy to straighten)

*If you have a blacksmith in town he might give you some ideas of how to straighten/relax them before machining.
 

GiroDyno

Aluminum
Joined
Apr 19, 2021
Location
PNW
When machining large composite structures more often than not we would have an uneven/floppy wet noodle to begin so we would set them on hard points and epoxy them in place for a first op. Clamped in an "unstressed" state we could cut a nice reference surface, break them free and flip to cut them with a nice flat bottom.
Epoxying parts to your table might not sound ideal but maybe burnish some tape to the table first or put down another piece of scrap material.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
Checked a piece of stock and damn if there isn't a nice 10-15 thousand warp. At least now I know the issue. Feel like a dumbass. I will flatten the stock and rerun the part. Let you all know the results.

Yep, extruded aluminum isn't normally very flat.
 

MCritchley

Hot Rolled
Joined
Mar 22, 2007
Location
Milwaukee
In general i like to get the stress that will warp a part out in 2 roughing opps, the part will move let it. As others have said shim under the hollow spots so there is support. And never bang the part down with a hammer, that will just bend the part.

Are you holding the part in a vice? A vice always warps a part with that geometry. If you are clamp lightly and do not be a hero when roughing, slow it down.

If you have time make a flat fixture plate with mite bite edge clamps to hold the part. I have an AL part 26 x 16 x.650 that needs to be flat within .002". No problem as long as i flip it 4 times, shim the hollows, and hold in a fixture as described above.
 

MiamiCNC

Plastic
Joined
Dec 2, 2019
Location
Florida, USA
Thanks for the all the input. Would like to give some follow up.
Took my time in stock prep. Did light facing on the floating stock, flip-flopped a few times and was able to get the flatness down to around 0.001 on both sides. Pretty damn good given the size of material (18-21") Bolting it down at this point didn't cause any significant deflection. So good to go, right?

Op1 do the flat side, leaving 0.010"
Op2 do the profile side

At this point there is a 1" frame of stock remaining along the perimeter. Flatness on both sides is good. Slot the part from the stock and measure..... Part still curls away from the area of most material removal. About 0.008" primarily on the four corners. Fortunately I was able to re-flatten the bottom. The low point was in the center. put a 10" weight on the center over the full-thickness area of the geometry, and took light finishing passes from the outside in, blending into the flat center. Ended up at 0.003" flatness. Of course there is now a bit of a taper on the flat thin wings on the top side.

I surmise that the outside frame of stock was holding the internal stresses in check during machining which resulted in the bowing of the corners once I removed the frame. Need to rethink work holding. I am thinking it would be best to use stock close to final dimension and just clamp the sides with pitbulls. On finish cut I could relieve the clamp pressure and allow the material to deform before finish cutting.

This has been a frustrating and expensive lesson, but those are the ones that stick I suppose. Aluminum has gotten WAY expensive lately.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
I surmise that the outside frame of stock was holding the internal stresses in check during machining which resulted in the bowing of the corners

Yep,you need to remove all of the "crust" as I call it from everywhere, unclamp to let it banana and then re-clamp.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Thanks for the all the input. Would like to give some follow up.
Took my time in stock prep. Did light facing on the floating stock, flip-flopped a few times and was able to get the flatness down to around 0.001 on both sides. Pretty damn good given the size of material (18-21") Bolting it down at this point didn't cause any significant deflection. So good to go, right?

Op1 do the flat side, leaving 0.010"
Op2 do the profile side

At this point there is a 1" frame of stock remaining along the perimeter. Flatness on both sides is good. Slot the part from the stock and measure..... Part still curls away from the area of most material removal. About 0.008" primarily on the four corners. Fortunately I was able to re-flatten the bottom. The low point was in the center. put a 10" weight on the center over the full-thickness area of the geometry, and took light finishing passes from the outside in, blending into the flat center. Ended up at 0.003" flatness. Of course there is now a bit of a taper on the flat thin wings on the top side.

I surmise that the outside frame of stock was holding the internal stresses in check during machining which resulted in the bowing of the corners once I removed the frame. Need to rethink work holding. I am thinking it would be best to use stock close to final dimension and just clamp the sides with pitbulls. On finish cut I could relieve the clamp pressure and allow the material to deform before finish cutting.

This has been a frustrating and expensive lesson, but those are the ones that stick I suppose. Aluminum has gotten WAY expensive lately.

Sounds like you have it nailed. Cutting forces may push down a lot more than most people would think. Having an adjusting screw under the part hollow might aid your first pass to make flatter.

I test a grinding job with a 3 finger push down,..that is about a 20 - 25 pound push, If it moves .001 then the wheel pressure will do the same. Most milling would be way more.
 

GiroDyno

Aluminum
Joined
Apr 19, 2021
Location
PNW
Once you're all out of ideas you could do it the way consumer 3D printers compensate for floppy print beds and create a mesh surface to mirror the .008" dish you're seeing and machine that :rolleyes5:
flat.jpg
We have a clapped out VF2 for side projects and when I have to put in any sort of "tight" tolerance bore I model it as an oval to compensate for the .003" slop in X.
 

charlie gary

Stainless
Joined
Oct 4, 2009
Location
near Seattle, Washington, USA
You haven't told us what you used to face the material, but if it's a face mill with inserts odds are pretty good that's the source of your warping stress. I've done 18"x24" fixture plates with a face mill and got parts with bad bows (about .010") in them. Same parts finish-machined with a nice 1/2" 3-flute sharp corner end mill came out flat within .0005".
 

MiamiCNC

Plastic
Joined
Dec 2, 2019
Location
Florida, USA
You haven't told us what you used to face the material, but if it's a face mill with inserts odds are pretty good that's the source of your warping stress. I've done 18"x24" fixture plates with a face mill and got parts with bad bows (about .010") in them. Same parts finish-machined with a nice 1/2" 3-flute sharp corner end mill came out flat within .0005".

The flat side was done with a 2.5" Ripper face mill. The pocketed side with a 1/2 EM.

Going to try again today. Will do a rouging of the entire part leaving 0.010 on each side. Check for flatness and compensate for any warpage with shims. Let you all know how this approach goes.
 

gustafson

Diamond
Joined
Sep 4, 2002
Location
People's Republic
The old school safe way to do it is basically whole part gets machined twice.
rough side one
rough side two pockets everything
finish side one[which hopefully gives you a flat surface to clamp to]
finish side two.

As mentioned if you clamp warped parts, you will get warped parts, but how many times have I tried to find a shortcut and screwed around for hours when the long way would have been faster
 

charlie gary

Stainless
Joined
Oct 4, 2009
Location
near Seattle, Washington, USA
The flat side was done with a 2.5" Ripper face mill. The pocketed side with a 1/2 EM.

Going to try again today. Will do a rouging of the entire part leaving 0.010 on each side. Check for flatness and compensate for any warpage with shims. Let you all know how this approach goes.

Try finish machining the big flat side with a sharp end mill instead of a face mill. It takes more time, but in the end your part won't be out of tolerance.
 

Halcyon

Plastic
Joined
Jul 17, 2022
Try finish machining the big flat side with a sharp end mill instead of a face mill. It takes more time, but in the end your part won't be out of tolerance.

To add to this, you could experiment with the cut direction. Had a part that would come out with a bird bath if cut in x, but cutting it in y it turned out .001//. Go home metal, you're drunk.

Also use a torque wrench/handle..
 








 
Top