Anybody with experience with FEA on pulling vacuum in a tank? 1

[PatriotsRule]

I am looking using ANSYS Workbench and am not getting comparitive results to a physical test.

Material- Polyethylene and Foam composite
Non-linear analysis
The FEA results show higher tank stiffness compared to buckling like behaviour on the tank

 

[btrueblood]

What kind of foam? I'm guessing some type of urethane foam injected/overlaid onto a molded PE skin for the below:

You & ANSYS are probably modelling the composite as having "perfect" bonding (no delaminations) and infinite bond shear strength, whereas the real condition is many, many sites of delamination, and very poor bondline shear strength (polyethylene doesn't want to bond to anything).

Try modelling the tank as if it was PE only (no foam, or very low foam stiffness) and compare to test results.

 

[PatriotsRule]

Thanks for your input btrue...
I have a PE foam molded on to a PE skin so compatibility is not an issue (meaning they are chemically bonded)
I am not too experienced in buckling and nonlinear modeling and my guess is that the physical tank is showing signs of buckling in the vacuum test (How do I model it???)
Heres the scenario:
The tank (cylinder with ends capped with truncated semi circle/ Capsule look-alike) is sitting on two 2"x4" bars (so the tank is sitting on a elevation). I pulled vacuum at different inches of Hg to see it deform and recorded that deformations/displacements.
In simulation mode, I used quarter of this tank model. I have added the 2 x 4 pads (.010" thick) on the bottom of the tank to represent the support area. I used compression only support on these pads. To eliminate rigid body motion, I picked a point on the top of the tank and gave it a fixed supoport constraint. I gave it a symmetry condition in the lateral and longitudinal direction by picking on the flat surfaces.. I selected all the inside surfaces of the tank and gave it a negative pressure. I turned the large deformation on.
Currently, I do not have a non linear property/stress-strain graph for the PE as well has the foam loaded in my workbench. But I do have the yield and the ultimate tensile strength.
Does my set up sound ok? If not can you please advise.....

 

[GBor]

The fixed constraint is not correct. The tank should be allowed to displace along the vertical axis of the tank (assuming the centerline of the "capsule" is vertical)...I guess I should say that the translational direction along the line where the two symmetry planes intersect should be free to move.

I also doubt you will see buckling behavior without some good stress/strain data.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community

 

[PatriotsRule]

Gbor
Unless I give a fixed constraint, I always get a rigid body motion error. How do I solve that problem?? Any ideas?
Also I was told by our Workbench Help desk that to simulate a non linear buckling behavior, I need to turn the large deformation ON, which I did. What it does is allows the nodal coordinates to update itself as it progresses towards a final solution. Is this correct?
By turning the large deformation ON I did get a little better result than before but I did not come close to the real life displacements.
Can you help?

 

[GBor]

You definitely need large deformation, the question is does Ansys large deformation use Total or Updated LaGrangian formulations (sorry, not an Ansys user). Either should do, but that may have some influence.

I hope I'm picturing your set-up accurately. In my mind, I originally had the tank mounted vertically, but now, I guess, I'm picturing a horizontal tank much like a propane tank only instead of the saddles, you have two bars running down the length. Either way, I'm assuming the bars are mounted to something that is much more rigid than the tank (concrete floor?).

To prevent the rigid body motions, you need boundary conditions at the mounting location and symmetry conditions along the appropriate symmetry planes.

If you are getting rigid body motions for this analysis, it sounds like something is not tied together appropriately. Run a modal analysis. You should get a very large displacement (nearly infinite) at some point in the model. If large portions of the model move, parts may not be attached properly.

 

[PatriotsRule]

Gbor
The test set up is tank being raised to sit on two 2"x4 " wood blocks which are laying transversely to the length of the bottom of the tank and which are sitting (not fixed)on 4 inverted plastic buckets. This was done to measure the displacements on the bottom of the tank (it gives us some room in the bottom). So in practice there is no fixed support. I am allowing the whole tank to "curl" up and deform in each and every direction. I hope this description helps

 

[cbrn]

Hi,
large deformation -> OK, of course you need it if you want to do a buckling analysis since by definition it violates the "small displacement" assumptions.
linear material properties -> in my opinion, definitely NOT OK since you will greatly over-estimate the stiffness at high strains. As already posted by others, first of all I'd look for more detailed / realistic constitutive law.
Boundary Conditions -> the fixed restraint should be avoided since it will possibly impeach some buckling modes. If you can't keep the model in position over its supports, try to build "realistic" supports sets using frictional contacts (remember to have them update at each equilibrium iteration!!!), or see if you can adapt the "3-2-1" method to your case.
What you are trying to achieve is really not easy, so IMO you'd better build BCs as realistic as possible (weight, friction,...) AND constitutive law as realistic as possible.

Regards

 

[GBor]

It does help, still not sure why you would get rigid body motions...hmmmm. Sounds like you could actually have 3 symmetry planes. If you ignore the friction between the wooden blocks and actually remove them from the model, you have a capsule centered around the midpoint and collapsing in. I know a thermal analysis will do this without any boundary conditions...seems like the symmetry should do the trick if they are applied properly.

If you keep the blocks in, are you applying gravity? Are you using surface contact for the interface between the wooden blocks and the tank? The base of the blocks could still be fixed because they seem to be irrelevant in the results. Surface to surface contact with gravity applied would allow the tank to properly slide over the blocks, but this, I assume, is just a line contact.

If I assume the tank is centered at the origin and cut be the three global planes with the x-axis running the centerline of the tank, the z-axis running parallel to the centerline of the buckets, and the y-axis defined by the right-hand rule, you would have no translation along the y-axis on the face in the xz plane, no translation along the x axis in the yz face and no translation along the z axis on the xy face. If you are using brick elements, rotations are not an issue. At the point where the capsule head intersects the x axis, both the y and z translations should be constrained. By my count, you get x, y, and z constraints using these boundary conditions...that should eliminate rigid body modes.

If you are using only two symmetry planes, it seems as though properly constraining the model should still eliminate rigid body modes...



Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community

 

[PatriotsRule]

Gbor
I am going to try to set it up as you have mentioned and see if it works..I will keep you updated. Thanks for your help

 

[MikeHalloran]

>>>>I have a PE foam molded on to a PE skin so compatibility is not an issue (meaning they are chemically bonded)<<<<

I'm really, really curious about how you do that.

Have you actually demonstrated significant peel/ cleavage strength, or are you makng an assumption here?



Mike Halloran
Pembroke Pines, FL, USA

 

[btrueblood]

Um. Trying to figure out, without access to your software, how the model will account for low-order buckling modes when you are only modelling a 1/4 section (I'm envisioning this as a 90-degree segment of the cylindrical tank?). I think you have artificially constrained the tank to only buckle in modes which are symmetric around a 1/4 section, which eliminates the simple "squash" mode where a single indent occurs on one side. This could result in higher predicted buckling loads. I would model the whole tank unless I KNEW that I could account for the artificial constraints of symmetry b.c.'s.

Also, modelling of buckling modes with FEA is tricky at best; even if you use shaped elements to approximate smooth cylinders, the faceting of the elements results in artificial stiffness within the model. Frankly, even testing of precision shells in a lab will give you "big" error bands due to what seem like 2nd order and 3rd order effects. Read Roark's and some of the references it points to in the elastic stability section. Also, what artificial asymmetries have you built into your model to account for real-world production tolerances (e.g. the real tank is not perfectly round, nor is wall thickness uniform, did you model that?). Try modelling with an artificial near-point load or moment applied in one place, to generate a buckling "trigger" moment.

Oh, and I agree with Mike.