Collapse pressure of thick walled cylinder 1

[vtmike]

Hi,

I’m currently working on a thick walled pressure tube collapse problem in ANSYS Workbench 11.

The material properties for alloy steel are as follows,
Young's Modulus = 2.95e7 psi
POisson's Ratio = .29
Density = .283 lbm/in^3
Bilinear Isotropic Hardening elastic - plastic material model is used with,
Yield Strength = 1.3e5 psi
Tangent Modulus = 2e6 psi (Assumed)

A section of the tube is selected using symmetry, and pressure is applied with large deflection turned ON.

Now the second part of the problem involves the same tube with same loads, material properties & boundary conditions but with imperfections (machined couterbores) on the outer surface.

The collapse pressure (i.e. pressure at which maximum principal stress > yield stress) comes close to actual test results for collapse for the tube with imperfections on the outside surface but the maximum principal stress is way off for the tube without imperfections on the outer surface as compared to actual test.

I have attached the simulation file and a few images showing the boundary conditions (A is zero displacement in X direction and B is zero deflection in Z direction, and C is applied pressure) and results.

Do you see a problem with my boundary conditions? Any suggestions would be highly appreciated!

http://files.engineering.com/getfil...a9fe-0ffa2190aa24&file=24000psi_mesh0.1_1.jpg

http://files.engineering.com/getfil...ad8a-db6dc5c8f8e9&file=24000psi_mesh0.1_2.jpg

http://files.engineering.com/getfil...d81-dc64aed58567&file=Boundary_Conditions.JPG

Thanks,
Mike

 

[cbrn]

In doing simulations like that, there are lots of "caveat".
First of all, in the FEM analysis you input a materal's constitutive law. You are not respecting 100% the "real" constitutive law of the "real" material (unless you have tons of experimental data for this material). This matter is adequately taken into consideration in any Norm with the "Direct Route" or "Inelastic Route" as you want to call it.
Then, the experimental data are affected by measuring errors. When you check results compatibility between FEM and experimental, you associate a tolerance to both.
The intrinsic error of a nonlinear calculation like yours can be as high as 10 or even 15%. When you say "the results are way off", did you take the "intrinsic uncertainty" into account?
These are only some ideas, anyway...
Regard

 

[gurmeet2003]

One important part of this analysis is interpretation of results. Your statement: "The collapse pressure(i.e.; pressure at which maximum principal stress> yield stress) is not correct. As shown by your results the material at the id of the tube begins to yield first. However this is not an indication of collapse. An indication of global collapse will be through yielding in the section. This is indicated by inablity of the numerical model to converge.

Thanks,

Gurmeet

 

[vtmike]

Hi,

Since I am still having problems with this model I thought I should repost my question by elaborating a bit more.
I am currently working on two cylinder models with external pressure acting on them.
The material properties for alloy steel are as follows,
Young's Modulus = 2.95e7 psi
Poisson's Ratio = .29
Density = .283 lbm/in^3
Bilinear Isotropic Hardening elastic - plastic material model is used with,
Yield Strength = 1.3e5 psi
Tangent Modulus = 2e6 psi (Assumed)

One has imperfections on its outer surface while the other does not. Both cylinders have the same ID and OD. A part of the vessel is taken according to symmetry, the same non-linear material model is applied, mesh density refined at critical locations for cylinder with imperfections on its outer surface, and a static analysis is performed.

The cylinder without imperfections was analyzed first, and no matter how much the magnitude of external pressure was increased, the cylinder did not buckle and stress in the model kept on increasing. This is because of the geometry being perfect.

Now, when a similar analysis was done on cylinder with imperfections on its outer surface, the cylinder started producing large deformations after a limit was reached on external pressure applied and the solution did not converge inspite of modifying the analysis settings. I am assuming this is a buckling response, since the calculated collapse pressure is close to applied pressure but not really sure.

I was under the impression that both models will not buckle no matter how much the magnitude of external pressure is increased since the inner surface of both models has perfect geometry.
Since the surface at the ID of the cylinder is perfect for both models, I have doubts about whether the extreme deformation response is indeed a buckling response?

I activated nonlinear STABILIZATION in ANSYS Workbench 11.0 by inserting following command snippet,

STABILIZE,CONSTANT,ENERGY,1E-4

but this did not help in converging the solution and getting a response. Although the solution went a little further than it did without the stabilize command.

Am I missing out on something here? Any help would be appreciated.

Thanks,
Mike

 

[TGS4]

Take a read through TFM on the topic of "snap-through" post-buckling analysis. If you want to know if you have buckling, you may be able to follow the part post-buckling.

BTW - symmetry is an absolute no-no for buckling analysis. You have artificially constrained the model from a potential buckling mode.

Also, how long is your model? Also, have you performed an Euler buckling analysis to see what the mode shapes might look like? Is your deformed second model deforming like a buckling mode?

 

[vtmike]

The way I am trying to do a collapse analysis on a complete tube model is restricting the left end in X, Y & Z directions and restricting the right end in X & Y directions (attached image shows coordinate system).

I am having trouble converging to a solution once a particular load is reached. Applying load in small steps and increasing the size of substeps did not help. So is there any other suggestion to get convergence for such a situation? Can I insert nonlinear stabilization or arclen commands in Workbench?

I did an Euler buckling analysis but it overpredicts the failure load by a very big margin. I am trying to figure out how I can use the deformed mode shape from the linear buckling analysis into a nonlinear buckling analysis in WB.

Thanks,
Mike