Elastoplastic Analysis of an Offshore Component

[wnmascare]

Hi everyone!

I was running an elastoplastic analysis of an offshore component with three different mesh refinements in Abaqus. The attached figure illustrates the meshes and the distribution of the equivalent plastic strain (PEEQ) for each mesh. A steel cable will tied in the hole and a force of 105 kN will be applied in the downward direction. The left side is fully constrained (encastred).

As you can see, the PEEQ jumped from a low value of 2.456% (coarser mesh) to 188.33% (finer mesh). In this case, the element size of the finer mesh is about 1/3 of the coarser mesh. Have you guys been through such similar situation, where the stress or plastic strains increased as the mesh was refined? One more thing: the force was applied by means of rigid elements (Kincoup).

Thank you in advance.

 

[wnmascare]

This the figure I mentioned previously.

 

[rb1957]

finer mesh is more sensitive to load spikes ... how distributed is the applied load ?

can you extract nodal results from the coarse model ? compare to a fine mesh element ?

another day in paradise, or is paradise one day closer ?

 

[wnmascare]

rb1957, thank you for your prompt reply.

The way I distributed the load can be seen in the attached figure. The red lines are the rigid elements (Kincoup). And they were distributed on the area of contact with the steel cable pin. Then, the load was applied on the central node. I tried to represent the steel cable pin by a cylindrical rigid surface and apply the contact condition, but I got overclosure problem. Even when I moved the cylindrical surface away from the contact surface in the hole, the overclosure problem remained. Thus, the utilization of Kincoup elements was my only alternative.

I took a look at the node values from both meshes and the difference between them is also huge. The maximum values are: coarser mesh (PEEQ) = 1.7% and finer mesh (PEEQ) = 216.7%.

I´m sorry, but what do you mean by "load spikes"? I don't get it.

Thank you in advance.

 

[ESPcomposites]

If you can't model it with contact (and you should be able to), you might apply the load as a cosine distribution to the hole. The way you are applying the load appears to be creating very localized peak stresses that are not real. If you run an elastic-plastic analysis this should "go away" though and give you a more realistic result. If you are trying to find the ultimate capability, these localized peaks won't matter too much. I am not sure what your goal is though.

As you increase the mesh density, you are better able to capture the stress concentration. At some point, you will reach an asymptotic value, but only if the load is applied in a reasonable manner. You may want to try a simple model and compare your answer to Peterson's stress concentration. I have found that the stress concentration for pin loaded parts can vary a decent amount based on whether you use contact (and the amount of clearance) or if you use simulated cosine load. But you should still be able to get a reasonable comparison to Peterson's. I am not sure that is the case with your current model.

Brian

http://www.espcomposites.com

 

[wnmascare]

Thank you guys for your help.
I could model the contact and it worked. The plastic strains are now in an acceptable level.