Buried pipe under soil motion

[Ardi_Eng]

Hello dears!

I'm going to model a buried pipe repaired by composite sleeve under soil large displacement. I'v tried to do modelling in Ansys "static" structural and used Mohr-Coulomb to define soil plasticity. I set 2 steps, in first step, internal pressure and Earth gravity were applied and in second step, large displacement of soil in vertical direction with 0.5 meter value was applied to bottom side of one of blocks. The model was solved in first step but it doesn't converge in second one and I don't know why.so my questions are:

1) IS Ansys "static" structural suitable for analyzing large displacement of soil or not?

2)Should I use Ansys "Transient structural" for these types of large motions or Ansys "Static" Structural can also be used for this modelling (with quasi static assumption)

3) If I use Static analysis for it, what should or can I do to achieve solution convergence.

Some photos of my modelling can be observed in attachment files
Any answer can be appreciated
Thanks in Advance

 

[Erik Panos Kostson]

That is a very large displacement, no wonder it can not solve. Normally with soil and structure (pipes and tunnels), the bottom of the mesh is fixed (side faces are not moving in normal direction), and boundary conditions are applied at the top of inside the structure (and gravity as global load), but not seen enforced displacement of 0.5 m applied at the bottom. If you still want this because you want to see when the pipe fails, apply the displacement gradually and see how far it can solve. You can also remove the soil and try and see if that helps and convergence is better (use compression only support on the pipe). Also try only the soil, but it is doubtful it can take these displacements. Otherwise feel free to post a .dat, or .db, or a nastran file and I can have a look.

Ps: quasi static assumptions are appropriate here

 

[Ardi_Eng]

Thank you dear Mr Erik Panos Kostson!
I've studied an article which used these boundary conditions for buried pipe. It can be received in attachment. It seems that this article studied large soil displacement using Ansys Apdl.However, I don't know it used either static or transient analysis for that.

Dear Eric! Thank you again for your consideration.

 

[Ardi_Eng]

Large displacement of soil without pipe can be solved easily. Deformation can be seen bellow.

 

[Erik Panos Kostson]

That is OK, I did not do much.

OK, I see why you can solve the soil, the two halfs are disconnected (never imagined that it was the case, normally soil is one piece).

Of course then the soil is not a problem to solve (just a rigid body movement). There must be something with the pipe then and/or the soil when both are active.

In your log file (not sure which one though), you should see where the force residuals or displacements are not converging (an element number). If we find this location we can see which part has a problem and why.

Then we could start removing nonlinearities (material and geometry) to get it to converge to see what is causing the problem.

Finally when we find out we can address it.
Nonlinear is always a bit tricky, but we always manage with some investigating.

Hope this gives you an idea. As for the analysis it is probably not dynamic since we do no care about any dynamic effects, thus quasi static (neglecting inertia), should be fine as far as I can see.

 

[Ardi_Eng]

Thanks dear Erik
You gave me nice ideas
I'll try to continue modellings in Ansys Static Structural.

 

[Erik Panos Kostson]

That is OK.

It is a very nice example.

I have solved this in Strand7 (for steel and GFRP), and it took me some time to get it right even though I would say that I know the software fairly well.
(convergence rates are very slow due to the soil material nonlinearity, not sure how it is ANSYS, but it can take many nonlinear iterations for an increment to converge - enforced displacements are applied gradually in increments/steps, so say 0.1 m, and then 0.2 m,...)

Hopefully we will have this as an example/webnote. many thanks for your post.