## General Mechanical

#### What support should be acting on base of tank in a 3D tank sloshing under earthquake.

• nikos
Subscriber

Hello all,

I would like some help regarding an attempt at simulating the sloshing of a 3D tank which contains liquid.

I use ANSYS Fluent to model the fluid parts (VOF, explicit, 2 fluid bodies for water and air) and Transient Structural to model the tank structure (two bodies, lower and upper, so they can be assigned to the corresponding fluid bodies for Data Transfer in System Coupling solver).

Apart from the Standard Earth Gravity, I would like to know what support I need for the base of the tank, so it resembles a tank on the ground, that has also the the freedom to move under a sinusoidal acceleration, attempting to simulate an earthquake.

My guess is the elastic support but I had some issues running with it.

Thanks for any answer and any light shed on the matter.

Nikos

• nikos
Subscriber

I am also attaching some screenshots.

The first one shows the fluid bodies (air in pink, water in orange)

The second shows the tank structure (tank wall that interfaces with air in orange, tank wall that interfaces with water in grey)

The third one shows the interior of the tank

• peteroznewman
Subscriber

The problem with Elastic Support is it only provides stiffness in one direction, which causes numerical problems when the forces move the tank sideways.

You will have to put a cylinder of concrete and/or soil material, with a margin beyond the tank, to support the tank.

• nikos
Subscriber

So what you are suggesting is that I make a base for the base of the tank and apply the elastic support on that?

Will it be essentially one more body underneath my tank with elastic support applied on it?

Should I also apply the sinusoidal acceleration on the new concrete/soil base cylinder?

Indeed, I need the tank to be able to move sideways.

• peteroznewman
Subscriber

The soil cut boundary (distant from the tank edge) would have a displacement BC that would have the XYZ displacement motion of the earthquake. The tank can sit on the soil and have frictional contact.

I recently worked with a 30 second earthquake record, sampled at 1,400 Hz so there were 42,000 rows of data in the 30 second time history, with 3 coordinates for a total of 126,000 numbers in the input data. I had to play some tricks to avoid bringing Mechanical to its knees.

If you just want sinusoidal motion, you can use an equation. How much time are you expecting to simulate? You will find that Transient Structural will rapidly fill up terabytes of space on your HDD.

• nikos
Subscriber

As you can see below I have created a base disk under the tank and have tried to apply a contact (under connections) so that ground and tank interact with a friction coefficient.

I have applied a Fixed Support on the lower surface of the "Ground" (not the one in contact with the tank).

The issue I have encountered, is that I cannot select Boundary Condition under Acceleration -> Base Excitation (Yes) -> Scope ->Boundary Condition.

• nikos
Subscriber

By inserting a Fixed Support under Modal, the Boundary Condition option became available so my setup is as follows:

The new issue that has come up, is that by inserting Modal and Base Excitation, it does not support System Coupling.

If there is any help it would be greatly appreciated.

• peteroznewman
Subscriber

Don't use a Modal pre-analysis. Delete that link and let the Transient be a full transient.

Replace the Fixed Support with a Displacement.  The displacement can be tabular time-history data or the equation that results after you perform a double integration of the acceleration equation.

• nikos
Subscriber

First of all, thank you petereoznewman for all your input.

Secondly, we have made some progress and managed to insert the erthquake as displacements.

The thing is that almost every time we run, we get the following two errors

1. "highly distorted elements error"

2. "Cortex received a fatal signal (SEGMENTATION VIOLATION)"

Any ideas on what might be causing these errors and how to solve them?

Thanks again.

• peteroznewman
Subscriber

1. Where is the distorted element?  The corrective action depends on where it is. Taking smaller time steps might resolve this problem.

2. This sounds like a computer error. How much RAM is installed in your computer?  How much memory does the solver need to solve incore?  You can find this last piece of information by opening the Solver Output under the Solution Information folder.

• nikos
Subscriber

Thank you peteroznewman.

However, please take a look at this:

New error appeared on the analysis run.

"Update-Dynamic-Mesh failed. Negative cell volume detected" time step is 0.002.

ERROR

ZONES/MESH

END OF RUN

We have also tried meshing in structural.

I have attached a wetrasnfer link to a .wbpz file from our analysis if you want to take a look at.

https://we.tl/t-aSQ3EIMxaw

Thank you for all your help.

• peteroznewman
Subscriber

Nikos,

I won't be opening your model as it exceeds the capability of the Student license.

There are several posts on this site about negative cell volume errors in FSI problems.
Search for that term and read those posts. The first thing to try is a smaller time step.

Good luck.
Peter

• nikos
Subscriber

we fixed the time step to be smaller and used an earthquake with smaller displacements.

Our model runs successful as you can see below, but every time the System Coupling is completed it gets stuck and does not really end the procedure.

Do you know some way to fix that issue??

Thanks again