[katweasle]

Hello everyone,

maybe someone's here who could help me by solving my specific problem, that would be great. I insert a sketch of the 2-dimensional situation.

There is an outer-tube made of metal. The tube is filled with water. In the center of the water-filled tube there is a round piece (core) made of aluminium. Now i want to move the core to the left side so that the water flows from the left space between the tube and the core to the right side).
So far the simulation is not a problem for me. Its a typical two-way fluid-strucure interaction. (transient structual--->fluent coupling in workbench).

But now it want to simulate, that the core hits the outer-tube after pressing the water from the compressed space on th left, to the right side.
In my opinion now it turns into a 3-way structure-->fluid-->structure interaction. Does anyone have experiences with that kind of simulations?
Maybe someone could help me by solving this problem. In the best case someone could provide me an workbench coupling ansys file of that (or of a similar) situation. I would be very happy if someone could help.

Bye

[Fole]

There is a tutorial on the Internet for structure-fluid and in the user manual of ANSYS itself.

From that, I think you need to couple systems. So if you want another structure, another system would be added.

Nevertheless, I have never done any FSI simulation.

Regards.

[Gweher]

Hi,

It doens't really change compared to the standard approach that you mentioned. With FSI you have either 1-way (weak coupling) or 2-way (strong coupling). The first scenario you assume that the feedback of the fluid on the structure can be neglected, and in the second case you take that into account.

If you want to simulate the additional interaction between the inner structure and outer structure its just an additional calculation in your 2-way FSI. So when you say: "Its a typical two-way fluid-strucure interaction. (transient structual--->fluent coupling in workbench)", you're maybe referring to a 1-way FSI instead of a 2-way that's maybe why you end up with the 3-way FSI

The tricky part would be to remesh when your 2 solid will be in contacts as the mesh volume of fluid in between will become infinitively small. It all depends on the accuracy that you want.

[katweasle]

Ok, so i will call it 2-way fluid-structure interaction with an additional structure-structure interaction.
Excatly, that the infinitivly small fluid mesh will be one big problem when the aluminium core and metal tube get in contact.
In my current simulation the contact between the core and the tube doesn't take a place and i still have problems with negative cells in the fluid mesh.
Further i don't have an idea how to setup the collisions between the core and the tube.

[Gweher]

Well if you have negative cell elements it can mainly come from 2 things. First the mesh present really small elements that become highly distorted, or your time step is too large -> large mesh displacements which can also lead to that error.

Can you add some pictures of your mesh ?

[malekan.cfd]

Dear Gweher,

I'm involving in a 2-way FSI problem simulation (transient structural + Fluent) which includes big structural deformation. I have used very small time step for transient structural part as well as system coupling part. However, system coupling delivers "highly distorted elements error" every time I run the problem. When I run the transient structutal alone, everything is OK. But, when I run system coupling it return highly distorted elements error for the first iteration, even for very small time steps (1e-6 sec). The loading is a distributed pressure with a magnitude of 4000 Pa. But, even with magnitude of 1 Pa, I still get the same error. Do you know how can I solve this problem?

Thanks,
Malekan

[katweasle]

Thanks for your answer. I will make a screenshot of the mesh whem i'm back home.

@Gweher

So my remeshing of the fluid mesh woks pretty fine. But when the core hits the pipe, like you already said, i'm getting the error "negative cell volume detected". Is there any possibility to adapt the remeshing settings, so that the mesh "leaves" the fluid area where the core hits the pipe? When not its obvious that the mesh cells will cause an "negative cell volume"-error.

Would be so great if someone could help me.

PS: I saw that video on youtube. Its the same kind of that problem of an collision of two objects under water. But when you look at the contact area you can see that theres still an smal fluid area between those objects in the contact point

https://m.youtube.com/watch?v=hy1yaRr5TMA

But i want an real collision with "NO" fluid-mesh in the contact point
With other words, is it possible to displace the mesh completely from the contact region. So that there won't be any fluid mesh any more?

[katweasle]

I added two pics of the mesh after gettin the "negative cell volume"-detection.

[Gweher]

Hi,

The video presents a similar problem as yours, but I think that in his case he’s using contact with a given pinball region so he doesn’t end up with infinitively small fluid elements. The pinball region allows you to specify a specific “interface search” between contact pairs. If in addition you want to “remove” the fluid in the contact region you can use the EKILL / EALIVE APDL commands that allow you to activate / deactivate elements during the simulation.

In your case I would first start with investing a bit of effort in the mesh derivation. For the central cylinder you should use a simple Ogrid, and I would use a small inflation layer for the fluid in contact with the cylinder. This will help you further on in the simulation process.

Another option could be to take advantage of overset mesh. This was released with Fluent 17 but if I remember well the dynamic mesh option was a beta feature, maybe something to check.

Have fun

[katweasle]

Thank you very much @ Gweher. That was exactly what i was looking for. The gap between the core and the pipe effects no negative cell volume any more when they contact each other. Thanks a lot!!

Now i have one more question and i hope for help again. I added a pic of the new situation. on top of the core i added an flapping rubber plate. so now when the core moves to the left the fluid stream passes the rubber plate and the plate starts to flap from left so the right (the intensity of the "flapping" depends on the rubber material properties and the velocity of the core movement, thats clear). So far i get the system coupling (transient structural and fluent) to work, BUT, only when the rubber is that stiff, that there is just a little flapping movement. When i increase the the flapping movement by increasing the core speed i'm getting an "error 2", negative cell volume. No matter what i'm doing, theres always an negative cell volume error. I was trying to simulate the movement in the transient structural mechanic only by putting an instant or ramped pressure force on the plate, everything works!. Then I changed the fluid mesh, i changed the fluent settings, i increased the transient structual calculation steps. I increased the coupling steps....and so on.

Now matter what, always "negative cell volume detected" after a few calculation steps. I nearly tried all i can, but i just can do it.
I made the calculation steps that small that the movement of the plat should be very very small each calculation step so that the fluid mesh should have enough time to remesh (the fluid remeshing works fine in the core-tube region), but it seems not to work in the near region of the plate. Like i already said, i tryed so many mesh sizes and changed so many settings, nothing works for me......

....please please help!