Learning Forum

[arnau994]

Hello,

I am running a FSI model with LS-Dyna R11.2. After intersecting nodes and creating elements for the ICFD mesh, the following error appears:

"Error 120003 (ICFD+3)"
"ICFD ERROR:: mesh error.Possible surface collapse 3".

I am aware that this error has already been discussed here, and the solution given was to check the "icfd_tmp_sm" file. However, in my case, when I check this file, it only displays the surface mesh that I have already created, and the collapse can not be located in it. The mesh has been checked in my pre-processor and it has passed all the correspondent checks (free edges, element intersection, coincident nodes/elements,...).

What causes could be triggering this error?
Does LS-Dyna have difficulties in volumetric meshing from surface mesh in specific geometries?
Is the "3" displayed in the error relevant?
In some simulations, the error is written with symbols and numbers instead of only letters. Might this be a possible hint?

I have run several iterations and simplifications of my model, and I have only been able to run a pure ICFD simplified model with 60,000 (surface) elements, which after 4 days, has simulated 0.15s out of 1.2s. I understand that these runtimes are not usual for an engineering-prepared workstation...

I am sorry for so many questions, but this has been following me for more than two weeks already. I really hope someone can provide me some advice or guidance on this.

Thank you very much for your time and help!
Arnau

[Reno Genest]

Hello Arnaud,

I did not find any information on this error message in our knowledge database. I will ask the developer.

In the meantime, could you post a screenshot of your surface mesh?

Maybe your geometry is "thin" and the surface mesh is not fine enough to get a volume mesh? Try refining the surface mesh and use a similar volume mesh size using *MESH_SIZE and *ICFD_CONTROL_MESH.

Also, do you have boundary layers? Adaptive meshing? Or other features in your mesh? I would try to simplify the mesh controls as much as possible and see if you can get a successful mesh. Then, add complexitties one-by-one. 

As a workaround, you could use your own volume (tet) mesh. Here is more information from the ICFD training course:

"Usermesh
•
First modification: Since the volume is now directly built by the user, the fluid nodes
and elements no longer correspond to surfaces but are directly linked to the fluid
volume
•
Consequently, The *MESH_SURFACE_ELEMENT and *MESH_SURFACE_NODE cards are
now replaced by respectfully the *MESH_VOLUME_ELEMENT card which works in a
similar way as *ELEMENT_SOLID in 3D cases and as *ELEMENT_SHELL in 2D cases, and
the *MESH_VOLUME_NODE card.
•
The *MESH_VOLUME keyword is no longer needed.
•
The Part ID associated to the *MESH_VOLUME_ELEMENT keyword is associated to a
*ICFD_PART

In order to define boundary conditions *ICFD_SET_NODE_LISTs have to be defined and
associated to the *ICFD_PARTs. The format of this keyword is similar to SET_NODE_LIST
*ICFD_SET_NODE_LIST
SID
: Node Set
PID
: *ICFD_PART ID associated to the Node

"

 

Reno.

[arnau994]

Hello Reno,

Thank you very much for your detailed response and the feedback the developer will provide.

I have attached below one of the surface mesh iterations, where I tried a coarser mesh on the wing (FSI interaction surface) and a finer mesh on the fluid domain to balance both element sizes. At the moment I don't have any boundary layers, adaptive meshing or any other kind of features (I think that the boundary layer is volume-meshed automatically?). I have also tried to attach the .k file with only the mesh in case it could be helpful, but I have been unable to do so.

To be honest, I didn't try to deep-refine the mesh, as I understood that a higher element count would be detrimental for the solver. I will try it and keep you updated. Same for the volume mesh workaround.

Thank you for your time. I really look forward to hear from the developer.

Arnau

[Reno Genest]

Hello Arnaud,

Make sure the surface mesh is watertight; the surface mesh should fully enclose the volume mesh with no holes or gaps. Also, the mesh has to be conformal.

Have you tried to use all triangles for the surface mesh? 

Also, the boundary layer is specified for the volume mesh using *MESH_BL. Make sure you don't have special mesh features that could complicate the mesh. Start simple and have a successful volume mesh. Then, add complexities one-by-one.

If you have access to the Ansys Learning Hub (ALH), you can acces the ICFD training course:

https://jam8.sapjam.com/groups/QyHAlhciRCZ0Xt6xKZ2MHi/overview_page/jPMouxqQ2AOP6jVZLBMZCl

Note that Ansys employees are not allowed to upload or download files on the Ansys Forum. So, I cannot look at your model, but maybe another user could.

If you are a commercial customer, you can create a support case on the Ansys Customer Support Space (ACSS) and we will have a look at your model:

customer.ansys.com

 

Let me know how it goes.

 

Reno.

[Reno Genest]

Hello Arnaud,

Which version of LS-DYNA are you using? The developer said that this error message is only in R12. The developer also suggested the following:

"It seems there is intersection of the initial surface mesh. I would suggest the customer switch to a later version of DYNA, the error message after R13 has improved and should show more and clearer information to the user.

For the latest version it can show the location of the intersection so it is easier for the user to find where goes wrong."

 

Reno.

[arnau994]

Hello Reno,

I can confirm my mesh is watertight and conformal with the solid body.

I have just tried to run it with Tethaedrons (triangles) and it seems that it has meshed successfully! However, the running time for the ICFD-only is still very low (2e-6s steps every 3min for a 80,000 elements on the surface mesh). Can you confirm this run time should be expected for an engineering-prepared workstation? Maybe there is still something wrong?

On the other hand, my LS-Dyna version is R11.2. It is good to know that future versions can locate the error, but unfortunately, license is provided by my university and I am afraid I can't ask for a newer version.

In any case, are these runtimes common?

Now that at least I can run the model, I can keep working on it. Thank you very much for your time and help in this, it is very much apreciated!

I hope you have a great day.
Arnau

[Reno Genest]

Hello Arnaud,

If DT=0 on *ICFD_CONTROL_TIME, then the CFL timestep calculated by the ICFD solver is used:

 

You could try to use a larger DT by specifying the timestep you want to use (DT=5e-6 for example) and see if the results are still good. 

Also, you could try to increase your mesh size a little bit.

Finally, it is recommended to use MPP LS-DYNA to run in parallel on many cores. 

 

Reno.

 

[arnau994]

Thank you Reno, your help has been invaluable. I hope you have a good day.

Arnau

[Reno Genest]

You're welcome! Have a good day too!

 

Reno.