I am trying to use preCICE to numerically investigate the flow dynamics of a density current interacting with a bottom-mounted elastic thin plate. I am thinking of whether InterFoam (the VOF multiphase OpenFOAM solver) can be coupled with CalculiX with the capacity of dynamic meshing. Would it be a similar route to this link (https://github.com/precice/precice/wiki/Tutorial-for-FSI-with-OpenFOAM-and-CalculiX)? Thanks!
interFoam has already been used with the OpenFOAM adapter:
There should be no fundamental problem and the approach would indeed be very similar to the standard FSI tutorial you mentioned.
“Dynamic meshing” sounds a bit more critical. Currently, preCICE relies on static coupling meshes. Meaning that you define them only once during initialization. This is enough if you do FSI based on an ALE approach. If you want to refine your fluid mesh, however, in every timestep and with this also your coupling mesh, then you reach the borders of preCICE currently. We are working on this, however: https://github.com/precice/precice/issues/225
Thanks! Those resources are very helpful.
I have a couple of questions:
Are you referring to the interaction between the different phases in interFoam by saying “fluid-fluid coupling”? Or, if I understood correctly, did you mean “fluid-structure coupling” instead? I plan to use interFoam as the only fluid model without others, e.g., heat transfer.
Does the “static coupling meshes” mean that the fluid mesh cannot change during the simulation in response to the obstacle deformation? What I would like to achieve is something like the figure below (a moving mesh) . I hope PreCICE is capable of this.
By “fluid-fluid coupling” we mean coupling two different flow domains (e.g. two connected pipes). What was meant above is that we have used the OpenFOAM adapter (with some changes about to be merged) with interFoam, so it technically works. You still need FSI with interFoam, which should be possible already (but I would be interested to know if you get any problems, I expect at least a trivial issue with automatically deriving the solver type between compressible and incompressible).
You can definitely get what you see in the picture already. In this picture we are using the Arbitrary Lagrangian-Eulerian method (ALE), where the interface is fixed in the beginning of the simulation (location and number of nodes), but each node gets a displacement that is then used in the calculations. This is the most common approach in FSI right now.
Non-static meshes in this context would mean that the interface is redefined in every time step. This is in our current research plans but you don’t need it in your case.
I can confirm that the preCICE coupling interFoam or interIsoFoam with CalculiX works, but we had to use an adaption of the force estimation for OpenFOAM according maoxm’s fix in https://github.com/precice/openfoam-adapter/issues/127 for preCICE 2.0. Otherwise the forces have been by a factor of 1000 too large, most likely due to an unnecessary multiplication of the pressure with the fluid density which is not required for inter*FOAM even if it is an incompressible solver in OpenFOAM terminology.
I am trying to compile the edited adapter by maoxm, but I am getting the following error:
Adapter.C: In member function ‘void preciceAdapter::Adapter::execute()’: Adapter.C:402:53: error: ‘directory’ is not a member of ‘Foam::fileName’ if (runTime_.timePath().type() == fileName::directory)
I know that maoxm’s adapter is for OF6, and I am currently using OF7.
I also saw this comment by @MakisH in pull request #91 and made the change from
fileName::directory. But I am stuck.
Not sure what else I am missing.
Currently using the OpenFoam7 branch of the OF adapter and preCICE v2.1
In Makis’ pull request it is changed to
fileType::directory (emphasis on fileType instead of fileName). In case you actually have changed it to
fileName::directory you could try to change it to
fileType::directory and compile again.
Thank you sooo much @ajaust.
After a day of errors, my brain was turned into mush. Couldn’t spot such simple thing.
I was able to build the adapter and have the
.so file, and will try and run the
interFoam simulation and hopefully get back with results.
2 posts were split to a new topic: FSI with interFoam and CalculiX: Convergence