Fluid–Structure Interaction Using System Coupling

Posted on by

With the release of ANSYS 14.0, ANSYS Fluent users can perform two-way fluid–structure interaction (FSI) simulations using the ANSYS next-generation coupling technology — system coupling.

The system coupling component in ANSYS Workbench offers a generic way to couple two or more participants in the Workbench environment. In release 14.0, you can link Fluent and ANSYS Mechanical via system coupling to facilitate FSI simulations.

This post provides a broad overview of the capabilities offered with system coupling and the types of cases you can solve. I’ll try to avoid just listing the features.In ANSYS 14.0, system coupling lets you perform cosimulation, one-way and two-way  force/displacement coupling between ANSYS Fluent and ANSYS Mechanical. Let’s look at what some of these terms signify. Cosimulation means that both solvers run simultaneously, exchanging data when needed without writing out intermediate results files. This is in contrast to static data transfers, in which one solver has already produced and written out its results. Static data transfers aren’t available yet using system coupling; but various approaches are available in previous releases. With cosimulation, data can be passed in one direction (one-way) or in both directions (two-way). A one-way cosimulation may pass force data to ANSYS Mechanical, but no displacements pass back to Fluent. On the other hand, a two-way simulation passes data in both directions. Lastly, force and mesh displacement are the variables that pass between the solvers for the current release.

When executing two-way FSI runs, coupling iterations are performed within each time step to converge the data transfers, which results in an implicit solution at convergence. This is termed an iteratively implicit approach to coupling. Implicit coupling is important, since an explicit approach typically requires a much smaller time step. Even after taking into account the extra iterations you perform with an iteratively implicit approach, run times are typically much shorter than with an explicit approach. The iteratively implicit approach also makes the solution more stable.

Stability at the fluid–solid interface can be a big concern with FSI simulations that use separate fluid and structural solvers, particularly when the structure is very flexible and the working fluid is a liquid. Biomedical cases, membranes, diaphragms and thin-walled structures often exhibit instabilities at the FSI interface. With system coupling, you can solve these types of cases without resorting to excessive underrelaxation or small time steps. For more details on this, enter “2022119″ in the “Search the Knowledge Resources” box on the ANSYS Customer Portal, or just search for “FSI.”

For those of you familiar with the ANSYS CFX with ANSYS Mechanical two-way FSI method, the new system coupling approach using Fluent adds fluid remeshing capabilities to FSI simulations. This allows you to solve FSI cases that would otherwise cause the fluid mesh to collapse.

For more information on system coupling, look for the upcoming ANSYS Fluent with ANSYS Mechanical FSI training course. This will include one-way and two-way FSI between using system coupling. Watch for this in the ANSYS Training Center in the next few weeks.

39 thoughts on “Fluid–Structure Interaction Using System Coupling”

  1. Thanks for your post,
    I have some question in using coupling system, may I ask you my questions?

  2. It seems to me that in R14, Fluent is getting all of the attention and new features. Is CFX being pushed to a second class citizen in WB?

    • ANSYS CFX prior to R14 had an established FSI solution using the MFX solver, while Fluent was clearly missing an easy-to-use 2-way FSI solution — so the new release upgrades Fluent. We concentrated CFX development in R14 on new advanced turbomachinary features (e.g. Transient Blade Row analysis). While CFX does have an existing FSI solution, the value in adding CFX to System Coupling is recognized and is currently under consideration.

  3. Hi, i would like to know how to couple fsi problems using fluent and mechanical APDL without workbench.

    • To do this you’ll be running from the command line. Some details are in the Workbench documentation ( // System Coupling User’s Guide // Workflows for System Coupling // Executing System Couplings Using the Command Line) but I’ll provide more details here. I’ll assume you’re on Windows for now.

      1. Create the MAPDL db file, Fluent cas file and System Coupling sci file. Creating the sci file is described in the documentation link above.
      2. Create a simple Fluent journal file that starts Fluent in batch, reads the cas file and solves.
      3. Create a simple MAPDL solver input file that resumes from the db file and solves.
      4. Start the coupling service:
      set PATH=%AWP_ROOT140%FrameworkbinWin64;%PATH%
      “C:Program FilesANSYS Incv140aisolbinwinx64Ansys.Services.SystemCoupling.exe” -inputFile -coupling.sci
      5. Note the port and hostname in the scServer.scs file that gets created.
      6. Starts the Fluent solver, e.g:
      “C:Program FilesANSYS Incv140fluentntbinwin64fluent.exe” 3ddp -hidden
      -driver null -scport=12345 –schost=hostname -scname=”Solution“ -i fluidflow.jou > FLUENT.out
      7. Start the MAPDL solver, e.g:
      “C:Program FilesANSYS Incv140ansysbinwinx64ANSYS140.exe” -b -scport 12345 -schost hostname -scname “Solution 1″ -i structural.dat -o ANSYS.out

  4. My topic is about TLD(tuned liquid damper). please inform me , does ansys have analysis capability of TLD attached to structure? if yes, can i use from couple as boundary condition between fluid and structure? if you send to me each information about this, i am so grateful.

    • In general you would be able to simulate TLD’s using System Coupling between Fluent and Mechanical. If the motion of the liquid tank walls is known ahead of time and the walls can be treated as rigid, then can just solve this in Fluent by imposing the boundary motion. Using System Coupling would be appropriate if the walls cannot be treated as rigid and/or the motion of the tank walls is more complex, in that it depends on the structural response. In Fluent the Dynamic Mesh boundary condition would be “System Coupling” while in Mechanical a Fluid Solid Interface would be defined. I could send a tank sloshing case via a support request on the Customer Portal (please mention this post in the support request).
      Best regards, Mike

  5. I have some problems in performing 2 way FSI using ANSYS CFX and ANSYS structural. I am trying to simulate a FSI for simple straight elastic tube with time varying velocity at inlet and time varying pressure at outlet. The wave speed is 5m/sec wit struc properties (1150 Kg/m3 density, E=5e5 and Poisons ratio=0.48) and fluid properties (density = 1050Kg/m3 and dynamic viscosity of 0.004Pa.s).

    Please give some hints, I tried a lot to explore the FSI, but still there are some problems. I was able to get the FSI simulation to some extent. But, problem is in structural the deformation at some points occurs in X-direction rather than radial expansion, but during some instants its radial.

    Also sir in some of the blogs, the density is expressed as slightly compressible by using expression density1=density+P/36 in CFX, may I know how did this 36 value is obtained from..?

    • It would be best to handle this case through a technical support request. I’ll ask a local support engineer to follow up with you.
      Best regards,
      Mike

      • Thanks Michael,

        I have brought this to notice of local tech support. They have also tried and we both have worked on this. But still there are few problems.

        FSI simulation of a straight tube, when subjected to inlet vel and outlet pressure for fluid and for structure, inlet and outlet nodes are fixed.
        For this nature of BC, we naturally expect uniform radial expansion, but in results we observe the bending, similar to buckling of slender structure.

        I tried using cylindrical coordinate system for both fluid and structure, but the results are same.

        Please suggest what can be the reason for this behavior.

  6. Can rotating solid interaction with slurry(multiphase) be done using this feature. I need lot of help in this…if you have a step bystep tutorial, it would be helpful..

    • Do you really need FSI for this? In general you would use FSI when the structural deformations are significant enough to change the flow field. If you have a rotating impeller that is mixing a slurry flow then the only reason to consider FSI is if the impeller bends/deforms due to the fluid forces, otherwise you should just use a rotating frame of reference.

      • Actually I am simulating the polishing operation whereby the slurry with solid particles deform the rotating wafer(pressed downwards with a certain force)…i tried using the embedded reference frame for 3d wafer rotation and pad rotation and in between the slurry but results are not convincing.So I thought of using immersed solid interaction..can u provide a simple step by step tutorial for multiphase slurry interacting with rotating solid which is non axisymmetric…or suggest any simple tutorial to simulate the above said model…pls help in this regard..

      • We don’t have a tutorial for such a specific application. It would be best to get some more detailed guidance for this case through a support request. Could you please log a support request via the Customer Portal or your Channel Partner for this case.
        Regards.

  7. I am teaching a course that uses ANSYS and would like to cover how to perform coupled fluid structure interactions. Is there a good step-by-step tutorial for some example problems available anywhere, or any powerpoint presentations?
    Thanks.

    • The Workbench documentation contains a tutorial (under Workbench > System Coupling), but the Fluent-Mechanical FSI training course material would likely be of more use to you. That should be posted on the Customer Portal in April.

  8. A simple question about parallellization of FSI simulation, it was a simple task in MFX by simply testing and assigning e.g. 4 cores to CFX and 2 cores to Mechanical but I could not find a way to this in Systemcoupling. Is there a way to manually find an optimal setup for arbitrary FSI case?

    thanks

    • Running Fluent and/or Mechanical in parallel with System Coupling is exactly the same as running them in parallel when not connected to System Coupling. To find the best mix, you can look at the CPU time required by each solution and judge which will benefit most from more cores. Keep in mind FEA solution time will not scale as well as CFD when adding more cores.

  9. I work with FSI in Ansys 14.0 using System Coupling, which makes the interaction part of the structure (Transient Structural) with the Fluid Flow (Fluent). But my problem is with the dynamic mesh (Remeshing), it doesn’t work. So the System Coupling gives error, because the mesh of the Fluid.

    The message de error: “Update failed for the Solution component in System Coupling. System coupling run completed with errors. Additional information: One or more elements have become highly distorted. Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere. Try ramping the load up instead of step applying the load (KBC,1).”
    Or
    “Update failed for the Solution component in System Coupling. System coupling run completed with errors. Additional information: Fluent encountered fatal error after sync point Solve”

    Please, can you help me? Thanks.

      • Thanks.
        But a question: is there support in ANSYS 14.0 to do remeshing in case two way FSI?

        Regards,
        Ana.

        • Yes, you can use remeshing in Fluent. The FSI interface surface mesh cannot change, but the interior elements can be remeshed.

          Regards,
          Mike

          • Thanks.

            But I am using System Coupling: the structure (Transient Structural) is deformed with the flow of water (FLUENT). So is it possible to use the Remeshing in Fluent yet?

            Good day!

            Thanks.

            Regards,

            Ana.

  10. Hello Michael,
    I am trying to get the natural frequencies and mode shapes of two problems a tank filled with water (free surface) and a tube filled with water. I did similar problem long time ago from APDL using the FLUID80 element. I am not sure how to do this in workbench. It doesnt seem to give me the option to choose the element type. I tried to couple modal analysis with CFX but it didnt work. Any advice?

    • Hi Ahmed,
      if you couple with CFX then you’ll have to solve in the time domain rather than performing a modal analysis, so I would not recommend this approach unless you need to accurately model the free surface sloshing. I would recommend the approach used here:
      http://www.idac.co.uk/enews/articles/Analyzing_Vibration_with_Acoustics.pdf
      which is likely very similar to what you did in the past with FLUID80 elements. To select the element type in Workbench/Mechanical you can insert a Command Object below the Solid or Surface bodies in the Geometry branch of the Outline tree. The Mechanical support team should be able to assist further if needed.
      Regards,
      Mike

  11. Good evening Mr. Mike i have query reg. the fluent import and CFX import of case files when a fluid,soild(eg: nozzle) is meshed using a gambit software and imported into a workbench it takes the fuid volume, solid volume mesh & mesh interfaces are they really required for the analysis of FSI or i need to merge the fluid and solid volume?

    • The solid side should not be meshed in Gambit, otherwise it’s difficult to get that mesh into Mechanical for an FSI analysis. I would recommend you mesh the solid in Workbench.

    • This looks possible. In the initial position you’ll need a small gap between the bottom of the solid and the bottom of the container, with a Fluent mesh in that gap. Also use a finite thickness for the solid; do not use shell elements and a wall/wall-shadow in Fluent otherwise you’ll have to map two Fluent surfaces to one Mechanical surface, which is not yet possible.

      • Here is my system coupling simulation process, which is a loading tire on the ground(using Transient Structural) and water flow through the tire(using Fluent).
        https://picasaweb.google.com/108705680307294891973/May122012#5741544495269856882
        Tire’s material is nonlinear material. It increase ground area after loading.
        When loading tire without system coupling, it would be fine.
        But it always shows occurrence of negative volume in tire or water when using system coupling.
        Is mesh quality too bad cause this problem?
        Or some additional boundary conditions should be set?
        Thanks for help.

        Honda

        • Some debugging would be needed here. A folded mesh is a common problem and could be caused by many things. The Fluent FSI training material has just been posted to the Customer Portal in the Training Materials > ANSYS Fluent section. The lecture on System Coupling convergence and the workshop on debugging common errors would both be useful here.
          Regards,
          Mike

  13. Mike,

    I want to thank you for the recent tutorials you posted. They are excellent reading and very informative. One thing was puzzling to me, however, in re-running the ‘Hyperelastic Flap’ case – the flap does not deflect in the direction of the flow as described in the lectures w/in the integration time. It only compresses longitudinally instead of bending with the flow as anticipated. Do I need to run the case longer to get it to bend as shown in the lecture? It seems odd that the Lagrange flap doesn’t appear to move with the transverse flow at all.

    Best Regards

    • In my download of the solved example, the symmetry normal for the flap was prescribed on the x-axis instead of z for the mechanical setup. Changing this to the z-axis fixes the result.

Comments are closed.