Multibody - Fluid Interaction

In this tutorial, you will learn how to setup a model in MotionView that will be coupled with AcuSolve through HyperMesh CFD.

Through this co-simulation interface, you can now solve multi-physics problems that involve complex rigid body movement, coupled with fluid flow, that generates pressure forces on the rigid bodies. This capability lets you enhance the fidelity of your multibody system, letting you generate more realistic results.

In this scenario, MotionSolve computes the displacements and rotations for the rigid bodies, while AcuSolve computes the forces and moments on those bodies. Both solvers exchange data with each other while stepping forward in time via the TCP socket protocol. This means that the two solvers can be located on different machines and on different platforms and still communicate with one another. For example, the CFD simulation can run on an HPC, while the MBS simulation can run locally on a laptop.

Tutorial Objectives

You will use the MotionSolve-AcuSolve co-simulation interface to couple the rigid body dynamics of a check valve within a pipe with the flow field. The AcuSolve model has already been setup for you in HyperMesh CFD.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Steps for running this model in HyperMesh CFD are included as part of this tutorial.

To learn more about how to setup the model in AcuSolve, please refer to Coupled Simulation of a Check Valve using AcuSolve and MotionSolve.

Software Requirements

To successfully complete this tutorial, the following software must be installed. Each software is installed through an installer package.
Software Installer Package
MotionView hwdesktop
HyperMesh CFD hwdesktop
MotionSolve hwsolvers
AcuSolve hwCFDSolvers
Note: All the above software can be installed at once using the Altair HyperWorks Products installer (hw). Please refer to the Installation Guide on how to install Altair HyperWorks Products.

The co-simulation is supported for both Windows and Linux platforms (64-bit). Cross platform co-simulation is also possible.

Simulation Environment

The co-simulation interface between MotionSolve and AcuSolve consists of a “middleware” utility executable, acuMSI.exe. This executable is responsible for:
  • Establishing a connection to both MotionSolve and AcuSolve.
  • Communicating the displacements and rotations from MotionSolve to AcuSolve.
  • Communicating the forces and moments from AcuSolve to MotionSolve.
  • Managing runtime and licensing.
This is shown schematically below.


Figure 1. Co-Simulation setup

Pipe with a Check Valve

A check valve is a mechanical device that permits fluid to flow in only one direction. This is controlled by a shutter body. Fluid flowing in one direction pushes the shutter body in one direction, thereby opening the valve. Fluid flowing in the opposite direction pushes the shutter body in the other direction, which causes the valve to shut and prevents flow reversal in the pipe. Check valves are found in pumps, chemical and power plants, dump lines, irrigation sprinklers, hydraulic jacks, for example.

The geometry that is modeled in this tutorial is illustrated in the figure below. It consists of:
  • A pipe with an inlet and outlet for the fluid flow.
  • A check valve assembly that consists of a shutter plate attached to a stem.
  • A stop mounted on a perforated plate downstream of the shutter body.
  • The fluid flow in the pipe is assumed to be axisymmetric. This allows you to model only a part of the check valve. In this example, a 30-degree section of the geometry is modeled, as shown by the blue part in the figure below. The advantage of doing this is a reduced simulation time while still capturing an accurate solution.


Figure 2. Pipe with check valve model setup

The check valve assembly consists of a disc-like body mounted on a stem. When fluid flows in the direction specified by the red arrows in the figure above, the fluid forces the shutter body to translate in the same direction as the fluid. The motion of the shutter body is also affected by a spring damper attached between the shutter body and the perforated plate. Finally, 3D rigid body contact is modeled between the shutter body and the stop to arrest the motion of the shutter body in the direction of the flow.

For the MBS model, only 1/12 of the shutter body and the perforated plate are modeled.

At the start of the simulation, the flow field is stationary. A pressure specified at the inlet drives the flow, which varies over time as a piecewise linear function. This is illustrated in the figure below. As this pressure rises, the flow accelerates which in turn pushes the shutter body open and allows flow through the pipe.


Figure 3. Inlet pressure

This dynamics of this kind of model can be termed as being “tightly” coupled between the two solvers. This means that the motion of the rigid bodies affects the fluid flow field, which in turn affects the rigid body motion in a cyclical fashion.

The rest of this tutorial assumes that this model has been correctly setup in HyperMesh CFD. Note that the model is designed to translate the shutter body until it collides with the perforated plate. The MotionView model has been designed with a contact between these two bodies that causes the shutter body to rebound appropriately. To allow the rigid bodies to come into contact without the CFD finite element mesh fully collapsing, the perforated plate in the fluid model has been offset by 0.002m in the positive X direction.

Load the Model in MotionView

  1. From the Start menu, select Altair <version> MotionView <version>.
    If the HyperWorks Launcher is seen, click on Create Session to start a MotionView session.
  2. Click and open the model Valve_model.mdl.
    This model is prepared to run in MotionSolve but requires modifications to run in co-simulation with AcuSolve. These steps are outlined below.
    Once the model is loaded into MotionView, the graphical window displays the shutter body, perforated plate, joint and spring entities, as well as a graphical representation of the spring damper as shown in the figure below.


    Figure 4. The MotionSolve model of the pressure check valve
    The MotionSolve model consists of the following components:
    Component Name Component Type Description
    Ground Body Rigid Body Ground Body
    Shutter Body Rigid Body 30-degree section of the shutter body.
    Shutter Body Graphic Graphic The graphic that represents the shutter body. This graphic is used for the contact force calculations.
    Perforated Plate Graphic Graphic The graphic represents the perforated plate belonging to Ground Body. This graphic is used for the contact force calculations.
    Contact 3D Rigid-Rigid Contact Force 3D rigid-rigid contact force between the Shutter body and the Ground Body (Perforated Plate).
    Solver Units Data Set The units for this model (Newton, Meter, Kilogram and Second).
    Note: The units in the MotionSolve and AcuSolve models need not match to run the co-simulation; however, the units must match to overlay the results animations in HyperView.
    Gravity Data Set Gravity specified for this model. The gravity is turned on and acts in the negative Y direction.
    Spring Graphic The graphic that represents the spring modeled between the shutter body and the perforated plate body. This is only for visualization and does not affect the co-simulation results.
    Translation Translational Joint This translational joint allows motion of the shutter body along the X axis.
    Spring Spring Damper This is a simple spring damper mounted between the shutter body and the Ground Body.
    ContactOutput Output An output signal that measures the contact force.
    Displacement Output An output signal that measures the displacement between the shutter body and the ground.
    Velocity Output An output signal that measures the velocity of the shutter body with respect to the ground.

Run the Model without Co-simulating with AcuSolve

To verify that the MotionView model is set up correctly, run the model in MotionSolve and verify that there are no warning/error messages from MotionSolve.

  1. From the Analyze ribbon, click Analysis settings, , to display the Run Motion Analysis dialog.
  2. Provide a Run name Valve_Model_no_cosim.
  3. Specify an Output directory.
  4. Click Run
  5. Review the log by clicking View Log on the Run Status dialog. Verify that the MotionSolve run is complete and there are no errors. Close the Run Status dialog.
Notice that there is no motion in any of the parts. This is because the actuation for this model comes from AcuSolve, which is not yet enabled.

Open the Fluid Model

In this step, you will open the fluid model prepared in HyperMesh CFD.

  1. From the Start menu, select Altair <version> HyperMesh CFD <version>.
  2. Open the model Check_Valve_Coupled.hm from the working directory.
  3. Switch to Case Setup as shown in the image below:


    Figure 5. Case Setup Ribbon
    Note: This model has already been set up for co-simulation. To learn about building a HyperMesh CFD model for co-simulation with MotionSolve, please refer to the tutorial ACUT-5021.
  4. For a successful coupling, the names of the interacting bodies need to match between MotionSolve and AcuSolve.
    1. In the MotionView Model Browser note the hierarchy and label of the Shutter body that will be interacting with the fluid domain. That would be Model-Shutter Body, which is the full label of the body that would be identified by MotionSolve during the simulation.


      Figure 6. Interacting body's label
    2. In HyperMesh CFD, go to the Motion ribbon. Click on the Settings icon under Setup group to display the Setup dialog.
    3. Make sure the External Solver selected is Motion Solve. Retain other settings for socket as default.


      Figure 7.
    4. Click on the External Surfaces icon under the Derived group to bring up the External Code surfaces tool.


      Figure 8.
    5. The Valve surface is already defined for this model. Right-click on Valve-Wall from the list of External Code Surfaces on the left of the screen. This is the fluid surface that would interact with the Shutter Body in the MotionSolve model. Confirm that the text for the Rigid body reads Model-Shutter Body as noted in MotionView previously.


      Figure 9.
    6. Exit the tool .

Set Up Interaction

To couple with AcuSolve, you need to specify one or more "wet" bodies. A "wet" body is a body in the MotionSolve model which interacts with the fluid flow and thus has forces and moments acting on it. Such a body can translate or rotate due to the actuating fluid force/moment as computed by AcuSolve as well as due to any actuating forces/moments in the MotionSolve model. In this example, you will define a single "wet" body – the Shutter body that translates along the X axis due to fluid impinging on it.

To specify a body as "wet" in MotionView:

  1. From the Project Browser, select the body Shutter Body.
    Figure 10. Selecting the Shutter Body
    The properties are displayed in the Entity Editor.
    Note: If the Entity Editor is not visible, turn it on from the View menu.
  2. From the Properties section, select Fluid interaction with AcuSolve
    Figure 11. Enabling Fluid Interaction with AcuSolve

Run the Co-simulation

  1. Verify that the end times for both models are set to the same values. For this tutorial, the end times for both the AcuSolve and MotionSolve runs are set to 0.35s. Also, the print_interval for the MotionSolve model needs to match the step size for the AcuSolve model. It is set to 0.002s.
    1. To verify the motion model, select Default Analysis from Model Browser in MotionView.
    2. From Entity Editor, view the Analysis Parameters.


      Figure 12. Analysis Parameters
    3. Verify that the MotionSolve Max Step Size, h_max, matches the Print Interval (0.002s in this case).


      Figure 13. MotionSolve Maximum Step Size
    4. In HyperMesh CFD, go to the Flow ribbon and click on Physics under the Setup group.
    5. Set the Time step size to 0.002 and Final time to 0.35.


      Figure 14.
  2. There are two methods to execute the MotionSolve solver.
    1. Live through MotionView.

      In this mode, the simulation progress with the motion model can be seen in MotionView through live animation of the model. This method is useful for a model with medium complexity and size, where run times are not large.

      1. From the Analyze ribbon, click on the Analysis settings icon.


        Figure 15.
      2. In the Run Motion Analysis dialog, provide a Run name.
      3. Provide an Output directory.
      4. Click Run.
      5. The Run Status dialog appears and MotionSolve is initiated and will wait for the coupling.
      Note: Based on firewall settings, a pop-up window could appear asking for permissions to start the coupling exe.

      Go to Step 6 to start the run in HyperMesh CFD.

    2. Offline through Altair Compute console.

      This method is useful for large CFD models that needs to solve on a cluster with higher computing power.

      1. Export the solver deck to your working directory, click File > Export > Solver Deck.


        Figure 16. Exporting the model to .xml
      2. Select Simulation Only and Format as XML.
      3. Provide a file name and click Export.
      4. From the Start menu, select All Apps > Altair <version> > Compute Console and select MotionSolve as the solver. Locate the model you just exported by clicking on the file open icon.


        Figure 17. Select the exported model from disk
      5. Click the ellipsis button next to the Options field to open the Select Solver Options dialog.


        Figure 18. Selecting the co-simulation flag
      6. Activate the –as_cosim option. When you activate this option, the following dialog is displayed and you are prompted for additional options:


        Figure 19. Specifying options for the co-simulation
        You may specify the following options here:
        acuMSI Options
        -aport <integer>
        Specifies the communication port number for communication between AcuSolve and acuMSI. The default is 48000.
        Note: If you need to change the default port for communication between AcuSolve and acuMSI, in addition to changing this argument, you also have to specify the changed port number in the AcuSolve input file.
        -mport <integer>

        Specifies the communication port number for communication between MotionSolve and acuMSI. The default is 94043.

        Note: If you need to change the default port for communication between MotionSolve and acuMSI, in addition to changing this argument, you also have to specify the changed port number in an environment variable MS_AS_PORT. MotionSolve checks for this environment variable at the start of the simulation and changes its listening port accordingly.
        -mi <integer>
        Specifies the maximum number of iterations per time step between the two solvers. The default is 0.
        -v <integer>
        Specifies the verbosity level of the output file from acuMSI. The default is set to 0 (verbosity OFF).
      7. To retain the default options, click None.
      8. Click Apply Selected and Close.
      9. You are now set up to start the co-simulation on the MotionSolve side. Click Run.


        Figure 20. Run the MotionSolve model
      This launches MotionSolve as well as the acuMSI executable. The MotionSolve run is paused at the first time step – it is now in waiting mode and the co-simulation will start as soon as AcuSolve is run.


      Figure 21. The MotionSolve simulation is waiting for a connection to AcuSolve

Run the AcuSolve Executable for Co-simulation

  1. From the Solution Ribbon tab in HyperMesh CFD, click the Run icon to invoke the Launch AcuSolve dialog.
  2. Set Problem name as Check_Valve_Coupled.
  3. Make sure that Problem directory is set to your current working directory. Use the Browse button to search for your working directory folder.
  4. Set AcuRun path as .../~altair_install/hwcfdsolvers/acusolve/win64/bin/acuRun.bat, found in the installation.
  5. Click Run to initiate the simulation in AcuSolve.


    Figure 22. Launching AcuSolve for the co-simulation

    As the solution starts, the Run Status dialog is opened, where you can watch the simulation’s progress. HyperMesh CFD generates the input files and launches AcuSolve.

    Soon, AcuSolve and MotionSolve should begin to communicate with one another. You should be able to see relevant time stepping information in both solver windows. For example, you should see something like the following in the MotionSolve window at the beginning of the co-simulation:
    INFO: [AS-COSIM] Connected to AcuMsi on port 94043
INFO: [AS-COSIM] License checked out.
…
Time=2.000E-06; Order=1; H=2.000E-06 [Max Phi=1.314E-16]
Time=3.600E-02; Order=2; H=2.000E-03 [Max Phi=1.653E-08]
…

    The co-simulation should take roughly 15 minutes to complete on a laptop (Intel i7. 2.8GHz).

    Note that there is no order dependency on launching the co-simulation – either MotionSolve or AcuSolve can be launched first.

Post-process the Results from the Co-simulation

HyperView and HyperGraph can be used to post-process the co-simulation results within a session.

The animation H3D generated by the MotionSolve part of the co-simulation contains only the results from MotionSolve. Similarly, the result files from AcuSolve only contain the results for the AcuSolve model. To animate the results from the co-simulation, follow these steps:
  1. Add a page to the MotionView session by clicking on the session page list drop-down on the toolbar at the top right corner and click +.


    Figure 23.
  2. Change the client of the newly added page to HyperView either from the menu bar or the top right of the modeling window.


    Figure 24.
  3. Load the animation H3D generated by MotionSolve in HyperView.
    1. Click on the Open icon to display the Load model and results panel.
      Note: If the panel is not visible, turn on the panel from the View menu.
    2. Click the file open button, , next to Load model and navigate to the results directory (the same directory where the .xml file is located).
    3. Select the .h3d file and click Open.
    4. Click Apply.


      Figure 25. Loading MotionSolve H3D in HyperView
  4. Click the Play icon on the Animation toolbar to animate the motion result.
  5. To load the AcuSolve results, they must first be converted to the .h3d format. This can be accomplished by using the Convert tool in HyperMesh CFD.
  6. In the Solution Ribbon, click on the Convert icon .
  7. Use the Browse button to load the solver’s .Log file as the AcuSolve log file parameter.
  8. Select H3D as the Output Format from the drop-down menu.
  9. Select all variables in the Variables section, by clicking on a variable and using ctrl + A on Windows.
  10. Similarly, select all Time Steps.


    Figure 26. Generate AcuSolve H3D file
  11. Click Convert. This creates a single .h3d file containing all the time steps available for the simulation.
  12. Using HyperView, overlay the newly-created H3D over the MotionSolve result H3D in HyperView. This is accomplished by repeating Step 1 described above and activating Overlay when selecting the AcuSolve result H3D.


    Figure 27. Overlaying AcuSolve H3D over the MotionSolve H3D in HyperView
  13. Click Apply.

    Once loaded, the modeling window contains both results and can be animated as before. To visualize the information contained within the AcuSolve results, a Contour plot may be used.

  14. Click on the Contour button to display the panel.
  15. Set the options as shown in the figure below and click Apply.


    Figure 28. Visualizing flow velocity using Contour
    This creates a contour plot of the velocity magnitude overlaid with the results from MotionSolve in one window.


    Figure 29. Velocity magnitude plot overlaid with the MotionSolve results in HyperView
Plotting the MotionSolve Results in HyperGraph

You can also interpret the results with a two-dimensional plot using HyperGraph. Use the multi-window layout, allowing both HyperView and HyperGraph to be open at the same time.

  1. From the top right corner, click the Set Page Layout button and split the page into two vertical pages.


    Figure 30. Splitting the page into two vertical pages

    This automatically adjusts the modeling window to accommodate two pages, defaulting to two instances of HyperView.

  2. Click anywhere in the page on the right and switch to HyperGraph by clicking the Client Selector to select HyperGraph from the drop-down list (as shown in the figure below).


    Figure 31. Open HyperGraph
  3. Click the Open Plot button to load the .plt file from the same results directory.
    Once the .plt file is loaded into HyperGraph, the two outputs are available for plotting.
  4. In the Y Source tab, perform the following selections:
    1. Under Types, select Displacement.
    2. Under Requests, select REQ/70000002 Shutter Body from Ground Body(Displacement).
    3. Under Component, select X.
    4. Click Plot.
    HyperGraph can be used to create additional traces on the same plot to generate the following plots.


    Figure 32. Select the signals for plotting


    Figure 33. Visualizing Shutter body results