ACU-T: 1000 Basic Flow Set Up

This tutorial introduces you to the workflow for setting up a Computational Fluid Dynamics (CFD) analysis using Altair HyperWorks CFD. HyperWorks CFD is a powerful tool which provides a streamlined platform for performing a CFD analysis, starting from importing CAD through solving using Altair AcuSolve. In this tutorial, you will learn how to use HyperWorks CFD for setting up a CFD analysis while exploring different capabilities available within the software for importing a geometric model, validating the geometry, setting up simulation parameters and boundary conditions, and generating a mesh. You will then launch AcuSolve simulation directly from HyperWorks CFD and post-process the results using Altair HyperView.

Prerequisites

To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Prior to running through this tutorial, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T1000_manifold.x_t from HyperWorksCFD_tutorial_inputs.zip.

Analyze the Problem

An important step in any CFD simulation is to examine the engineering problem at hand and determine the important parameters that need to be provided to AcuSolve. Parameters can be based on geometrical elements, such as inlets, outlets, or walls, and on flow conditions, such as fluid properties, velocity, or whether the flow should be modeled as turbulent or as laminar.

The system being simulated here is a manifold pipe, analogous to an inlet manifold in an engine. An inlet manifold distributes the incoming flow to multiple outputs. As can be seen in the image below, the pipe has a single inlet and multiple outlets, thus distributing a fraction of the flow among each outlet. Ideally in an inlet manifold used in an engine, the manifold design is such that it ensures near-equal distribution of flow among all the outlets. However, the geometry being used here is purely a demonstration case and not an optimized manifold geometry.


Figure 1. Schematic of the Problem

Start HyperWorks CFD and Create the HyperMesh Model Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperWorks CFD.
    When HyperWorks CFD is loaded, the Geometry ribbon is open by default.
  2. Create a new .hm database in one of the following ways:
    • From the menu bar, click File > Save.


      Figure 2.
    • From the Home tools, Files tool group, click the Save tool.


      Figure 3.
  3. In the Save File As dialog, navigate to the directory where you would like to save the database.
    This will be your problem directory and all the files related to the simulation will be stored in this location.
  4. Enter a name for the database (eg. Manifold) then click Save.

Import and Validate the Geometry

Import the Geometry

Before you start this step, copy the input file, ACU-T1000_manifold.x_t, to your problem directory.
  1. From the menu bar, click File > Import > Geometry Model.
  2. In the Import File dialog, browse to your working directory then select ACU-T1000_manifold.x_t and click Open.
  3. In the Geometry Import Options dialog, leave all the default options unchanged then click Import.


    Figure 4.
  4. Once the geometry is loaded, rotate and observe the features of the model.
    The view of the model displayed in the modeling window can be controlled using the following view controls.
    Button View Control
    Middle mouse scroll Zoom in and out
    Right-click hold and drag Pan the model
    Middle mouse click hold and drag Rotate the model


    Figure 5.

Validate the Geometry

  1. From the Geometry ribbon, Cleanup tools, click the Validate tool.


    Figure 6.
    The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

    The current model doesn’t have any of the issues mentioned above. Alternatively, if any issues are found, they are indicated by the number in the brackets adjacent to the tool name.

    Observe that a blue check mark appears on the top-left corner of the Validate icon. This indicates that the tool found no issues with the geometry model.


    Figure 7.
  2. Press Esc or right-click in the modeling window and select Exit from the context menu to exit the tool.
  3. Save the database.

Set Up the Problem

In this step, you will set the general simulation parameters such as equation, solver settings, etc. Then, you will assign the surface boundary conditions and material properties to the fluid domain.

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, Setup tools, click the Physics tool.


    Figure 8.
    The Setup dialog opens.
  2. Click the Time setting and ensure that Steady is selected.


    Figure 9.
  3. Click the Flow setting.
  4. Check that the flow type is set to Turbulent.
  5. Select Spalart-Allmaras as the Turbulence model.
    The robustness and accuracy of the Spalart Allmaras turbulence model makes it an excellent choice for simulation of steady state flows.


    Figure 10.
  6. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.


    Figure 11.
  7. Exit the Setup dialog.

Assign Material Properties

  1. From the Flow ribbon, Domain tools, click the Material tool.


    Figure 12.
  2. From the modeling window, click anywhere on the manifold.
    The entire manifold geometry is highlighted and a Material microdialog appears.


    Figure 13.
  3. Click the drop-down menu and select Water from the list of materials.
  4. On the guide bar, click to execute the command.
    The changes made in the tool are not effective until they are executed by clicking the icon.
    Once the command is executed, the color of the geometry changes to indicate the material assigned to the volume. In this case, there is only one volume in the geometry so there is a single color. Alternatively, if there are multiple volumes with different materials assigned, the model will be displayed accordingly with distinct colors for each material assigned.


    Figure 14.
  5. On the guide bar, click to exit the tool.

Assign the Flow Boundary Conditions

The current model has one inlet, three outlets, and walls for the rest of the surfaces. When a geometry model is imported into HyperWorks CFD, all the surfaces are placed in the Default Wall (i.e. Type = auto_wall). As you start assigning the surface boundary conditions, those surfaces are moved into a new boundary condition group. All the surface boundary condition tools are placed under the Boundaries sub-section of the Flow ribbon.

  1. From the Flow ribbon, Domain tools, click the Profiled tool.


    Figure 15.
  2. In the modeling window, click the surface of the inlet.


    Figure 16.
    Observe that a new group named "Inlet" is created under the Boundaries list in the top-left corner of the modeling window. Once the current command is executed, the highlighted surface will be moved into the Inlet group.
  3. In the dialog that appears, enter a value of 2.0 m/sec for Average velocity.


    Figure 17.
  4. On the guide bar, click to execute the command.
    The color of the inlet surface in the modeling window is updated.
    Note: The color assigned to the surfaces is random. Therefore, the color of the surfaces shown in the images below might be different from what you see on your screen.


    Figure 18.
  5. From the Flow ribbon, Domain tools, click the Outlet tool.


    Figure 19.
  6. Click the three outlet surfaces shown in the figure below.


    Figure 20.
  7. Leave the default options in the dialog unchanged then click on the guide bar to execute the command.
    The color of the outlet surfaces change and the list of boundaries on the left are updated. The number of surfaces under each group are shown in the brackets.


    Figure 21.
    Note:
    • To update the color of any group, click on the colored-square on the left of the group name and select the color of your choice from the palette.
    • To update the name of any group, right-click on the group name and select Rename from the context menu.
  8. On the guide bar, click to exit the tool.
  9. Save the model.

Define Mesh Controls

Now that you have assigned the material properties and boundary conditions, you will define the meshing parameters for the model and then generate the mesh.

Define the Surface Mesh Controls

  1. From the Mesh ribbon, Mesh Controls tools, click the Surface tool.


    Figure 22.
  2. Right-click in the modeling window and go to Select > All.


    Figure 23.
    All the surfaces in the model are highlighted and a dialog for surface mesh parameters appears.
  3. Enter 0.003 for the Average element size.


    Figure 24.
  4. Leave the default values for the remaining parameters unchanged then click on the guide bar to execute the command.

Define the Boundary Layer Mesh Parameters

  1. From the Mesh ribbon, Mesh Controls tools, click the Boundary Layer tool.


    Figure 25.
  2. Right-click in the modeling window and go to Select > Advanced Select > By Boundaries > Default Wall.


    Figure 26.
    All the wall surfaces are highlighted and a dialog for boundary layer parameters appears.
  3. Enter the values in the dialog as shown in the figure below.


    Figure 27.
  4. On the guide bar, click to execute the command.

Generate the Mesh

  1. From the Mesh ribbon, Mesh tools, click the Batch tool.


    Figure 28.
  2. In the Meshing Operations dialog, enter an Average element size of 0.005.


    Figure 29.
  3. Click Mesh.
    Once the meshing process has started, the Run Status dialog appears. To view the status of the meshing process, right-click on the process row and select View log file.
    Once the meshing is done, the run status is updated accordingly, and you are automatically moved to the Solution ribbon.


    Figure 30.

Run AcuSolve

  1. From the Solution ribbon, Simulation tools, click the Run tool.


    Figure 31.
  2. In the Launch AcuSolve dialog, verify that the Problem directory and AcuRun path are pointing to the correct location.
  3. Set the Parallel processing option to Intel MPI.
  4. Optional: Set the number of processors to 4 or 8 based on availability.
  5. Deactivate the Automatically define pressure reference option.
  6. Expand the Default initial conditions menu.
  7. Deactivate the Pre-compute flow option and enter 2.0 for x-velocity.
  8. Deactivate the Pre-compute turbulence flow option and enter 1e-5 for Eddy viscosity.
  9. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 32.
    The Run Status dialog opens again and the AcuSolve run appears on the list.
  10. Right-click on the AcuSolve run and select View log file.

    A summary of the run printed in the dialog indicates that AcuSolve has finished running the simulation. Once the solution is converged, the Status will be updated accordingly.



    Figure 33.
  11. In the Run Status dialog, right-click on AcuSolve and select Plot time history from the context menu.
  12. In the Plot Utility dialog, double-click on the Residual Ratio row to open the plot of residual ratios.


    Figure 34.

    The above plot shows the residuals of the equations as the solution progresses through each time step. You can see the residuals dropping smoothly. Once the pressure and velocity residual ratios reach a value less than the specified convergence tolerance (0.001), the solution is considered to be converged. By default, the eddy viscosity convergence tolerance is set to a magnitude of one order higher than the specified convergence tolerance (0.01).

Post-Process the Results with HyperView

This part of the tutorial shows you how to work with steady state analysis data in HyperView once the solution has converged.

Open HyperView and Load the Model and Results

  1. Start HyperView from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is Manifold.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Apply Pressure Contours on the Boundary Surfaces

  1. Click on the Results toolbar to open the Contour panel.
  2. In the Contour panel, select Pressure (s) as the Result type.
  3. Click Apply.


    Figure 35.
  4. In the panel area, under the Display tab, turn off the Discrete color option.


    Figure 36.
  5. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
    The pressure contour should be displayed as shown in the figure below.


    Figure 37.

Save Plots as Image Files

  1. On the Image Capture toolbar toggle the / icons so that it shows the icon to save to file.
  2. Click the icon on the Image Capture toolbar.
  3. Provide a name for the image in the dialog and click Save.
    If you want to use the image in a presentation you can copy them to the clipboard by toggling the Save Image to File/Clipboard icon to instead of . Then paste the image in your presentation.

Create Pressure and Velocity Contours on a Cut Plane

  1. To create a new cut plane, right-click in the Results Browser and select Create > Section Cut > Planar from the context menu.
    A new entity, Section 1, is created in the Results Browser.
  2. Right-click Section 1 and select Edit from the context menu.
  3. In the Section Cut panel verify that Define plane is set to Y Axis.
  4. Under the Display options, activate the Cross section check box.
  5. Verify that the Clip elements check box is activated.
  6. For the Base coordinates, enter a value of -0.015 for the Y-coordinate and press Enter.


    Figure 38.
  7. Click on Gridline in the panel area.
  8. In the dialog, uncheck the Show option under Gridline then click OK.


    Figure 39.
  9. Click on the Results toolbar to open the Contour panel.
  10. In the Contour panel select Velocity as the Result type.
  11. Click Apply.


    Figure 40.

Create a Clipping Plane

The section cut plane can be used as a clipping plane as well. In this step you will create a clipping plane.
  1. Right-click Section 1 under Section Cuts in the Results Browser and select Edit from the context menu.
  2. In the Section Cut panel change the selection under Display options from Cross section to Clipping plane.


    Figure 41.
  3. Click Reverse to toggle the clipping direction to your choosing.


    Figure 42.

Create Velocity Vectors

  1. In the Section Cut panel under Display options, set the selection back to Cross section.
  2. Click the icon on the Results toolbar.
  3. On the Vector panel, make sure that the Result type is set to Velocity (v).
  4. Set the Selection mode to Sections using from the drop-down menu.
  5. Click the Sections collector to open the Extended Entity Selection dialog.
  6. Click Displayed.


    Figure 43.
  7. Select the Z+X Resultant option.


    Figure 44.
  8. Click Apply.
  9. Click the Display tab and set the options as shown in the figure below.


    Figure 45.
  10. Click the Section tab and activate the Projected and Evenly distributed check boxes.
  11. Set the Number of rows and columns to 20 and 50 respectively then click Apply.


    Figure 46.
    The vector plot should be displayed as shown in the figure below.


    Figure 47.

Display Streamlines

  1. In the Results Browser, expand the Section Cuts folder.
  2. Click the icon next to Section 1 to turn off its display.
  3. In the Results Browser, turn off the display for all components except Inlet and Outlet.


    Figure 48.
  4. Click the icon on the Results toolbar to open the Streamlines panel.
  5. Click Add to add a new set of streamlines.
  6. Set the Rake type to Line, if not already selected.
  7. Click the icon.
    The Reference point dialog opens.
  8. Enter the reference points as shown in the figure below.


    Figure 49.
  9. In the panel area, set the Integration mode to Downstream and the Number of seeds to 20.
  10. Make sure that the Source is set to Velocity.
  11. Click Create Streamlines.
  12. Enter the Streamline Size as 3 and press Enter .


    Figure 50.


    Figure 51.

Summary

In this tutorial, you worked through a basic workflow to carry out a CFD simulation and post-processed the results using HyperWorks products, namely HyperWorks CFD and HyperView. You started by importing and meshing the model in HyperWorks CFD. You also set up the model and launchedAcuSolve directly from within HyperWorks CFD. Upon completion of the solution by AcuSolve, you used HyperView to post-process the results. You learned how to create contours on the boundary surfaces and the section cuts, velocity vectors, and streamlines.