ACU-T: 1000 HyperWorks UI Introduction

This tutorial provides the instructions for setting up a Computational Fluid Dynamics (CFD) simulation making use of the HyperWorks package. HyperWorks is a comprehensive suite of various Computer-Aided Engineering (CAE) products, each specialized in a certain aspect of the CAE process. These include HyperMesh as a generic, powerful geometric modeling and pre-processing tool, and HyperView as a post-processing and visualization tool. Bridging these two applications is a complete range of solvers for a gamut of engineering applications. Among these solvers is AcuSolve, which is Altair’s offering for fluid flow and thermal analysis simulations.

HyperMesh’s inbuilt geometric modeling and finite element meshing capabilities will allow you to create the geometry for your problem and generate excellent quality meshes in a single tool. Meshes generated in HyperMesh can be exported in the format that AcuSolve will recognize. Moreover, HyperMesh’s integration with AcuSolve also allows you to complete the pre-processing steps in HyperMesh itself, including the problem setup. Once you have completed setting up your simulation in HyperMesh, you can directly generate the AcuSolve input files. You can also choose to directly launch AcuSolve from within HyperMesh. This integration is expected to be especially beneficial for you if you happen to be a traditional user of HyperMesh for your modeling and meshing requirements.

The HyperWorks package has a powerful tool for post-processing and visualizing the results of your CFD simulations, called HyperView. HyperView enables you to visualize data interactively as well as capture and standardize your post-processing activities using process automation features. HyperView combines advanced animation and XY plotting features with window synching to enhance results visualization. HyperView also saves 3D animation results in Altair's compact H3D format so you can visualize and share CAE results within a 3D web environment using HyperView Player. HyperView has a rich feature set that you might find beneficial to your post-processing activities and are useful to explore. HyperView has inbuilt direct-reading capabilities for AcuSolve results and does not require any conversion steps.

In this tutorial, you will learn how to use HyperMesh for importing a geometric model and generating a mesh. You will then set up and launch the simulation from within HyperMesh. Following that, you will learn how to use HyperView for post-processing AcuSolve results.

In this tutorial you will do the following:
  • Analyze the problem
  • Start HyperMesh and create a model database
  • Import the geometry for the simulation
  • Generate and organize the mesh using the Mesh Controls Browser
  • Set general problem parameters
  • Set solution strategy parameters
  • Set the appropriate boundary conditions
  • Run AcuSolve
  • Monitor the solution with AcuProbe
  • Post-process with HyperView

Prerequisites

To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve. This tutorial introduces you to HyperMesh and HyperView so no prior experience is expected.

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

The file ACU-T1000_manifold.x_t stores the geometry information for the fluid portion of the model for this problem in Parasolid ASCII format.

The color of objects shown in the modeling window in this tutorial and those displayed on your screen may differ. The default color scheme in HyperMesh is "random," in which colors are randomly assigned to groups as they are created. In addition, this tutorial was developed on Windows. If you are running this tutorial on a different operating system, you may notice a slight difference between the images displayed on your screen and the images shown in the tutorial.

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

Introduction to HyperMesh

HyperMesh is a generic tool offering a combination of geometric modeling and pre-processing capabilities.

HyperMesh supports a number of commonly used solvers used in simulating various engineering applications, providing direct interfaces to most of them. This offers you flexibility to use HyperMesh as a single tool for most, if not all, of your modeling and pre-processing activities.

AcuSolve is among the solvers that are closely integrated with HyperMesh. In order to simplify the interfaces associated with each solver, HyperMesh uses user profiles to automatically manage the templates for a given solver. Each user profile has an associated pre-defined set of menus, options and toolbars visible. User profiles ensure that the solver setup is in accordance with the options and requirements of the solver associated with the profile in which it is generated. It is advised that you make sure you are using the correct user profile when setting up a model. Also, it is recommended that the active user profile is not to be changed while the current HyperMesh database is populated.

In this tutorial, you will be working in a user profile associated with AcuSolve. Once you begin the tutorial, you will change the active user profile to the AcuSolve user profile. HyperMesh remembers the last active user profile when it is restarted. If the last HyperMesh user on your machine was working in the AcuSolve user profile when you launch HyperMesh, it will start with the AcuSolve user profile.

A HyperMesh session loaded with the AcuSolve user profile looks like the image below.


Figure 2. HyperMesh Interface with Active AcuSolve User Profile
  1. Menu bar: Located at the top of the window, just under the title bar. Like the pull-down menus in many applications, these menus drop-down a list of options when clicked.
  2. Toolbars: Located around the modeling window. These have icons that provide quick access to commonly-used functions, such as changing display options. They can be dragged and placed as per the user preference.
    Below are some of the commonly used toolbars.


    Figure 3. Standard Toolbar

    Provides the options for creating, opening or saving the database, import/export options and changing user profiles.



    Figure 4. Checks Toolbar

    On the Checks toolbar, you can access various checks and calculations tools that are commonly used in the model building process.



    Figure 5. ACU Toolbar

    The ACU toolbar has options for creating, deleting and organizing entities, accessing meshing panels, and launching AcuSolve or HyperStudy.



    Figure 6. Display Toolbar

    On the Display toolbar, you can control what entities HyperMesh displays, primarily by masking entities to hide or display. This toolbar is usually located along the left edge of the modeling window.



    Figure 7. Visualization Toolbar

    Options available on the Visualization toolbar control how HyperMesh visualizes entities in the modeling window.

  3. Tab area: The two areas marked 3 and 4 in Figure 2 make up the tab area. The tab area is so named because various specialized tools display on tabs in this area of the interface. One of these tabs is the Model tab, which you will be using most frequently. The Model tab will also be the tab active by default when you start a HyperMesh session. The top half of the tab area, marked 3, is the browser area. Depending on the selected tab, you will be able to see the various options or entities which belong to the active HyperMesh database. For example, when the Model tab is selected, the Model Browser will display the entities present in the model, each of which carry some information about the model. This information may be related to the geometrical components that make up the model, the material information, the load information, and so on. The model structure is viewed as a flat, listed tree structure within the browser.
  4. Entity Editor: The bottom half, marked 4 in Figure 2, is the Entity Editor. In the Entity Editor, you will be able to view and edit the information associated with the different entities available in the browser. Clicking on an entity in the browser area will display the entity related information in this area.
  5. Main Menu: The main menu displays the available functions. You access these functions by clicking on the button corresponding to the function you want to use. Clicking on the button will open the panel associated with the function in the menu area.
  6. Modeling Window: The modeling window is the display area for your model. You can interact with the model in three-dimensional space in real time. In addition to viewing the model, entities can be selected interactively from the modeling window.
  7. Status bar: The status bar is located at the bottom of the screen. The four fields on the right side of the status bar display the current include file, current part, current component collector and current load collector. As you work in HyperMesh, any warning or error messages also display in the status bar on the left side.

Introduction to HyperView

HyperView is a generic post-processing and visualization environment for finite element analysis (FEA), CFD, multi-body system simulation, digital video and engineering data.

HyperView offers direct-reading capabilities for AcuSolve generated results. AcuSolve results can be directly opened in HyperView. HyperView also has process automation features, which can enable you to expedite and standardize your post-processing activities.

The image below shows the HyperView interface when it is started.


Figure 8. HyperView
  1. Menu bar: Located at the top of the window, just under the title bar. Like the pull-down menus in many applications, these menus drop-down a list of options when clicked.
  2. Toolbars: Located around the modeling window. These have icons that provide quick access to commonly-used functions, such as changing display options. They can be dragged and placed as per the user preference. Below are some of the commonly used toolbars.


    Figure 9. Standard Toolbar

    Provides the options for creating or opening a model, saving an HyperView session and import/export options.



    Figure 10. Results Toolbar

    On the Results toolbar you can access various options related to displaying the results, for example, contours, vectors and streamlines.



    Figure 11. Display Toolbar

    The Display toolbar provides you with quick access to the Mask panel, Section Cut panel and Display Controls.



    Figure 12. Visibility Controls Toolbar

    The Visibility Controls toolbar provides you quick access to the visibility controls of the entities in the Results Browser.



    Figure 13. Image Capture Toolbar

    The Image Capture toolbar provides you quick access to the image and video capturing capabilities.

  3. Tab area: The two areas marked 3 and 4 in Figure 8 make up the tab area. The tab area is so named because various specialized tools display on tabs in this area of the interface. In HyperView, one of these tabs is the Results tab, which you will be using most frequently. Results tab will also be the tab active by default when you start an HyperView session. The top half of the tab area, marked 3, is the browser area. Depending on the selected tab, here you will be able to see the various options or entities which are part of the active HyperView model, in a listed tree structure similar to HyperMesh.
  4. Entity Editor: The bottom half, marked 4, is the Entity Editor. In the Entity Editor, you will be able to see and edit the information associated with the different entities available in the browser. Clicking on an entity in the browser area will display the entity related information in the Entity Editor.
  5. Panel area: The panel area displays the function panel associated with the active function selection. You can access these functions by clicking on the icon on a toolbar corresponding to the function you want to use. Clicking on the icon will open the panel associated with the function in the panel area. When you launch HyperView, you will see the Load Model panel in this region.


    Figure 14.
  6. Modeling window: The modeling window is the display area for your model. You can interact with the model in three-dimensional space in real time. In addition to viewing the model, entities can be selected interactively from the modeling window.
  7. Status bar: The status bar is located at the bottom of the screen. As you work in HyperView, any warning or error messages also display in the status bar, on the left side.

Define the Simulation Parameters and Import the Geometry

Start HyperMesh and Create a Model Database

In this tutorial, you will begin by creating a model database in HyperMesh, loading the geometry and generating and organizing the mesh. Next you will set up the problem parameters, component parameters, and boundary conditions and then launch AcuSolve to solve for the number of time steps specified. Finally, you will visualize some characteristics of the results using HyperView.

In the next steps you will start HyperMesh and create the database for storage of the simulation settings.

  1. Start HyperMesh from the Windows Start menu by clicking Start > Altair <version> > HyperMesh.
    A User Profiles dialog opens.
    Note: If it does not show up for you, click Preferences on the menu bar and select User Profiles.
  2. Select HyperMesh from the Application drop-down menu.
  3. Select AcuSolve from the list of applications.
  4. Click OK.


    Figure 15.

    Traditional HyperMesh users will be able to tell the difference between the default HyperMesh profile and the CFD (AcuSolve) profile. There will be an additional CFD toolbar visible. Also, the Model Browser will be populated with some entities relevant to a CFD simulation setup.



    Figure 16.
  5. Click File > Save to open the Save Model dialog.
    Save the model database frequently as you proceed through the tutorial steps.
  6. Browse to the location that you would like to use as your working directory.
    This directory is where all files related to the simulation will be stored. When you are setting up the problem, there will be a file with extension hm in this directory, which corresponds to an HyperMesh model database. Once the mesh and solution are generated, additional files and directories will be added by HyperMesh and HyperMesh.
  7. Create a new directory in this location. Name it ACU1000_HyperWorks and navigate into this directory.
  8. Enter ACU1000_HyperWorks as the file name for the database, or choose any name of your preference.
    Note: In order for other applications to be able to read the files written by HyperMesh, the database path and name should not include spaces.
  9. Click Save to create the database.

Import the Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of ACU-T1000_manifold.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.
  1. Click File > Import > Geometry.
    Tip: Alternatively, click the arrow next to the Import Solver Deck icon on the standard toolbar and select Import Geometry.
  2. Select Parasolid as the File type.
    Note: In general, if you are not sure about the geometry file type, leave the File type option as Auto Detect.


    Figure 17.
  3. Click .
    Note: If you see anything in the list of import files, clear the list before this step by clicking .
  4. In the Select Parasolid file dialog, select ACU-T1000_manifold.x_t and click Open.
  5. Make sure that the selected file is in the list of import files and click Import.
  6. Click Close.
  7. Click on the Visualization toolbar to display the surfaces.


    Figure 18.
    Tip: Use the following controls for visualizing the model:
    1. Ctrl + Left-Click: Rotate the model
    2. Ctrl + Scroll: Zoom in/out
    3. Ctrl + Right Click: Pan the model

Define Mesh Controls and Generate the Mesh

In the following steps you will set up the mesh controls and generate the mesh for the model. You will be introduced to the Mesh Controls Browser for this purpose.
Select Mesh > Mesh Controls from the menu bar.
The Mesh Controls Browser opens.


Figure 19.

The Mesh Controls Browser lets you access all of the different meshing technologies in the single browser. As you can see in the image above there are options to generate the surface mesh, volume mesh, refinement zones, and so on. Within these options there are associated model, local, feature, and refinement controls available. The model controls apply to the entire model. The local controls apply to a specific entity in the model, such as surfaces and elements.

You will start by creating a surface mesh control followed by a volume mesh control with active boundary layers. You will then add a volume mesh local control for the surfaces that do not require a boundary layer.

Set up the Surface Mesh Controls and Generate Surface Mesh

  1. Right-click on Surface Mesh in the Mesh Controls Browser. From the context menu that appears, select Create > Model > Size and Bias > Surfaces.
  2. Optional: In the Entity Editor, set the entity name to Surface_Mesh_Control.
  3. Set the Element Size to 0.003.
  4. Set the Element Type to Trias.
  5. Under the Entity Selection group, click in the field next to Entities then click the Surfaces collector.


    Figure 20.
    The surface entity selector menu opens in the menu area.
  6. In the menu area, click the surfs collector and select all.
  7. Click proceed.
  8. Expand the Advanced group and verify the following settings:
    1. Destination Component: Original
    2. Mesh Connectivity: Keep


      Figure 21.
  9. In the Mesh Controls Browser, right-click on Surface Mesh and select Mesh.
    Surface mesh is generated on the model.

Organize the Surfaces Elements

In this step, you will create component collectors for the surface elements and move the surface mesh elements on the Inlet and Outlet surfaces into the respective components. Organizing the surface mesh elements will help you in specify boundary conditions at the surfaces. Use the following figure as reference:


Figure 22.
  1. From the menu bar, select BCs > Components > CFD.
    The Create CFD Components dialog opens.
  2. In the dialog, click the Check none icon then activate the Inflow and Outflow fields.
  3. Click Create then Close.


    Figure 23.
  4. Close the dialog and go to the Model Browser and expand the list of components. Right-click on Part 1 and select Rename.
  5. Type Wall as the new component name and press Enter.
  6. Open the Organize panel by doing one of the following:
    1. Click organize in the panel area.


      Figure 24.
    2. Click BCs > Organize from the menu bar.
    3. Click on the CFD toolbar.
  7. In the modeling window, zoom in on the inlet surface region and select any mesh element on the inlet surface.


    Figure 25.
  8. In the panel area, click the elems collector and select the by face option.
    All the elements on the inlet surface are selected in the modeling window.
  9. Click dest component = and select Inflow.
  10. Click move.
    All the inlet surface mesh elements are colored in the Inflow component color.
  11. Similarly, select a mesh element on each of the Outflow surfaces then click on the elems collector and select the by face option. Verify that all the surface elements on the three outlet surfaces are now highlighted then set the dest component = to Outflow and click move.
    The model should now look similar to the figure below.


    Figure 26.
  12. Click return to exit the panel.

Set up the Volume Mesh Controls

  1. Go to the MeshControls tab and right-click on Volume Mesh. From the context menu that appears, select Create > Model > BL + Tetra.
    Selecting BL + Tetra will show options for the boundary layer specification in addition to tetra volume meshing options.
  2. In the Entity Editor, set the entity name to Volume_Mesh_Control.
  3. Under the Entity Selection group, click in the value field next to Entities then click the Components collector.


    Figure 27.
    The Select Components dialog opens.
  4. Select all three components in the dialog and click OK.


    Figure 28.

    You can click the icon in the dialog to quickly select all of the components.

  5. Click OK to close the dialog.
  6. Expand the Boundary Layer group and set the boundary layer parameters as follows:
    1. Change the Method to Advanced
    2. Set First Layer Thickness to 0.0005
    3. Select Acceleration as the BL Growth Rate Method.
    4. Set Initial Growth Rate to 1.3
    5. Set the Number of Layers to 5
    6. Change Hexa Transition Mode to All Prism


      Figure 29.

      When generating boundary layer meshes in HyperMesh, it is recommended to use All Prism as the boundary layer meshing mode for superior element quality. The prism elements can later be split into tetrahedral elements, which is the recommended element type for HyperMesh.

      This completes the boundary layer mesh control. You will now add a local control for surfaces that do not require a boundary layer.

  7. Right-click on Volume Mesh in the Mesh Controls Browser. From the context menu that appears, select Create > Local > No BL.
  8. Optional: In the Entity Editor, set the entity name tono_BL_control.
  9. Under the Entity Selection group, click in the value field next to Entities then click the Components collector.


    Figure 30.
    The Select Components dialog opens.
  10. Select Inflow and Outflow from the list and click OK.


    Figure 31.
  11. Expand the Boundary Layer group and set Base Surface Mesh Treatment to Float.


    Figure 32.
  12. Finally, add a volume selector control to put the boundary layer and the core tetra mesh in the same component.
    1. Right-click on Volume Mesh in the Mesh Controls Browser. From the context menu that appears, select Create > Volume Selector.
    2. In the Entity Editor, activate the check box for BL and Tetras in One Component.


      Figure 33.

Generate the Volume Mesh

In the previous steps, you created some model and local mesh controls. Your Mesh Controls Browser should look like the figure below.



Figure 34.

When you set up the mesh controls, at least one active model control should be present before you generate the mesh. You can create multiple model controls, but only one model control can be active at a time. Surface and volume mesh however have different mesh controls.

Local controls are optional. You can create multiple local mesh controls, however only the ones which are selected at the time of mesh generation will be applied.

  1. In the Mesh Controls Browser, make sure that both the Model and Local volume mesh controls are enabled.
  2. Right-click on Volume Mesh and click Mesh.

    The generated volume mesh is placed in a single collector called CFD_tetcore001 under the list of components. This collector will be visible in the Model Browser. Once the meshing is complete, observe the mesh using the visualization controls.



    Figure 35.

    You can turn off the surface display to view the mesh more clearly. On the Visualization toolbar, click the icon to display the geometry as wire frame. This will turn off the surface display. To turn on the surface display, click the icon. Zoom in to observe the boundary layer generated.



    Figure 36.
  3. In the Model Browser rename the collector CFD_tetcore001 to Fluid. In the Entity Editor, change the Type to FLUID.
    This collector will hold all of the 3D volume elements.

    The mesh generated has prismatic elements in the boundary layer. These elements will be split to create tetrahedral elements.

  4. Click Mesh > Edit > Elements > Split Elements.
    The Split Elements panel opens.
  5. Select the solid elements sub-panel.
  6. Click the elems collector and select all.
  7. Change the split pattern to split into tetras.
    This is the optimized mode for splitting elements into tetras for a CFD simulation.
  8. Click split.
    Observe the mesh after the splitting process is complete.


    Figure 37.
  9. Click return to exit the panel.

Set up Simulation Parameters for AcuSolve

The next step after creating the mesh is to set up the simulation parameters. You will use the Solver Browser for this purpose. The Solver Browser provides a solver perspective view of the model structure in flat, listed tree structure.

Set General Simulation Parameters

In next steps you will set parameters that apply globally to the simulation.
  1. Click View > Solver Browser to open the Solver Browser.
    The Solver Browser lists every entity mapped to the active solver profile within the session and places those entities into their respective entity group folders.


    Figure 38.
  2. Expand 01.Global and then expand 01.PROBLEM_DESCRIPTION.
  3. Click PROBLEM_DESCRIPTION to open the Entity Editor.
  4. Type Manifold for the Title.
  5. Change the Turbulence model from Laminar to Spalart Allmaras.


    Figure 39.

Specify the Solver Settings

  1. In the Solver Browser, expand the 02.SOLVER_SETTINGS group then click SOLVER_SETTINGS to open it in the Entity Editor.
  2. Verify that the Convergence tolerance is set to 0.001.
  3. Change the Relaxation factor to 0.4.
  4. Check that Flow and Turbulence are set to On.


    Figure 40.

Set Nodal Initial Conditions

  1. In the Solver Browser, expand the 03.Nodal_Initial_Condition group then click Nodal_Initial_Condition to open it in the Entity Editor.
  2. Set the X velocity to 2 m/sec.
  3. Set the Eddy viscosity to 1e-05 m2/sec.


    Figure 41.

Apply Volume Parameters

Volume groups are containers used for storing information about a volume region. This information includes solution and meshing parameters applied to the volume and the geometric regions that these settings are applied to.

There is one volume collector in this model, fluid. In the next steps you will set the material properties for it.

  1. In the Solver Browser, expand 11.Volumes then expand the FLUID volume group and click Fluid.
    The fluid collector entity opens in the Entity Editor.
  2. Click in the value field for Material (it is Unspecified by default).
  3. Click Material.
    The Select Material dialog opens.
  4. Select Water_HM and click OK.


    Figure 42.

Apply Surface Parameters

Surface groups are containers used for storing information about a surface, including solution and meshing parameters, and the corresponding surface in the geometry that the parameters will apply to.

  1. In the Solver Browser, expand 12.Surfaces then expand the WALL surface group. Click Wall to open it in the Entity Editor. Verify that the Type is set to WALL.


    Figure 43.
  2. Expand the OUTFLOW surface group then click Outflow to open it in the Entity Editor. Verify that the Type is set to OUTFLOW.


    Figure 44.
  3. Expand the INFLOW surface group then click Inflow to open it in the Entity Editor. Verify that the Type is set to INFLOW. Set Inflow type to Average velocity. Set the Average velocity to 2 m/sec.


    Figure 45.
  4. Save the model.

Compute the Solution and Review the Results

Run AcuSolve

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

  1. In the Model Browser, ensure that the visibility of the mesh for all collectors to be exported to AcuSolve is activated. In this case, Fluid, Wall, Inflow and Outflow should be activated.


    Figure 46.

    The display of the mesh icon beside the component name indicates that the visibility of mesh for that component is on. The display of the mesh of a component can be turned on/off by clicking on that icon.

  2. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.


    Figure 47.

    For this case, the default settings will be used. You may choose to change the number of processors to allow AcuSolve to run using more processors (4 or 8), if available. HyperMesh will generate the required solver input files and launch AcuSolve. AcuSolve will calculate the steady state solution for this problem.

  3. Verify that Auto run AcuProbe is On.
    This will open an AcuProbe dialog which will let you monitor the solution progress.
  4. Click Launch to start the solution process.
    As the solution progresses, an AcuTail and an AcuProbe dialog will open. Solution progress is reported in the AcuTail dialog. An AcuSolve Control dialog will also open from which you can control the solution process. In this dialog you have options to stop the solution or generate the output files at the end of the current time step.


    Figure 48.

    A summary of the run printed in the AcuTail dialog indicates that AcuSolve has finished running the solution.



    Figure 49.

Monitor the Solution with AcuProbe

AcuProbe can be used to monitor various variables over solution time.
  1. In the AcuProbe dialog, expand Residual Ratio.
  2. Right-click on Final and select Plot All.
    Note: You might need to click on the toolbar in order to properly display the plot.


    Figure 50.

    The plot above 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).

  3. You can also save the plots as an image.
    1. From the AcuProbe dialog, click File > Save.
    2. Enter a name for the image and click Save.
  4. The time series data of the variables can also be exported as a text file for further post-processing.
    1. Right-click on the variable that you want to export and click Export.
    2. Enter a File name and choose .txt for the Save as type.
    3. Click Save.

Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

Open HyperView and Load the Model and Results

  1. In the HyperMesh main menu area, click Applications > 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 ACU1000_HyperWorks.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 51.
  4. In the panel area, under the Display tab, turn off the Discrete color option.


    Figure 52.
  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 53.

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 54.
  7. Click on Gridline in the panel area.
  8. In the dialog, uncheck the Show option under Gridline then click OK.


    Figure 55.
  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 56.

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 57.
  3. Click Reverse to toggle the clipping direction to your choosing.


    Figure 58.

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 59.
  7. Select the Z+X Resultant option.


    Figure 60.
  8. Click Apply.
  9. Click the Display tab and set the options as shown in the figure below.


    Figure 61.
  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 62.
    The vector plot should be displayed as shown in the figure below.


    Figure 63.

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 Inflow and Outflow.
  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 64.
  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 65.


    Figure 66.

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 HyperMesh and HyperView. You started by importing and meshing the model in HyperMesh. You also set up the model and launchedAcuSolve directly from within HyperMesh. 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.