# ACU-T: 1000 HyperMesh CFD UI Introduction

This tutorial introduces you to the workflow for setting up a Computational Fluid Dynamics (CFD) analysis using Altair HyperMesh CFD. HyperMesh CFD is a powerful tool which provides a single, streamlined platform for performing a CFD analysis, starting from importing CAD through post-processing results. In this tutorial, you will learn how to use HyperMesh 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 HyperMesh CFD and post-process the results using HyperMesh CFD Post.

## Prerequisites

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

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

## 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.

## Introduction to HyperMesh CFD

The HyperMesh CFD graphical user interface can be divided into seven general categories as shown in the figure above.

1. The menu bar contains the drop-down menus for File input-output, Edit, and View operations.
2. The modeling environment switcher is used to populate relevant ribbons and tools based on modeling tasks.
3. Ribbons contain various functionalities and tools available in HM-CFD. Navigate between various ribbons by clicking the ribbon tabs to the right of the modeling environment switcher. After selecting a ribbon, the corresponding tool icons are displayed on the screen. The functionalities of various ribbons and corresponding tools are briefly explained in this section.
Sketch ribbon
The Sketch ribbon provides multiple ways to define sketching plane by selecting planes aligned with global coordinate systems. You can also get references of existing geometry by cutting geometry or projecting geometry to a plane. It provides capabilities to create sketches using multiple interactive tools. A dimensioning capability enables you to parametrize dimensions of sketches. One of big use case for CFD is to get cutting lines of rotating geometry and create a non–cylindrical axisymmetric MRF region around them.
Geometry ribbon

The Geometry ribbon consists of tools for repairing, creating, editing, and validating the geometry.

When a geometry file is imported, the Repair tools can be used to detect any defects present in the CAD model like intersections, free edges, duplicates, sliver surfaces, and so on and fix those errors.

The tools available under the Create sub-section can be used to create geometric entities like points, lines, surfaces, and solids.

The tools required for performing operations like plugging cavities, stitching surfaces, and so on are available under the Edit sub-section.

The Defeature tool can be used to resolve defects or model a new geometry, while the Validate tool can be used to detect any defects present in the CAD model. This process is usually known as CAD cleanup.

Discrete ribbon

The Discrete ribbon consists of tools used for working with FE geometry. You can cap openings, connect geometry, define local or proximity-based wrap controls, enclose the model, remesh the enclosed results, and fix the mesh quality.

Assembly ribbon
The Assembly ribbon is useful for finding, managing, and organizing the parts in your model.
Flow ribbon
The Flow ribbon contains tools for setting up simulation parameters, solver settings, and reference properties such as material properties, heat sources, porous media, and so on. The Setup sub-section is where you set up the physics equations and solver settings as well as create material models, multiplier functions, and parameters.
The Domain sub-section contains tools for assigning reference properties such as materials, heat and momentum sources, and reference frames to volumes.
Surface boundary conditions such as inlets, outlets, and far fields, can be assigned using the tools under the Boundaries sub-section. By default, all the surfaces are assigned a boundary condition of type ‘auto_wall’ and are placed under Default wall. Refer to the AcuSolve Surface Processing manual for more information about auto_wall. As you assign boundary conditions to the surfaces, they are moved into the respective group.
The Radiation ribbon is where you define radiation physics, create thermal, solar, and participating media models, and apply radiation parameters.
Motion ribbon
Mesh boundary conditions and mesh-motion-related parameters can be defined using the tools available in the Motion ribbon. Parameters such as mesh motion type and mesh displacement constraints can be defined here. In addition to the mesh boundary conditions, code coupling with external codes such as OptiStruct and MotionSolve can be defined here
AcuTrace ribbon
The AcuTrace ribbon computes particle traces as a series of segments solving particle motion. It computes traces for unsteady as well as steady flow fields, for flows with mesh motion as well as without, and for flows computed on meshes with interface surfaces. To solve a problem with AcuTrace, you must first run AcuSolve. You can set up for finite mass and massless particles.
Mesh ribbon
Meshing parameters such as surface mesh controls, boundary layer parameters, volume mesh parameters, and zone meshing parameters can be defined here. This ribbon also has tools for local remeshing. Once all the mesh controls are defined, you can generate the mesh using the Volume tool.
Aerodynamics and Aeroacoustics Setup
The setup ribbon is used carry out external aerodynamics and fan noise simulations with the ultraFluidX solver.
Solution ribbon
The Solution ribbon is used to set up monitors for any individual point, surface, or volume set output. The Field tool is used to set the nodal output frequency for the entire model. The Initialize tools are used to set the nodal initial conditions for variables like pressure, velocity, and variables specific to each turbulence model.

Once the complete set up is done, the Run tool is used to launch AcuSolve. Once the AcuSolve run parameters are set, the simulation can be started, and you can monitor the status of the run using the run manager.

Post ribbon
The Post ribbon is where you can post-process the results. The Visualize tools under the Post ribbon can be used to create things like plots, streamlines, iso surfaces, and section cuts. The Measures tools can be used to probe variables at desired locations.
Morphing Ribbon
The Morphing ribbon is used to morph mesh or FE geometry. You can define constraints to fix some nodes or define relative movement.
Once morphing is done, you can create shapes and design variables using the “Shape” tool and submit DOE studies using “DOE Study” tool.
4. The modeling window is where the model is displayed. The model display can be manipulated using the view controls shown in the table below. Clicking on the model will highlight the entity being selected and right-clicking on an entity will give you additional options for the operations that can be done based on the context. Some of the functions available using right-click are Show, Hide, Isolate, Select, Advanced select, Create groups, and so on.
Button Operation
Middle mouse scroll Zoom in and out
Right-click hold and drag Pan the model
Middle mouse click hold and drag Rotate the model
Left-click Select entity
Ctrl + Left-click Select multiple entities
Left-click hold and drag Window select
Shift + Left-click Deselect entities
5. The entity selector enables you to control what entities can be selected using the left-mouse button. The selector can be set to any of the entities shown in the figure below. When you open any tool, the selector is automatically set to the entity (entities) which are appropriate for that command.
6. The visualization of the model can be controlled using the tools available in View Controls toolbar. The display of mesh, model coloring, section cuts, standard views, and so on can be controlled using these tools.
7. The browsers show the entities and setup parameters in the model and list them in a tree structure. They can be turned on or off from the View menu. Some common functions that can be performed in all browsers are show, hide, and isolate.

## Start HyperMesh CFD and Create the HyperMesh Model Database

1. Start HyperMesh CFD from the Windows Start menu by clicking Start > Altair <version> > HyperMesh CFD.
When HyperMesh 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.
• From the Home tools, Files tool group, click the Save As tool.
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 (Manifold, for example) and 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 and then select ACU-T1000_manifold.x_t and click Open.
3. In the Geometry Import Options dialog, leave all the default options unchanged and then click Import.
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

### Validate the Geometry

1. From the Geometry ribbon, click the Validate tool.
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 does not 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.
2. Press Esc or right-click in the modeling window and swipe the cursor over the green check mark from right to left.
3. Save the database.

## Set Up the Problem

In this step, you will set the general simulation parameters such as equation, solver settings, and so on. 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, click the Physics tool.
The Setup dialog opens.
2. Under the Physics models setting:
1. Verify that the Incompressible option is selected under Single phase flow.
2. Set the Time marching to Steady.
3. 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.
3. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.
4. Close the dialog and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. From the modeling window, click anywhere on the manifold.
The entire manifold geometry is highlighted and a Material microdialog appears.
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.
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 HyperMesh 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, Profiled tool group, click the Profiled Inlet tool.
2. In the modeling window, click the surface of the inlet.
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 microdialog, enter a value of 2.0 m/sec for Average velocity.
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.
5. Click the Outlet tool.
6. Click the three outlet surfaces shown in the figure below.
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.
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, click the Surface tool.
2. Right-click in the modeling window and go to Select > All.
All the surfaces in the model are highlighted and a dialog for surface mesh parameters appears.
3. Enter 0.003 m for the Average element size.
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, click the Boundary Layer tool.
2. Right-click in the modeling window and go to Select > Advanced Select > By Boundaries > Default Wall.
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.
4. On the guide bar, click to execute the command.

### Generate the Mesh

1. From the Mesh ribbon, click the Volume tool.
2. In the Meshing Operations dialog, enter an Average element size of 0.005 m.
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.

## Run AcuSolve

1. From the Solution ribbon, click the Run tool.
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 m/s for x-velocity.
8. Deactivate the Pre-compute turbulence flow option and enter 1e-5 m2/s for Eddy viscosity.
9. Leave the remaining options as default and click Run to launch AcuSolve.
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.

11. In the Run Status dialog, right-click on AcuSolve run and select Plot time history to launch the Plot Manager.

The above plot shows the residual and solution ratios of the equations as the solution progresses through each time step. The convergence check is performed on the residual and solution increment ratios of each equation in the problem. For the residual, the ratio of the residual norm over the norm of the forces of the systems is used. For the solution increment, the ratio of the solution increment norm over the solution norm is used. These ratios are computed separately for each solution field, such as pressure and velocity.

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).

Once the pressure and velocity solution ratios reach a value less than the specified convergence tolerance (0.01), the solution is considered to be arrived at steady state. The eddy viscosity solution ratio convergence tolerance is set to a magnitude of one order higher than the specified solution ratio convergence tolerance (0.1).

## Post-Process the Results with HyperMesh CFD Post

This part of the tutorial shows you how to work with a steady state solution using HyperMesh CFD Post.

1. Once the solution is completed, navigate to the Post ribbon.
2. From the menu bar, click File > Open > Results.
3. Browse to your working directory. Select the file Manifold.1.Log and click Open.
The solid and all the surfaces are loaded in the Post Browser.

### Create Pressure Contours on Boundary Surfaces

1. Click the Boundary Groups tool.
2. Select all surfaces in the model by holding the left mouse button, dragging, and drawing a rectangle across the manifold.
3. In the microdialog, set the Display variable to pressure.
4. Activate the Legend toggle and click to reset the range.
5. Click and set the Colormap Name to Rainbow Uniform.
6. Click on the guide bar.

The pressure legend is in Pa.

7. In the Post Browser, right-click on Boundary Group 4 and select Rename. Name it Pressure_plot.

### Plot Velocity and Pressure Contours on a Section Cut

1. In the Post Browser, turn off the display of the boundary surfaces by clicking on the icon next to Flow Boundaries.
2. Click the Slice Planes tool.
3. Select the x-z plane in the modeling window.
4. In the microdialog, click to adjust the plane with the Vector tool.
5. In the Vector tool dialog, click to define the coordinates of the center of plane. Set the value of Y to -0.015 and press Enter.
6. Press Esc twice.
7. In the slice plane microdialog, click to create the slice plane.
8. In the display properties microdialog, set the Display variable to pressure.
9. Activate the Legend toggle and click to reset the range.
10. Click and set the Colormap Name to Rainbow Uniform.
11. Click on the guide bar.

The pressure legend is in Pa.

12. In the Post Browser, right-click on Slice Plane 1 and select Edit.
13. In the microdialog, change the Display variable to velocity (m/s) then click on the guide bar.

## Summary

In this tutorial, you worked through a basic workflow to carry out a CFD simulation and post-process the results using HyperMesh CFD. You started by importing the geometry and meshing the model in HyperMesh CFD. You also set up the model and launched AcuSolve directly from within HyperMesh CFD. Upon completion of the solution by AcuSolve, you post-processed the results in the Post ribbon. You learned how to create contours on the boundary surfaces and section cuts.