ACU-T: 6000 Static Mixer Simulation – AcuTrace

Prerequisites

This tutorial provides the instructions for setting up, solving and viewing results for a simulation of a static mixer in combination with the post-processing moduleAcuTrace. In this simulation, AcuSolve is used to compute the species mixing within a simple mixer and AcuTrace is used to compute the particle motion of finite mass particles within the mixer. This tutorial is designed to introduce you to concepts necessary to visualize particulate flow with AcuTrace.

Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 Basic Flow Set Up, and have a basic understanding of HyperMesh CFD and AcuSolve. The following additional capabilities of AcuSolve are introduced in this tutorial:
• Generation of finite mass particle with AcuTrace.
• Conversion of the nodal output data with AcuTransTrace for reading into HyperMesh CFD Post.
• Post-processing the nodal output with HyperMesh CFD Post to visualize particles movement.
Before you begin, copy the file(s) used in this tutorial to your working directory.
Note: This tutorial does not cover the steps related to geometry cleanup and mesh settings.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of a mixing tube that contains several swept walls to instigate mixing within the tube. The diameter of the inlet is 0.1 m and the length of the mixing tube is 0.525 m. The fins have a mean diameter of 0.1 m. The maximum thickness of the fins is 0.003 m.

The boundary condition at the inlet is defined to produce a fully developed inlet profile with velocity of 1.0 m/s. One portion of the inlet is defined to contain 100 percent of species_1, while the other inlet is defined to contain 0.0 percent of species_1.

The fluid in this problem is an epoxy resin, which has a density of 1264.0 kg/m3 and a viscosity of 1.49 kg/m-sec.

Start HyperMesh CFD and Open the HyperMesh Database

1. Start HyperMesh CFD from the Windows Start menu by clicking Start > Altair <version> > HyperMesh CFD.
2. From the Home tools, Files tool group, click the Open Model tool.
The Open File dialog opens.
3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T6000_Static_Mixer.hm and click Open.
4. Click File > Save As.
5. Create a new directory named Static_Mixer and navigate into this directory.
This will be the working directory and all the files related to the simulation will be stored in this location.
6. Enter Static_Mixer as the file name for the database, or choose any name of your preference.
7. Click Save to create the database.

Validate the Geometry

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.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.

Set Up the Problem

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 Time marching is set to Steady.
2. Select Spalart-Allmaras as the Turbulence model.
3. Set the Number of passive species to 1.
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.

Define the Material Model

1. From the Flow ribbon, click the Material Library tool.
The Material Library dialog opens.
2. Click the My Materials tab.
3. Click to add a new fluid material model.
4. In the material creation dialog, click the name in the top-left corner and rename the material to Epoxy Resin.
5. In the Density tab:
1. Set the Type to Constant.
2. Set the Density value to 1264 kg/m3.
3. Set the Isothermal compressibility value to 0
6. Click the Specific Heat tab and set the Specific heat value to 2386 J/kg-K.
7. Click the Viscosity tab and set the Viscosity value to 1.49 kg/m-s.
8. Click the Conductivity tab and set the Conductivity value to 0.286 W/m-K and Turbulent Prandtl number to 0.91.
9. Close all dialogs and save the model.

Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. Select the solid model then select Epoxy_Resin as the fluid medium.
3. On the guide bar, click to execute the command and exit the tool.

Define Flow Boundary Conditions

1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.
2. In the modeling window, click the inlet surface highlighted in the figure below.
3. In the microdialog, set the Average velocity to 1.0 m/s.
4. Click the Species tab and enter a value of 1.0 for Species 1.
5. On the guide bar, click to execute the command and remain in the tool.
6. Right-click Inlet in the Boundaries legend and select Rename. Change the name to Inlet S1.
7. Select the other inlet surface highlighted in the figure below.
8. In the microdialog, set the Average velocity to 1.0 m/s.
9. Click the Species tab and enter a value of 0.0 for Species 1.
10. On the guide bar, click to execute the command and remain in the tool.
11. Right-click Inlet in the Boundaries legend and select Rename. Change the name to Inlet S2.
12. Click the Outlet tool.
13. Select the surface highlighted below and then click on the guide bar.
14. Click the No Slip tool.
15. Select the wall of the tube highlighted in the figure below and then click on the guide bar.
16. Rename the surface group from Wall to Pipe Wall.
17. Right-click Default Wall in the Boundaries legend and select Isolate.
18. Select all the surfaces highlighted in the figure below and then click on the guide bar.
19. Rename the surface group from Wall to Fin Walls.
20. Click on the guide bar.
21. Turn on the visibility of all the surfaces by right-clicking in the modeling window and selecting Show All or by simply pressing the A key.
22. Save the model.

Define Surface Monitors and Run AcuSolve

1. From the Solution ribbon, click the Volumes tool.
2. Select the model and then click on the guide bar.
3. Click on the guide bar.
4. From the Solution ribbon, click the Run tool.
The Launch AcuSolve dialog opens.
5. Make sure the problem directory is set to the correct location. If not, use the Browse option to select the correct directory.
6. Set the Parallel processing option to Intel MPI.
7. Optional: Set the number of processors to 4 or 8 based on availability.
8. Leave the remaining default options and then click Run to launch AcuSolve.

Post-Process With the Plot Tool

1. From the Solution ribbon, click the Plot tool.
2. Observe the residual and solution ratios as the simulation progresses.

Post-Process with HyperMesh CFD Post

1. Navigate to the Post ribbon.
2. From the Home tools, Files tool group, click the Open Model tool.
3. Open the AcuSolve .log file in your problem directory to load the results for post-processing.
4. Verify that the default step is set to Last in the Reader Options dialog and then click Import.
The solid and all the surfaces are loaded in the Post Browser.
5. In the Post Browser, right-click Pipe Wall and select Edit. Set the transparency to around 80%.
6. Similarly, edit the transparency of Fin Walls to around 30% .
7. Hide Outlet and Inlet S2.
8. Click the Slice Planes tool.
9. Select the x-z plane in the modeling window and then click Calculate.
10. In the display properties microdialog, set the display to species 1 and activate the Legend toggle.
11. Click to reset the legend.
12. Click and set the Colormap name to Rainbow Uniform.
13. Click on the guide bar.
The plot below shows the mixing effectiveness as the maximum value of species 1 is reduced to 0.7 at the outlet, while the minimum value of species 1 is increased to 0.3.

Prepare Particle Trace Attributes for AcuTrace

Now that the steady-state simulation is complete, you can use the finite mass particle tracer to simulate micro-particles of SiO2, which are often used to add strength to the epoxy.

Define Particle Trace Parameters for Static Analysis

1. Navigate to the AcuTrace ribbon.
2. Click the Setup tool.
3. Click Problem definition and set the Particle type to Finite Mass.
4. For the AcuSolve working directory, select the ACUSIM.DIR (flow results) folder in your problem directory.
5. Make sure the Flow field type set to Static.
6. Disable Mesh motion if it not disabled already.
7. Click Finite mass set-up and leave all the parameters as shown below.
8. Close the dialog.

Define Particle Seeds

In the next steps, you will define the particle seeds that are moving into the flow regime.
1. Click the Seeds tool.
2. In the Seed location window, click .
3. Browse to the location where you saved seeds1.csv and seeds2.csv.
4. Select seeds1.csv file and click Open.
This accounts for the particles being fed from Inlet S1.
5. Click Parameters on the guide bar and enter the following details.
6. Click on the guide bar to execute the changes.
7. Right-click on Particle Seeds in the legend and select Rename. Change the name to Inlet S1 Seeds.
8. Repeat the same process and open seeds2.csv.
9. Click Parameters on the guide bar and enter the following details.
10. Click on the guide bar to execute the changes.
11. Right-click on Particle Seeds in the legend and select Rename. Change the name to Inlet S2 Seeds.
12. On the guide bar, click to execute the command and exit the tool.

Define Finite Mass Boundary Conditions

1. Click the Reflecting tool.
2. In the Boundary Conditions window, select the Pipe Wall and then set the Coefficients of restitution values to 0.2.
3. Click on the guide bar to execute the changes.
4. Right-click on Reflecting Wall in the legend and select Rename. Change the name to Pipe Wall.
5. In the Boundary Conditions window, select the Fin Walls and then set the Coefficients of restitution values to 0.8.
6. Click on the guide bar to execute the changes.
7. Right-click on Reflecting Wall in the legend and select Rename. Change the name to Fin Walls.
8. On the guide bar, click to execute the command and exit the tool.
9. Click the Stopping tool.
10. In the Boundary Conditions window, select the Outlet.
11. Click on the guide bar then .

Define Output Parameters

1. Click the Output tool.
2. Check Trace output and enter the values shown below.
3. Click the Time cut setting and enter the values shown below.
4. Close the dialog.

Run AcuTrace

1. Click the Run tool.
2. Check that acuRunTrace.bat is pointing to the correct path: <installation_directory>\hwcfdsolvers\acusolve\win64\bin\acuRunTrace.bat.
3. Set the Parallel processing option to Intel MPI.
4. Optional: Set the number of processors to 4 or 8 based on availability.
5. Leave the remaining options as default and click Run to launch AcuTrace.

Convert Results for Ensight

Once the run is complete, you need to convert the results so that they can be read in HyperMesh CFD Post. To do this, run the AcuTransTrace utility. This tool can be used to convert data for Ensight, FieldView or AcuDisplay.
1. Click the Convert tool.
The AcuTrace Data Translator window opens.
2. Browse to the location where the AcuTrace log file (*.tlog) is located.
3. Set the Output format to Ensight.
4. Set Data type to Time Cut.
5. Click Convert.
Once the conversion is successful, it generates two Ensight result files.
6. Close the dialog.

Post-Process the Ensight File

1. Navigate to the Post ribbon.
2. From the Home tools, Files tool group, click the Open Model tool.
3. Open the Ensight case file (static_mixer.trace.case) in your problem directory to load the results for post-processing.
Note: A warning opens wherein if some results were previously loaded it will try to remove the results first then load the current results. Click Continue.
The solid and all the surfaces along with the Particles are loaded in the Post Browser.
4. In the Post Browser, turn off the display for all surfaces except for Pipe Wall and Fin Walls.
5. Set the transparency for Fin Walls to around 30% and the transparency for Pipe Wall to around 80%.
6. Right-click Block8 under Particles and select Edit.
7. Set the display to Radius. Click and set the point radius to 0.003.
8. Activate the Legend toggle and click to refresh the range.
9. Click and set the colormap name to Rainbow Desaturated, the colormap style to Filled, and the number of colors to 2.
10. Switch to the Display properties. Set the Orientation to Horizontal and select the Lower Center button.
11. Click the Isometric face on the View Cube to align the model.
12. Rotate the model as shown in below figure such that you can view the particles movement inside the domain more precisely.
13. Click at the bottom of the modeling window to view a live animation of the flow.
14. Save the animation.
1. Go to File > Screen Capture > Advanced Screen Capture.
2. Click and uncheck Include mouse cursor.
3. Set the frame rate to 30.
4. Click on the toolbar then drag over the area you want to record.
5. Click to begin recording and the same icon to stop recording.
6. Name the file and save it.

Summary

In this tutorial, you successfully set up and solved for a steady simulation of a static mixer to visualize the particle flow. You started the tutorial by opening a database in HyperMesh CFD and setting up the simulation parameters to compute the species mixing within the mixer. Then, you set up the particle seeds and ran AcuTrace to generate the particles flow within the static mixer. Lastly, you converted the data using AcuTransTrace to visualize the particles flow in HyperMesh CFD Post.