# ACU-T: 6000 Static Mixer Simulation - AcuTrace

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 module AcuTrace. 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 streamlines and produce particle path with AcuTrace.

TThe basic steps in any CFD simulation are shown in ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The following additional capabilities of AcuSolve are introduced in this tutorial:
• Generation of finite mass particle paths with AcuTrace.
• Conversion of the nodal output data with AcuTranstrace for reading into AcuFieldView.
• Post-processing the nodal output with AcuFieldView to visualize streamlines and particle path.

## Prerequisites

You should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

Prior to running through this tutorial, copy AcuConsole_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract StaticMixer.acs from AcuConsole_tutorial_inputs.zip.

## Analyze the Problem

An important step in any CFD simulation is to examine the engineering problem 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 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 inlet face is split into two regions, one containing 100 percent of species_1 and the other containing zero.

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 are 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.

In addition to setting appropriate conditions for the simulation, it is important to utilize a mesh that will be sufficiently refined to provide good results. In this application, the flow will accelerate as it passes over the fin walls. This leads to the higher gradients that need finer resolution. Proper boundary layer parameters need to be set to keep the y+ near the wall surface to a reasonable level. Although a slightly refined mesh is used in this area, it should be noted that a proper mesh refinement study is necessary in order to determine the required mesh controls to obtain a grid independent solution. The mesh controls used in this tutorial are very coarse and are only intended to illustrate the process of setting up the model and to retain a reasonable run time. A significantly higher mesh density is needed to achieve a grid converged solution.

## Define the Simulation Parameters

### Start AcuConsole and Create the Simulation Database

In the next steps you will start AcuConsole, and open the database for storage of the simulation settings. In this tutorial, you will begin by loading the existing database, preparing the particle trace settings and running the model. Next you run AcuTrace to generate the particle paths within the flow field and convert the data for reading into AcuConsole. Finally, you will visualize some characteristics of the results using AcuConsole.

1. Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
2. Click the File menu, then click Open to open the Chose a file dialog.
3. Browse to the directory where StaticMixer.acs is stored.
4. Select StaticMixer.acs and then click Open to open the database.

### Set General Simulation Parameters

In next steps you will review parameters that apply globally to the simulation. To make this simple, the basic settings applicable for any simulation can be filtered using the BAS filter in the Data Tree Manager. This filter enables display of only a small subset of the available items in the Data Tree and makes navigation of the entries easier.

The general parameters that you will set for this tutorial are for turbulent flow, steady analysis, and mesh type as fixed.

1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
2. Double-click the Global Data Tree item to expand it.
Tip: You can also expand a tree item by clicking next to the item name.
3. Double-click Problem Description to open the Problem Description detail panel.
Tip: You can also open a panel by right-clicking a tree item and clicking Open on the context menu.
4. Enter Mixing_tube as the Title.
5. Enter Steady State as the Sub title.
6. Change the Analysis type to Steady State.
7. Set the Species equation to Advective Diffusive.
8. Change the Turbulence equation to Spalart Allmaras.
9. Set the Mesh type to Fixed.

### Set Solution Strategy Parameters

1. Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
2. Check that the Analysis type is set to Steady State.
3. Set the Max time steps as 100.
4. Check that the Convergence tolerance is set to 0.001 seconds.
5. Set the Relaxation factor to 0.4.
The relaxation factor is used to improve convergence of the solution. Typically a value between 0.2 and 0.4 provides a good balance between achieving a smooth progression of the solution and the extra compute time needed to reach convergence. Higher relaxation factors cause AcuSolve to take more time steps to reach a steady state solution. A high relaxation factor is sometimes necessary in order to achieve convergence for very complex applications.

### Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum, and Water, with standard parameters defined. For this tutorial you will use a newly defined material model, “Epoxy Resin” which has been preloaded into the AcuConsole database. In the next steps you will check the material characteristics of the predefined "Epoxy Resin" to match the desired properties for this problem.
1. Double-click Material Model in the Data Tree to expand it.
2. Double-click Epoxy Resin in the Data Tree to open the Epoxy Resin detail panel.
3. Click the Density tab. The density of the epoxy is 1264.0 kg/m3.
4. Click the Viscosity tab. The viscosity of the resin is 1.49 kg/m – sec.
5. Save the database to create a backup of your settings. This can be achieved with any of the following methods.
• Click the File menu, then click Save.
• Click on the toolbar.
• Click Ctrl+S.
Note: Changes made in AcuConsole are saved into the database file (.acs) as they are made. A save operation copies the database to a backup file, which can be used to reload the database from that saved state in the event that you do not want to commit future changes.

### Prepare Output Data Stream

In order to utilize the finite mass particle trace functionality for particles that have non-constant density, you are required to store additional variables during the simulation. This is done by using the Derived Quantity Output mechanism.

1. In the Data Tree, double-click Output to expand it.
2. Double-click Nodal Output.
3. Change the Time step frequency to 1000.
4. Set the Time frequency to 0.
5. In the Data Tree, double-click Derived Quantity Output to open the Derived Quantity Output detail panel.
6. Change the Time step frequency to 1000.
7. Set the Time frequency to 0.

## Compute the Solution and Review the Results

### Run AcuSolve

In the next steps you will launch AcuSolve to compute the solution for this case.

1. Click on the toolbar to open the Launch AcuSolve dialog.
Note: For this case, the default values will be used. AcuSolve will run using four processors, and AcuConsole will generate AcuSolve input files and will launch AcuSolve. AcuSolve will calculate the steady state solution for this problem.
2. Click Ok to start the solution process.

While computing the solution, an AcuTail window opens. Solution progress is reported in this window. A summary of the solution process indicates that the run has been completed.

The information provided in the summary is based on the number of processors used by AcuSolve. If you use a different number of processors than indicated in this tutorial, the summary for your run may be slightly different than the summary shown.

3. Close the AcuTail window and save the database to create a backup of your settings.

### Monitor the Solution with AcuProbe

AcuProbe can be used to monitor residuals.

1. Open AcuProbe by clicking on the toolbar.
2. In the Data Tree on the left, expand Residual Ratio.
3. Right-click on Final and select Plot All.
The Solution ratio measures how much the solution is changing from one step to the next.
Note: You might need to click on the toolbar in order to properly display the plot.

### Prepare Particle Trace Attribute 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

In the next steps you will define the particle trace data.

1. In AcuConsole, click ALL in the Data Tree Manager to see all settings in the Data Tree.
2. In the Data Tree, expand Particle Trace to show only items related to particle tracing.
3. Double-click Problem Description to open the Problem Description detail panel.
4. For Particle equation, select Finite mass.
5. In the Data Tree, double-click on Flow Field to open the detail panel.
6. Set the Flow field type to Static as this is a static analysis.
7. In the Data Tree, double-click on Finite Mass to open the detail panel.
8. Verify that Density model is set to Use flow values.
In order to utilize the Use flow values option, the derived quantity output needs to be specified. If the derived quality output is not available, you can select Constant and enter in a Constant density value. This allows the particles to maintain a specified value for density.

#### Define Finite Mass Boundary Conditions

In the next steps you will set the finite mass boundary conditions.

1. Under Particle Trace, right-click on Finite Mass Boundary Condition and select New.
2. Right-click on Finite Mass Boundary Condition 1 and select Rename.
3. Enter the new name as SideWalls.
4. Double-click on SideWalls to open the Finite Mass Boundary Condition panel.
5. Set the Particle surface to Pipe Wall.
6. Leave the Wall type set to Reflect and the Normal and Tangential coefficient of restitution type set to Constant.
7. Enter 0.2 for both the Normal and Tangential coefficient of restitution.
8. In the Data Tree, right-click on Finite Mass Boundary Condition and select New.
9. Rename Finite Mass Boundary Condition 2 to FinWalls.
10. Double-click FinWalls to open the Finite Mass Boundary Condition panel.
11. Set the Particle surface to Fin Walls.
12. Leave the Wall type set to Reflect and the Normal and Tangential coefficient of restitution type set to Constant.
13. Enter 0.8 for both the Normal and Tangential coefficient of restitution.
This will allow for less energy to be lost when the particle hits the wall and in turn will reflect off of the wall with a greater velocity.

#### Define Particle Seeds

In the next steps you will define the particle seeds that are moving into the flow regime.

1. Under Particle Trace, right-click on Particle Seed and select New.
2. Rename Particle Seed 1 and to S1.
3. Double-click on S1 to open the Particle Seed panel.
4. For Coordinates type, select Surface Random.
5. For Particle surface, select Inlet S1.
6. For Number of seeds, enter 500.
7. For Constant density, enter 200.
8. For Constant radius, enter 0.0001.
9. Under Particle Trace, right-click on Particle Seed and select New.
10. Rename Particle Seed 1 and to S2.
11. Double-click on S2 to open the Particle Seed panel.
12. For Coordinates type, select Surface Random.
13. For Particle surface, select Inlet S2.
14. For Number of seeds, enter 500.
15. For Constant density, enter 200.
16. For Constant radius, enter 0.00015.

#### Define the Output Parameters

In the next steps you will define the output parameters.

1. Under Particle Trace, expand Output.
2. Check the box for Trace Output.
3. Double-click Trace Output to open the detail panel.
4. For Output frequency, enter 10.
This is equivalent to outputting the streamlines of the data at a frequency that relates the number of segments, or the approximate length of the particles. In order to reduce the amount of disc required in AcuTrace, it is recommended that the output frequency be larger than 1, more specifically, an order of magnitude larger.

### Compute the Particle Paths and Review

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

#### Run AcuTrace

In the next steps, you will launch AcuTrace to compute the solution for this case.

1. Click on the toolbar to open the Launch AcuTrace dialog.
2. Accept the default settings and select Ok to start the solution process.

#### Convert Results for AcuFieldView

Once the run is complete, you need to convert the results so that they can be read in AcuFieldView. To do this, run the AcuTransTrace utility. This tool can be used to convert data for Ensight, FieldView or AcuDisplay.

1. Start AcuSolve Command Prompt from the Windows Start menu by clicking Start > Altair <version> > AcuSolve Cmd Prompt .
2. Change the directory to your working location using the cd command.
3. Enter the command:
acuTransTrace –to fieldview –fvopt streamline,steady

### Post-Process with AcuFieldView

The tutorials have been written with the assumptions that you have become familiar with the AcuFieldView interface and basic operations. In general, it will be helpful to understand the following basics:
• How to find the data readers in the File pull-down on the Main menu and open up the desired reader panel for data input.
• How to find the visualization panels either from the Side toolbar or the Visualization panel pull-downs on the Main menu to create and modify surfaces in AcuFieldView.
• How to move the data around the modeling window using mouse actions to translate, rotate and zoom in to the data.
This tutorial shows you how to work with the steady state data and load a particle paths file.
Launch AcuFieldView from the AcuConsole window using the icon on the toolbar.
You will see that the pressure contours have already been displayed on all the boundary surfaces. The image below was captured with the mesh turned off.

#### Create a Boundary Surface and Coordinate Plane in Mixer

1. In the Boundary Surfaces dialog, change the Coloring to Geometric.
2. Select grey from the color tab.
3. Uncheck the Show Mesh option to turn off the mesh display.
4. From the Boundary Types list, select OSF: Fin Walls and click Ok.
5. Orient the geometry to show that the flow moves from bottom to top of the screen.
6. In the Boundary Surfaces dialog, click Create to create a new boundary surface.
7. From the Boundary Types list, select OSF: Pipe Walls and click OK.
8. Set the Display Type to Outlines and set Coloring to Geometric.

#### Set the Coordinate Surface Showing Velocity Magnitude on the Mid Coordinate Surface

1. Click to open the Coordinate Surface dialog.
2. Click Create to create a new surface.
3. Set the Coord Plane at the mid –Y coordinate surface.
4. Change the Display Type to Constant.
5. Change the Coloring to Scalar.
6. For Scalar Function, select z-velocity as the scalar function to be displayed, and click Calculate.
7. Click the Colormap tab, and change the coloring to Local.
8. Click the Legend tab, and activate the Show Legend check box to display the velocity magnitude values on the coordinate plane.

#### Set the Boundary Surface and Particle Paths

1. Click the Paths icon to open the Particle Paths dialog.
2. Click Import.
3. Browse to the .fvp file created with acuTransTrace and click Open.
4. In the Particle Paths dialog, change the Coloring type to Scalar.
5. Set the Scalar Variable to particle_z_velocity.
6. Click the Legend tab and turn on the legend.

## Summary

In this tutorial, you successfully set up and solved for a steady simulation of a static mixer to visualize the particle path. You started the tutorial by opening a database in AcuConsole and setting up the simulation parameters to compute the species mixing within the mixer. You ran AcuTrace to generate the particle paths within the static mixer and converted the data using AcuTranstrace to visualize the particle paths in AcuFieldView.