# ACU-T: 5202 Flow Closing Valve

This tutorial provides the instructions for setting up, solving and viewing results for a simulation of a flow closing valve. In this simulation, AcuSolve is used to set up the motion of the valve from open to a fully closed configuration. This tutorial is designed to introduce you to modelling concepts necessary to perform mesh motion simulations involving near contact simulations.

The basic steps in any CFD simulation are shown in the ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The basic steps involving rigid body mesh motion are shown in the ACU-T: 5200 Rigid-Body Dynamics of a Check Valve. The following additional capabilities of AcuSolve are introduced in this tutorial:

• Creating a mesh motion with mesh distortion correction
• Creating advanced solution strategy parameters for mesh displacement stagger
• Creating multiplier function for translational mesh motion in terms of velocity or displacement
• Using the ogden model associated with Arbitrary Lagrangian Eulerian (ALE) mesh movement technology to run the simulation

In this tutorial, you will do the following:

• Analyze the problem
• Start AcuConsole and work with an existing database
• Set advanced simulation parameters
• Create a mesh motion to simulate near contact
• Assign mesh distortion correction parameters
• Create a multiplier function associated with velocity or, alternatively, displacement
• Edit the configuration file to run AcuSolve using the ogden ALE
• Monitor the solution with AcuProbe
• Post processing the time series output with AcuProbe
• Post processing the nodal output with AcuFieldView

## Prerequisites

In order to run this tutorial, you should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow and ACU-T: 5200 Rigid-Body Dynamics of a Check Valve tutorial. It is assumed that you have 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 Closing_Valve.acs from AcuConsole_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 problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of a rectangular channel with two flow paths, one of which may be closed by a valve.

The inlet height is 0.2 meters and the length of the domain is 1.0 meter. The initial position of the valve is at 9.165 millimeters from the opening, thus simulating an open condition.

The valve moves at a constant speed of 18.33 mm/s towards and away from the opening during a time duration of 1 second.

Note that AcuSolve cannot simulate near contact configuration with the default settings. The mesh distortion correction and mesh stagger parameters need to be tweaked to allow the mesh elements to collapse and recover given sufficient iterations.

## Define the Simulation Parameters

### Start AcuConsole and Open the Existing Simulation Database

In the next steps you will start AcuConsole and open the existing database for storage of additional simulation settings. In this tutorial, you will begin by opening a database, creating advanced simulation settings for flow, turbulence, and mesh stagger, and creating the required mesh motion. Next, you will create a multiplier function based on velocity or displacement, modify mesh distortion parameters, and assign the mesh motion to the moving surface. Then, you will run AcuSolve to solve for the number of time steps specified. Finally, you will visualize some characteristics of the results using AcuFieldView.

1. Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
2. Click File > Open to bring up the Open data base dialog.
Note: You can also bring up the Open data base dialog by clicking on the toolbar.
3. 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. The AcuConsole database file (.acs) is stored in this directory. Once the mesh and solution are created, additional files and directories will be created within this directory.
4. Select Closing_Valve.acs and click Open to open the database.
Note: In order for other applications to be able to read the files written by AcuConsole, the database path and name should not include spaces.

Once you open the database, you will notice that the geometry, mesh, simulation settings, and most of the boundary conditions have already been populated in the file.

### Set Advanced Simulation Parameters

In the database, the general simulation, solution strategy, material model, and mesh parameters have already been created.

In next steps, you will create and set the advanced solution strategy parameters that apply to the simulation. To make this as simple as possible, you will use the PB* filter in the Data Tree Manager. This filter reduces the number of items shown in the Data Tree and makes navigation of the entries easier.

1. Click PB* in the Data Tree Manager to display all the available settings related to general problem setup in the Data Tree.
2. Under the Global Data Tree item, double-click Advanced Solution Strategy, then double-click the Stagger tree.

The advanced solution strategy tree contains settings that can be used to finely tune the solver parameters, such as time increment, time marching, staggers, linear solver, convergence check, etc.

The stagger command specifies the nonlinear iteration and linear solver parameters for the solution of an equation. Each stagger loops over several nonlinear iterations, within which the residual, and optionally, the LHS matrix of the stagger are formed, the resulting linear equation system is solved, the corresponding solution field is updated, and its sub-staggers are executed.

3. Double-click on the mesh_displacement stagger to bring up the detail panel.
4. Turn on Modify advanced settings.
5. Set the Min stagger iterations and Max stagger iterations to 1 and 5 respectively.
6. Set the Convergence tolerance to 0.01.

## Assign Mesh Controls

### Create a Multiplier Function

1. Click PB* in the Data Tree Manager to display all the available settings related to general problem setup in the Data Tree.
2. Expand the Global Data Tree item.
3. Create a new multiplier function named Velocity_Multiplier.
4. Define the multiplier function parameters.
1. Double-click Velocity_Multiplier to open the detail panel.
2. Click the drop-down control next to Type and select Piecewise Linear.
3. Click the drop-down control next to Curve fit variable and select Time step.
4. Click on the Open Array tab next to Curve fit values.
5. Click Add twice to add two more rows.
6. Enter the time step values as shown in the image below.
7. Click Plot << to see the plot of the multiplier function.
8. Click OK to close the window.

### Create Velocity-Based Mesh Motion

AcuSolve uses the mesh motion command to define the movement of nodes within the model. In this tutorial, you will use a translational mesh motion to determine the motion of the nodes.

A multiplier function is used to scale values as a function of time or time step. In this tutorial, the stop valve moves towards and away from the opening at a constant speed. This variation is accomplished by assigning a multiplier function to the mesh motion.

In the next steps, you will create a mesh motion to simulate the motion of the valve.

1. Click FSI in the Data Tree Manager to filter the settings in the Data Tree to show only those related to mesh motions and fluid/structure interactions.
2. Double-click the Global Data Tree item to expand it.
3. Right-click Mesh Motion and click New.
4. Rename the mesh motion.
1. Right-click Mesh Motion 1.
2. Click Rename.
3. Type Valve_Motion and press Enter
5. Define the mesh motion parameters.
1. Double-click Valve_Motion to open the detail panel.
2. Change the Type to Translation.
3. Click Open Array next to Translation velocity to open the array editor.
4. Change the units to mm/sec and enter -18.33 in the X-component field.
This corresponds to the x component of the velocity defining the mesh motion.
5. Click OK to close the editor.
6. Click the drop-down next to Velocity variable and select Multiplier function.
A new option called Translation multiplier function becomes available.
7. Set Translation multiplier function to Velocity_Multiplier.

When this translation mesh motion is defined, the nodes of the element set move at a constant velocity of 18.33 mm/s in the negative x direction. For this case, the location of each node in the element set is given by:

(1) $x={x}_{0}+tv$

Where ${x}_{0}$ is the initial condition of the node, $v$ is given by translation velocity, and $t$ is time.

A multiplier function can be defined with velocity_variable=multiplier_function to modify the scaling of velocity. Then the location of each node is given by:

(2) $x={x}_{0}+fv$

Where $f$ is the given translation variable multiplier function.

### Create Displacement-Based Mesh Motion

An alternate approach for defining a multiplier function for translation mesh motion is to define a unit (1.0) velocity value in the mesh motion and assign the displacement of the moving body to the multiplier function directly.

This approach is particularly useful in cases where you are given the displacement-time values or curves defining the motion of the moving body.

In the next steps, you will define the mesh motion and multiplier function based on the approach discussed in previous sections.

1. Define a translation mesh motion using the same process and parameters as previously described.
Important: You should not keep two sets of mesh motions and multiplier functions. Given your simulation parameters, this section is intended as a substitute to velocity-based mesh motions.
2. Set the X-velocity to 1.0 m/sec in the X-component field of the array editor.
3. Create a multiplier function called Displacement_Multiplier using the same process and parameters as described in the previous section
4. Enter the displacement values for the curve fit variables in the array editor, as shown in the image below.

This approach allows you to define the motion of the valve based on the displacement against the time steps.

### Assign Mesh Distortion Parameters

When AcuSolve is performing a moving mesh simulation, a check is performed to detect the presence of bad elements. If any highly distorted element are found, the code either exits (when mesh=specified or mesh=eulerian) or adds more non-linear iterations with an incremental update strategy (when mesh=ale). Two parameters control the algorithm: mesh_distortion_tolerance and mesh_distortion_correction_factor. The first parameter determines whether the correction needs to be applied to the element Jacobian and the second quantifies the amount of correction. Mesh distortion is checked within the ALE loop, and then acuSolve decides how forgiving it should be to highly distorted elements.

In the next steps you will assign the values of mesh distortion parameters to the fluid volume.

1. Expand the Model tree.
Note: You'll need to switch back to BAS in the Data Tree Manager.
2. Expand Volumes.
3. Double-click Fluid to expand the tree then double-click Element Set to open the detail panel.
4. Enter 0.0005 as the value for the Mesh distortion correction factor.
5. Enter 0.05 as the value for the Mesh distortion tolerance.

### Assign Mesh Motion to the Valve Surface

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.

The database has all the volume and surface groups already assigned.

In the next steps, you will assign the created mesh motion to the valve surface.

1. Expand Surfaces.
2. Double-click Valve_Wall to expand the tree then double-click on Simple Boundary Condition to open the detail panel.
3. Click the drop-down menu next to Mesh motion and select Valve_Motion.

## Compute the Solution and Review the Results

### Run AcuSolve

In order to use the ogden model associated with Arbitrary Lagrangian Eulerian (ALE) mesh movement technology, you need to add the corresponding flag in the configuration file and then run the simulation using the AcuSolve command prompt.

In the next steps, you will run AcuPrep from the GUI, edit the configuration file, and launch AcuSolve from the command prompt in order to get a solution for this case.

1. Click on the toolbar to open the Launch AcuSolve dialog.
For this case, only the AcuPrep module will be used, and AcuConsole will generate AcuSolve input files and launch AcuSolve.
2. From the drop-down menu next to Solver modules, select prep.
3. Click Ok to launch the AcuPrep process.
This will generate the input files and a configuration file called Acusim.cnf.
4. Browse to your working directory, open Acusim.cnf in a text editor, and add the following line to the end of the file: aletech=ogden.
This will cause AcuSolve to use the ogden model to run the simulation.
5. Start AcuSolve command prompt from the Start menu by clicking Start > All Programs > Altair HyperWorks <version> > AcuSolve > AcuSolve Cmd Prompt.
6. Browse to your working directory using the cd command.
7. Launch AcuSolve with the command AcuRun -np 4 -nt 1 -do solve to run the simulation with four processors and only the solver module.
Note: The solution progress can be monitored by launching AcuTail using the icon from the toolbar and selecting the log file from your working directory.
After AcuSolve has finished running, a summary of the solution process indicates that the simulation has been completed.

### Post Process with AcuProbe

After the simulation is complete, the plot for mesh_x_displacement can be viewed using AcuProbe.

1. Open AcuProbe by clicking on the toolbar.
2. In the AcuProbe window, double-click on Surface Output to expand the tree.
3. Double-click on Valve_Wall to open the surface output list.
4. Double-click on Geometry to open the list of properties related to geometry.
5. Right-click on mesh_x_displacement and click plot.
Note: You might need to click on the toolbar in order to properly display the plot.

Other flow quantities can also be plotted using AcuProbe.

### View Results with AcuFieldView

Now that a solution has been calculated, you are ready to view the flow field using AcuFieldView. AcuFieldView is a third-party post-processing tool that is tightly integrated to AcuSolve. AcuFieldView can be started directly from AcuConsole, or it can be started from the Start menu, or from a command line. In this tutorial you will start AcuFieldView from AcuConsole after the solution is calculated by AcuSolve.

In the following steps you will start AcuFieldView, display velocity magnitude and animate the view to show mesh displacement. You will then display velocity vectors and pressure contours when the valve shutter is closed.

This tutorial has 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 graphics window using mouse actions to translate, rotate and zoom in to the data.

This tutorial shows you how to work with transient data. It also shows how to visualize the flow parameters on the complete geometry when only a section of it is simulated in AcuSolve by using multiple datasets.

#### Start AcuFieldView

1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
2. Click Ok to start AcuFieldView.
When you start AcuFieldView from AcuConsole, the results from the last time step of the solution that were written to disk will be loaded for post-processing.

Once AcuFieldView opens, you will see that the pressure contours have already been displayed on all the boundary surfaces with mesh.

#### Animate the Display of Velocity Magnitude Contours

In the next steps you will create a transient sweep and save it as an animation that can be viewed independently of AcuFieldView.

1. Change the background color to white.
2. Disable perspective view from the Viewer Options menu.
3. Disable the axis markers from the Viewer Options menu.
4. Orient the geometry so you can see the wall, the inlet, and the symmetry+Z surface as shown in the figure below.
5. In the Boundary Surface dialog, select velocity magnitude as the Scalar Function.
6. Turn on the legend in the legends tab and change the color to black from the color palette.
Note: You can move the legend using Shift + left click.
7. Change the annotation color to black.
8. Turn off the display for the mesh by unchecking the Show Mesh option under the Surfaces tab.
9. Go to Tools > Flipbook Build Mode and click OK on the warning displayed.
10. Go to Tools > Transient Data and move the slider all the way back to reflect the first time step data on the boundary surface.
11. Click Build to build the animation.
12. Once the animation is built, click on Frame Rate and change the value to 0.1.
13. Save the animation as velocity_mag.

#### Display Pressure Contours and Velocity Vectors on a Mid-Z Coordinate Surface at Valved Closed Position

1. From the Boundary Surface dialog, under the surfaces tab, disable the visibility for the boundary surfaces.
2. Change the view to +Z from the Defined Views menu.
3. Click to open the Coordinate Surface dialog.
4. Create a new surface at the mid Z coordinate plane.
5. Change the Display Type to Smooth.
6. Change the Coloring to Scalar.
7. Select pressure as the Scalar Function to be displayed.
8. Set Scalar Coloring to Local from the Colormap tab.
9. Create another coordinate surface and set the Display Type to Vectors.
10. Change the coloring to Geometric and select white from the color palette.
11. Click Options to open the Vector Options dialog.
12. Check Skip and enter 62.5%.
13. Turn the legend on for the pressure coordinate surface.
14. Go to Tools > Transient Data and move the slider to the 50th time step.