This tutorial will cover all the set-up steps, but we recommend that you work through the Forte Quick Start Guide first and become familiar with the workflow of the Ansys Forte user interface.

The files for this tutorial are obtained by downloading the fsi_pulse_jet.zip file here .

Unzip the fsi_pulse_jet.zip to your working folder.

Files provided in this tutorial include a Forte project file that has been fully configured as well as a set of facilitating input files that can be used to set up the Forte project starting from a blank project. Specifically, the files include:

Forte may be launched in a command line mode to perform certain tasks such as preparing a run for execution, importing project settings from a text file, or various other tasks described in the Forte User's Guide. One of these tools allows exporting a textual representation of the project data to a text file.

Example

forte.sh CLI -project <project_name>.ftsim -export tutorial_settings.txt 

Briefly, you can double-check project settings by saving your project and then running the command-line utility to export the settings in your tutorial project (<project_name>.ftsim), and then use the command a second time to export the settings in the provided final version of the tutorial. Compare them with your favorite diff tool, such as DIFFzilla. If all the parameters are in agreement, you have set up the project successfully. If there are differences, you can go back into the tutorial set-up, re-read the tutorial instructions, and change the setting of interest.

This Forte project is set up with a final simulation time of 2 ms. As a guideline for your own simulations, this tutorial is estimated to take approximately 3 hours on a Linux cluster using an Intel 2.6 GHz processor (84 cores).

In this tutorial, we will import an existing geometry into Ansys Forte and set up the automatic mesh generation using a global mesh size and adapting the mesh where extra resolution is needed. To import the geometry, go to the Workflow tree and click Geometry. This opens the Geometry icon bar. Click the Import Geometry   icon. In the resulting dialog, pull down and select Surfaces from one or more STL files, then select the provided STL file, valved_pulse_jet.stl. In the dialog that opens with STL file import options, accept the defaults. The mesh will be automatically generated during the simulation. Note that once you have imported the geometry, there are a number of actions that you can perform to modify the provided project on the items in the Geometry node, such as scale, rename, transform, invert normals, or delete geometry elements. Use the   button to fit the entire geometry in the graphic window.

To later allow easy identification of the bending direction of the reed, let us create one local reference frame for each valve. From the Geometry node, select Reference Frames and create the new reference frames. Their origins are indicated in Table 21.2: New reference frame origins in global coordinates.

In the configured project that you previously downloaded, you can also see that a clip plane is created to allow a better view of the various components and reference frames, and a Sub-Volume region named Chamber.

The mesh creation occurs on-the-fly during the simulation, however, there are a few parameters that need to be set in the Mesh Controls node:

Material Point: This is needed to identify the simulation domain where the mesh will be generated. It should be located at least one unit cell length away from any boundaries and must be inside of the domain throughout the entire simulation. Set it at the Global Origin.

Global Mesh Size: Set the Global Mesh Size to 4 mm.

Refinements: These are needed to refine the mesh around key geometry features. They are of different types, those used in this tutorial are: Surface Refinement Depth, SAM (Solution Adaptive Mesh) , and Gap Feature Control. The Gap Feature Control automatically detects small gaps between the specified surface pair based on the user-specified Surface Proximity criterion and applies refinement in the detected gap region based on the user-specified refinement level. When Gap Feature Control is used, the spatially resolved solution will contain a variable called GapCellFlag, which uses non-zero integer values to mark the zones identified as gap zones. Detailed mesh control parameters are listed in Table 21.3: Settings for Mesh Control refinements.

All the settings in this node can be kept as the default, but don’t forget to import the provided chemistry set. Specifically:

Chemistry set: The chemistry input file used in this tutorial is the default NaturalGas_1comp_29sp.cks and it can be found in your Forte installation path inside the subfolder, Program Files\ANSYS Inc\V242\reaction\forte.win64\data\. To use it, navigate to the Chemistry module, click the New Import Chemistry   icon and select the chemistry set, NaturalGas_1comp_29sp.cks.

Boundary conditions must be specified for each of the geometry elements. To match the provided project, follow these instructions for each boundary condition:

Inlet: Defined as an inlet boundary  . Set the Mole Fraction Composition to be 1 ch₄, 7.52 n₂, and, 2 o₂ and the location is inlet. Then select Total Pressure, Time Varying, set Time as a Time Option. Next to Pressure Profile select Create new... and then click the Edit button  . Once the Editor panel opens, click Load CSV to upload the provided pressure profile (PulsedPressureProfile.csv). The Total Temperature is 600 K and the Turbulence parameters are kept at the default values.

Outlet: Defined as an inlet boundary  , to force the reverse flow condition to be explicitly defined. Set the Mass Fraction Composition as air, 0.24 o₂ and 0.76 n₂, and the location to be outlet. The Total Pressure is set to 2 bar and the Total Temperature to 350 K. Turbulence parameters are kept at the default values.

Chamber: Defined as a wall boundary  . The location selection lists center_ring, chamber, chamber_flat. The Heat Transfer check box is selected, the Wall Temperature is constant at 350 K, and the Heat Transfer Model in use is the Han-Reitz Model.

Diffuser: Defined as a wall boundary  . The location selection lists the diffuser and the rings. The Heat Transfer check box is selected, and the Wall Temperature is constant at 600 K, and the Heat Transfer Model in use is the Han-Reitz Model.

Spark: Defined as a wall boundary  . The location selection lists only the spark_plug. The Heat Transfer check box is selected, and the Wall Temperature is constant at 450 K, and the Heat Transfer Model in use is the Han-Reitz Model.

Then add the following boundary condition to each reed valve, replacing X with the number of each valve.

Reed X: Defined as a wall boundary  . The location selections are reedX and reedX_bottom. The Heat Transfer check box is NOT selected.

The entire domain is initialized with the premixed composition listed in Table 21.1: Dimensions and operating conditions, and a constant Temperature and Pressure of 350 K and 2 bar, respectively.

The first setting in the Simulation Controls node is Time Based as the simulation option. Then set the Max. Simulation Time to be 2 ms.

Time Step: Only two parameters differ from the defaults to accommodate a larger time step without affecting much the accuracy and the stability of the solution. These are the Fluid Acceleration Factor, set to 2 and the Rate of Strain Factor, set to 2.4.

Built-in FSI : Activate the Built-in FSI feature by checking the box, click the   icon to create a new "Bending Beam" and name it Reed 1. Now, select the Reed 1 in the location list and choose Point Load in the Load Type option. Assuming that the reed valves are made of steel, set the Young's Modulus to 1.8e5 MPa. Select the Enable Inertial and Damping Effects check box, and set the Mass of Body to be 6 mg. Then set the other parameters as shown in Figure 21.3: Built-in FSI Bending Beam panel. The figure also shows the Reed 1 reference frame previously specified in Table 21.2: New reference frame origins in global coordinates; use it in the Fixed End Position, the Neutral and Beam Axis panels. The Fixed End Position specifies the origin of the beam and it corresponds to the origin of the Reed 1 reference frame, so all the coordinates are set to 0 cm. Then the Neutral Axis is the direction along the main dimension of the beam, set it to Z = 1 cm. Finally the Beam Axis is the axis by which the beam will rotate, with positive deflection given by the right-hand rule, set it to Y = 1 cm. Now repeat the above steps to model for all the other valves as bending beams, making sure to replace each time their selected location and the reference frames for the Fixed End Position, the Neutral and the Beam Axes. In all the Bending Beams the Restrict to Positive Displacement box is checked to constrain the valve motion. The Max. Travel Per Step is set to 0.05. This represents the maximum deflection of the beam as a fraction (5%) of the maximum displacement (1 cm) between mesh updates.

Figure 21.3: Built-in FSI Bending Beam panel

Output controls determine what data are stored for viewing during the simulation and for creating plots, graphs and animations in Ansys EnSight.

Spatially Resolved: Allows you to control when spatially resolved data such as velocity, temperature, pressure, etc., will be output. In the Spatially Resolved panel, set the Time Output Control to report every 0.1 ms. You can optionally increase the frequency of output to create smoother animations. Select then the Solution Count in the File Size Control and set the Solutions per Results File to 1 to have a single *.ftres per each output Time. Amongst the Spatially Resolved Species and Solution Variables, select variables of your interest like Pressure, Temperature, VelocityX, VelocityY, VelocityZ and Velocity Magnitude.

Spatially Averaged and Spray: Opt for Time and set the interval to 10 µs, then choose the species of interest if any.

Restart Data: This option allows a restart file to be saved at the end of the current simulation if the Write Restart File at Last Simulation Step option is checked. Such a restart file is useful if you decide to extend the simulation duration to do parameter studies because it provides a much better guess for initial condition than a uniform one.

Monitor Probes: Choose an Inquiry Frequency of 1 µs then create two monitor probes of type Geometric and shape Spherical with a 7 mm radius. Place them at 8 mm and -9 mm in the x-direction and 4.4 cm in the z-direction with respect to the Reed 3 reference frame and name them Chamber_sphere_reed3, and Diffuser_sphere_reed3, respectively. Let the probe output Pressure and Temperature.