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_piston_pump.zip file here .

Unzip fsi_piston_pump.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:

The tutorial sample compressed archive is provided as a download. You have the opportunity to select the location for the file when you download and uncompress the sample files.

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 to run for three complete revolutions. As a guideline for your own simulations, this tutorial is estimated to take approximately 25 hours on a Linux cluster using an Intel 2.6 GHz processor (112 cores).

In this tutorial, we 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, piston_compression_pump.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 Refit button   to fit the entire geometry in the graphic window.

To allow later easy identification of the direction of the valves and piston motion, create one local reference frame per valve plus one for the main chamber. From the Geometry node, turn ON the Reference Frames and create the new reference frames as indicated in Table 20.2: New Reference Frame Origins in global coordinates.

In the already set-up project that you have previously downloaded, you can also see that a clip plane is created to allow a better view of the various components and reference frames, as shown in Figure 20.2: Clip view of the Geometry and Reference Frames.

Figure 20.2: Clip view of the Geometry and Reference Frames

The mesh creation occurs on-the-fly during the simulation. However, there are several parameters that must be set in the Mesh Controls node:

Material Point: It 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. Place it at the origin of the Main_Chamber_RF.

Global Mesh Size: Specify as 2 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 20.3: Settings for Mesh Control refinements. The Active property is set to Always for all the mesh controls.

All the settings in this node can be left at the default settings (as described in the Note in Files Used in This Tutorial), but do not forget to import the provided chemistry set into the project.

Boundary conditions must be specified for each of the geometry elements. In the already set-up project, you can find the following boundary conditions:

Inlet: Defined as an inlet boundary  . Set the Mole Fraction Composition to be 0.21 o2_in and 0.79 n2_in, and the selected location is inlet. The Static Pressure is set to 1 bar and the Total Temperature to 300 K. 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 Mole Fraction Composition to be 0.21 o2_out and 0.79 n2_out, and the selected location is outlet. The Static Pressure is set to 5 bar and the Total Temperature to 350 K. Turbulence parameters are kept at the default values.

Walls: Defined as a wall boundary  . The location selection lists connector_wall, discharge_pipe, discharge_seat, head, intake_pipe, intake_seat, liner. The Heat Transfer check box is selected and the Wall Temperature is constant at 300 K.

Piston: Defined as a wall boundary  . The location selection lists only the piston. The Heat Transfer check box is selected and the Wall Temperature is constant at 300 K. The Wall Motion is activated with type Slider Crank, Stroke = 10 cm, Connecting Rod Length = 15 cm and Direction of motion set to Y = 1 cm.

Intake_Valve: Defined as a wall boundary  . The location selection lists intake_valve_narrow_end, intake_valve_side, intake_valve_wide_end. The Heat Transfer check box is NOT selected.

Discharge_Valve: Type wall. The location selection lists discharge_valve_narrow_end, discharge_valve_side, discharge_valve_wide_end. The Heat Transfer check box is NOT selected.

The entire domain is initialized with air, 0.21 o2 and 0.79 n2 concentration (note that this is the "original" air, not one of the duplicates), with a constant Temperature and Pressure of 450 K and 5 bar, respectively, since the initial piston location is at its top dead center and therefore the main chamber conditions are closer to the outlet pipe.

For the Simulation Controls node, first select the Crank Angle Based simulation option. Then set the initial Crank Angle to be 0 and the final to be 1080 degrees, since the cycle type is only 2-stroke and we want to have 3 full cycles. The piston RPM is 3000.

Time Step: Keep these parameters at their default values.

Chemistry Solver: Set the Activate Chemistry option to Always Off because this simulation does not involve chemical reactions.

Built-in FSI: Activate the Built-in FSI feature by checking the box, click the   icon to create a new spring mass-system and name it Intake_Spring. Now, select the Intake_Valve in the location list and choose Linear in the Spring Type option. Then set the other parameters as shown in Figure 20.3: Built-in FSI Spring-Mass-System Editor panel, and don't forget to select the Intake_Valve_RF as reference frame in the Direction panel with the only non zero component being in the x direction. Repeat the above steps to create the Discharge_Spring as new Spring-Mass-System. This time use a Mass of Body of 15 g, a Preload Displacement of 2 mm, and use the Discharge_Valve_RF and a single X = 1 component in the Direction panel. In both Spring-Mass-Systems, the Restrict to Positive Displacement box is checked to constrain the valve motion. The Max. Travel Per Step is set to 1; in case you want to modify the tutorial tune this parameter to fix the maximum valve motion per each time step. For example, a value of 0.05 will force the valve to move by only 5% of the computed displacement for that step.

Figure 20.3: Built-in FSI Spring-Mass-System Editor 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, species concentrations, etc., will be output. In the Spatially Resolved Editor panel, set the Crank Angle Output Control to report every 20 degrees (to manage the size of the output file). You can optionally increase the frequency of output during the cycles to create smoother animations. Select the Solution Count in the File Size Control option and set the Solutions per Results File to 1 to have a single *.ftres per each output Crank Angle. For 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: Select Crank Angle and set the interval to 0.5 degrees, then choose the species of interest.

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 0.5 degrees and then create three monitor probes of type Geometric and shape Spherical with a 5 mm radius. Place them at 2.5 cm, 12 cm, and 7.1 cm in the x-direction with respect to the global origin reference frame and name them Intake_Probe, Discharge_Probe, and Chamber_Probe, respectively. Select probe outputs of Pressure and Temperature.