This tutorial covers all the set-up steps, but Ansys recommends that you work through the Forte Quick Start Guide first to become familiar with the workflow of the Ansys Forte user interface.

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

Unzip two_stroke_udf.zip to your working folder. The files provided for this tutorial are the following:

All the files related to the UDF are collected inside a UDF_files subfolder:

The tutorial sample file 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 your tutorial project settings by saving your project and then running the command-line utility to export the settings used 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 360 crank angle degrees. As a guideline for your own simulations, this tutorial is estimated to take approximately 10.27 hours on a Linux cluster using an Intel 2.6 GHz processor and 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 TGF file, then select the provided TGF file, 2stroke_UDF_geometry.tgf. In the dialog that opens with TGF file import options, accept the defaults. In exporting this specific geometry from SpaceClaim, our default CAD tool, we used the Fine option for the facet resolution, with a maximum edge length of 5 mm and an angle resolution of 6°. Although the TGF format is used in this tutorial and preferred because it guarantees that each component is represented by a watertight geometry, several other formats are also allowed. See the Geometry Import section in the Forte User's Guide for details. No matter which format is used, in all cases, the volume mesh will be automatically generated during the simulation. Note that once you have imported the geometry, there are a number of modifications to the Geometry items that you can apply to the current project, such as scale, rename, transform, invert normals, or delete geometry elements. Use the Refit   button to fit the entire geometry in the graphic window. If the provided TGF surface mesh is used, once imported, it is important to check and confirm that the surface mesh normals point away from the fluid domain. To check that, display the normals by right-clicking the surface in question. In this specific tutorial, the normal vectors of the triangulated surface mesh of the housing and ports already point towards the exterior of the fluid domain. However, the normal vectors of the 3 solids and moving components, the piston, crankshaft and connecting rod, should point inwards (away from the fluid region). Therefore, select the surfaces associated with these three components, right-click, apply Invert normals.

The Geometry node also allows setting new reference frames to facilitate the rest of the setup. The new reference frames created are listed in Table 10.2: New Reference Frame 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 10.2: Clip-plane view of the Geometry and Reference Frames.

Figure 10.2: Clip-plane view of the Geometry and Reference Frames

Automatic mesh generation in Forte requires you to specify a material point, a global mesh size that serves as the reference size for mesh refinement, and various refinement controls. In this tutorial we placed the Material Point 21 cm away from the origin in the positive z-direction, and let the Global Mesh Size be of 4 mm.

Next, we add adaptive and fixed refinement controls, as listed in Table 10.3: Mesh refinement controls.

In this section the main models parameters are discussed, but you should also refer to the Forte User's Guide for a more complete description of each panel.

Boundary conditions are set as follows:

Outlet: From the Boundary Conditions node, in the Editor panel, click the New Outlet   icon and create Outlet. Select the outlet item in the Location list. Set the Static Pressure = 0.95 bar and the Turbulence Boundary Conditions to Turbulent Kinetic Energy and Length Scale of 3,600 cm2/sec2 and 1.0 cm, respectively.

Inlet: From the Boundary Conditions node, in the Editor panel, click the New Inlet   icon and create an Inlet named Inlet. At the top of the Editor panel, select Create new gas mixture... for the Composition. Click the Add Species button and then select o2 (oxygen) and n2 (nitrogen) as the species. Specify Mass Fraction of 0.23 for o2 and 0.77 for n2. Name the composition air and click Save and then Close. Returning to the Editor panel, select inlet from the Location list. Select Total Pressure, Time Varying as the Inlet Option and Crank Angle as the Time Option. For the pressure profile, select Create new... and import the pressure profile using the Load CSV option. The name of the pressure profile is inletPressureProfile.csv. On the Load CSV dialog, retain the selected Read Column Titles option. The unit for Column 1 should be Angle and degrees and for Column 2 the units should be Pressure and bar. Name the profile inletPressureProfile and click Save and then Close. Enable the Repeat Profile Each Cycle Option. Define Turbulence using values for Turbulent Kinetic Energy and Length Scale of 3,600 cm2/sec2 and 1.0 cm, respectively. Set the Static Temperature = 298 K. Click Apply.

PistonMoving: This is one of the 3 moving components, and it will be using the built-in slider crank motion. From the Boundary Conditions node, go to the Editor panel and click the New Wall   icon and name it PistonMoving. Select the piston_external, piston_internal and piston_top items in the Location list. Set the Thermal Boundary Condition to Wall Temperature, Constant and 400 K. Turn ON the Wall Motion option and set the piston Motion Type to use a Slider Crank with a Stroke of 7.22 cm and a Connecting Rod Length of 11.95 cm with 0.0 Piston Offset. To set the axis for translation, under Direction, the Reference Frame is Global Origin and the Coordinate System is Cartesian. Set X = 0.0 cm, Y = 0.0 cm, Z = 1.0 cm. Change the Movement Type to Sliding Interface and select the liner and piston_external items from the list of surfaces. For this setting, the moving piston should be selected along with the surface it is sliding/moving past. Leave the other parameters at their defaults.

Pistonpin_conPin: This is moving following the same translation of the PistonMoving boundary condition. The only surface selected in the location list is the piston_pin. The only reason this boundary is treated as a separate one is to impose the Sliding Interface option between another pair of surfaces: con_rod_pin and piston_pin. Other than that, all the parameters are the same as those described for the PistonMoving boundary.

Crankshaft: This is the second moving component in this simulation, and it simply rotates around its center. Click the New Wall   icon, select the crank_perimeter, crank_shaft, crank_shaft_sides, and crank_sides items in the Location list, and impose a Wall Temperature of 300 K. Enable Wall Motion and choose Rotation as the type. Let it rotate at the origin of the global coordinate system around the x-direction (Axis Direction of (1.0, 0.0, 0.0)) with an angular velocity of 3167 RPM. At the bottom of the editor panel, add the Sliding Interface option, and select the pair of surfaces con_rod_crankpin and crank_shaft, to avoid any mesh distortions, any fluid cells in-between, and allow the two surfaces to literally slide one on top of the other.

ConRod: This is the remaining moving component in this simulation connected to both the moving piston and the crank shaft surfaces. Due to the combo motion to which it is subjected (translation in the vertical direction and rotation around the x-direction), we will use a UDF to describe its motion. Refer to the Simulation Controls node to see how the UDF is implemented and linked to this project file. Do NOT select any wall motions at this point. The motion will be imposed only via UDF. For now, treat this boundary as a simple wall. So click the New Wall   icon, select the con_rod_crankpin, con_rod_peripheri, con_rod_pin, con_rod_side, con_rod_side2 items in the Location list, then add a Wall Temperature of 350 K.

IntakePort: Click the New Wall   icon and name the new wall IntakePort. Select the inlet_port item in the Location list and turn ON the Heat Transfer option and set the Temperature to 298 K. Now reproduce the IntakePort with Copy   and Paste  , four times, to create four new boundaries as detailed in the following table.

The domain is initialized with the operating conditions, species concentrations, and temperatures. The Default Initialization species composition is at the expected exhaust composition, assuming complete combustion. The intake and exhaust must also be initialized to the boundary condition values. Set the initialization parameters as described in the following sections.

Default Initialization: Select Default Initialization in the Workflow tree. In the Editor panel, set the Initialization Order to 1. Select Create new gas mixture... for the Composition. This opens the Gas Mixture panel, where you select Add Species. Set a Mass Fraction of o2=0.1123911, n2=0.7421674, co2=0.0996009, and h2o=0.0458404, and Save this composition as exhaust_gas. On the Editor panel, set a Constant Temperature of 1,273 K and a Constant Pressure of 3 bar.

The Turbulence initialization uses the Constant option and the Turbulent Kinetic Energy and Length Scale option with values 3,600 cm2/sec2 and 1.0 cm, respectively. Accept the defaults for the remaining parameters and click Apply.

Now we will create 5 other initialization regions of type Other via the New Secondary Region From Material Point   option. Follow the instructions in Table 10.7: Initialization region settings.

On the Simulation Controls node, let the simulation be Crank Angle Based, going from 70° to 430° with 3167 RPM. Select 2-Stroke as the Cycle Type and leave everything else as default.

 

10.3.6.4. UDF Walkthrough

The provided fsi_UDF_conRod.cpp includes multiple commented lines and helper functions that will aid understanding the written code, while providing further examples of general useful operations to modify the UDF itself. Take the time to go through it.

In this section we are focusing on the connecting rod motion implemented in the fsi_UDF_conRod.cpp file, specifically from lines #496 to #582. The method: DLL_SO_VOID Forte_UDF_FSI_Get_Updated_Vertices is called once per boundary per UDF update cycle. The UDF instance should use this method to provide updated vertex locations (and optionally velocity) for the specified connecting rod. See Figure 10.3: Sketch of the piston-connecting rod-crank motion.

Figure 10.3: Sketch of the piston-connecting rod-crank motion

Figure 10.3: Sketch of the piston-connecting rod-crank motion shows a sketch of a piston-crank mechanism in which the piston translates in the z-direction and the crank rotates around the x-direction while being centered at the global origin on point O. The connecting rod moves with a combined motion. Point A, linking the connecting rod with the crank, simply rotates, whereas Point B simply translates. All the other connecting rod points in between A and B have both the translational and the rotational displacement components in the y-z plane.

Inside the DLL_SO_VOID Forte_UDF_FSI_Get_Updated_Vertices method we find:

• Line #499. Every time the UDF updates the connecting rod vertex locations, a message like this is printed out in the MONITOR file

  "Entering FSI UDF Vertex Update";

• Lines #504 to #515. The slider crank variables (that is, the crank radius and the connecting rod length) are specified.

• Lines #518 to #522. The crank angle θ is updated and employed to define the connecting rod angle ϕ as follows:

  rsin θ=L sin⁡ϕ

• Lines #524 to #531. These lines define auxiliary entities needed later in the implementation. They make use of the GLM open-source library that can be downloaded here: https://www.opengl.org/

• Lines #533 to #540. Here the connecting rod matrix, M_rod, is built as a sequence of translation, rotation, and again translation operations. Note that the order at which these operations are performed is significant and affects the final result.

• Lines #542 to #561. Finally, a for-loop around all the vertex belonging to the connecting rod is performed to update their position, p, via the operation on line #549: p=M_rod*p;

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

Spatially Resolved: Two different data formats are available: CGNS and DVS. In this tutorial we use CGNS. We set to output spatially resolved data every 20° crank angles and add then a few extra angles around the top dead center location, through the User Defined Crank Angle Outputs option. Variables of interest are selected.

Spatially Averaged and Spray: Opt for Crank Angle in the Spatially Averaged Output Control and set the interval to 1°, then choose the species of interest if any.

Restart Data: It is good practice to enable the restart data writing at the end of a simulation in case you want continue it later. You could also choose to have restart files written at a certain frequency or at specified times depending on your needs.

Monitor Probes: Two spherical probes are set to collect pressure, p, and temperature, T, values over time. The first one is labeled PT_inlet, and averages p and T over a sphere with a 1 mm radius placed inside the intake port, at (0.0, 7.0, 7.2) cm. The second one is named PT_Cylinder_point, and averages p and T over a sphere of 2 mm radius located inside the dome, at (0.0, 0.0, 21.0) cm.