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 h2_engine.zip file here .

Unzip h2_engine.zip to your working folder.

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

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.

The installation includes the cgns_util export command, which you can use to compare the parameter settings in the project file generated at any point during your tutorial set-up against the provided .ftsim, which has the parameter settings for the final, completed tutorial. This command is described in the Forte User's Guide.

Briefly, you can double-check project settings by saving your project and then running the cgns_util to export your tutorial project, and then to export the provided final version of the tutorial. Save both versions and 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 one full cycle. As a guideline for your own simulations, this tutorial is estimated to take roughly 22 hours on a Linux cluster using Intel 2.6 GHz processor and 160 cores.

One of the main advantages of using Forte in your simulation is that you don’t need to create the volume mesh beforehand, since it will be automatically generated on-the-fly. Instead, you only need to create a surface mesh and import it in Forte. For this tutorial we provide the surface mesh in the .stl format exported from the CAD geometry in Ansys Discovery, that you need to import in the Forte UI. Go to the Geometry node and click on Import Geometry  , select the Surface from one or more STL files option, pick your file or the LT_wInj_Tutorial.stl and choose cm as units. Note that once you have imported the geometry, there are a number of actions that you can perform to modify the geometry elements, such as scale, rename, transform, invert normals, or delete. It is important at this stage that the imported engine geometry has the piston at its top dead center independently from the initial crank angle of the simulation. This facilitates the stretching of the mesh and allows the piston to slide all the way down to the bottom dead center.

Create now 3 new Reference Frames for an easier setup later on in the workflow tree. See Table 8.1: Reference Frames in cartesian coordinates for further details on their cartesian coordinates.

Once you have imported the geometry, go to the Sub-volume node, create a New Sub-Volume and label it chamber. The selected surfaces bounding the new sub-volume are crevice_bottom, crevice_side, head, liner and piston. Chose the sub-volume material point to be at X = 0 cm, Y = 0.5 cm, Z = 0 cm in cartesian coordinates, and select the Multiple passes as the Capping Method.

It is always useful to create a Clip Plane to double check that the material point lays within the watertight geometry. Create one centered at the origin with -z as the plane normal.

To allow the mesh generation on-the-fly, you are required to setup the material point inside the fluid domain. For geometries with moving boundaries, like the one in this tutorial, you also want to make sure the material point will remain within the domain throughout the simulation. For this reason, we placed the material point between the injector and the piston at its top dead center.

The coordinates of the Material Point are: X = 0 cm, Y = 0.5 cm, Z = 0 cm, and we chose a Global Mesh Size of 2 mm with static refinements applied as indicated in Table 8.2: Mesh refinements settings.

Among the Mesh controls there is an additional dynamic refinement type, the Gap Feature Control  , applied to the crevice_side and liner. This type of refinement is of key importance when small gaps are present. In its editor panel setting, you are asked to indicate a Surface Proximity that will identify the gap between the pair of surfaces selected in the Location box. For this tutorial we set the Surface Proximity to be 12 mm and the refinement level for those cells within the gap to ½ of the global mesh size.

Starting from 2024 R1, it is possible to modify the angular deviation between faces forming a gap. A value of zero indicates the faces bounding a gap must be parallel, a higher value is more permissive and will detect more gap cells. For this tutorial we kept the default value. In the same editor panel check the Enable Gap Model box to compensate for the under-resolution in the gap zones. In other words, setting the refinement level to ½ of the global mesh size, indicated that the fluid cells sizes within the gap are of 1 mm which means that some of the gaps only contain a fraction of a Cartesian cell cut by the physical boundary. Therefore, by enabling the Gap Model a momentum sink term is applied, which accounts for the underpredicted wall shear stress and over-predicted mass flow rate on the coarse grid. The Gap Model takes both the gap size and the local fluid cell size as inputs, and therefore the flow solution is not expected to be very sensitive to the gap refinement level.

The last parameter to set in the Gap Feature Control editor panel is the Gap Size Scale Factor. It can be used to enlarge or shrink the gap sizes measured on the geometry. The scaled gap size is then used as the input for the gap model in each local CFD cell in the gap zone. If the gap size in the geometry accurately reflects the size in the actual gap, the best practice is to use the default value of 1.0. In this tutorial, we use the default value.

A reduced version of the Ansys MFL hydrogen mechanism has been used for this case. The hydrogen mechanism Hydrogen_MFL2021.cks can be found in the MFL Skeletal mechanism folder. MFL mechanism folders can be found in InstallDirectory\reaction\data\ModelFuelLibrary (where InstallDirectory on Windows is typically C:\Program Files\ANSYS Inc\version). Starting from that mechanism, for this non-reacting case all species and their associated reactions were removed except for nitrogen (n2) and hydrogen (h2).

This tutorial uses the RANS RNG k-epsilon turbulence model, which is the default turbulence model option. Other turbulence modeling options are available under Models > Transport > Turbulence.

Boundary conditions must be specified for each of the surfaces found in the Geometry node. To match the provided project, follow these instructions for each boundary condition:

In the Initial Composition under Default Initialization is created with the IVC calculator utility. It imposes a mass fraction of N2 = 0.99936 and H2 = 6.39e-4. The Temperature is set to 309.15 K, the Pressure to 1 atm, the Turbulent Kinetic Energy and Length Scale to their default values. Set the initialization order to 3.

In addition to the Default initialization, there are other 3 Secondary Regions Initializations of type Other, identified by a material point. Those are reported in Table 8.3: Secondary Regions Initializations

Let the simulation to be Crank Angle Based and set it to run from -360 to 360 crank angle degrees. The RPM is 1500, and the Cycle Type is 4-Stroke. Everything else is as default.

In the Time Step editor panel, have the Initial Simulation Time Step to be 5e-7 sec, and the Max. Simulation Time Step to be 5e-6 sec.

In the Chemistry Solver editor panel, turn off chemistry by setting Activate Chemistry to Always Off.

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

Spatially Averaged and Spray: Opt for Crank Angle in the Spatially Averaged Output Control and set the interval to 0.5 degrees, 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.

Additional Output: Starting with Ansys Forte 2022 R1, alongside the standard spatially resolved outputs (.ftres format), Forte offers the possibility to have an additional or an alternative set of output format, namely EnSight DVS (Dynamic Visualization Store). The DVS format helps reduce the loading time and the stepping through transient solution points in Ansys EnSight, thanks to the smaller size of the files generated. Better performance is also expected during the solution writing, especially when running a job on a cluster with many processors. To utilize the EnSight DVS format, start by clicking the EnSight icon on the Additional Output editor panel. Then check the Enabled box under EnSight DVS Settings. The output settings follow the same structure as Forte's native spatially resolved outputs. In other words, select your Interval Based Output Control frequency and pick your Solution Variables of interest. Only those in this list will be found in EnSight, so it is always suggested to have amongst this at least Pressure and Velocity Magnitude. If you scroll down in the same EnSight DVS editor panel you can also add the Spatially Averaged Datasets in the same additional output files set.

The DVS results will be contained in a subfolder of the run directory, named according to the user-supplied name of the DVS output added to the Workflow tree. To load the results in EnSight, within an EnSight session, choose File > Open and select the .dvs file from this directory or use the EnSight launcher shortcut on Forte's Run panel, which will search for and provide a list of available .dvs files in the analysis directory that can be preselected and passed to the newly launched EnSight instance.