This tutorial will cover all the set-up steps, but you should 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 generic_gerotor_tutorial.zip file here .

Unzip generic_gerotor_tutorial.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 Generic_Gerotor_Tutorial.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 your tutorial project's settings, and then to export the provided final version of the tutorial's settings. 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 4 complete revolutions, 120 ms. As a guideline for your own simulations, this tutorial is estimated to take approximately 15 hours on a Linux cluster using an Intel 2.6 GHz processor and 112 cores.

One of the main advantages of using Forte in your simulation is that you don't need to create your volume mesh beforehand, since it will be automatically generated on-the-fly. Instead, you only need to create a surface mesh and import it into Forte. For this tutorial Ansys provides the surface mesh in the .stl format exported from the CAD geometry in Ansys SpaceClaim, that you need to import in the Forte user interface. Go to the Geometry node and click Import Geometry , select the option Surface from one or more STL files, pick your file or the Generic_Gerotor_Surface_Geometry.stl and choose cm as the 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.

Before moving away from the geometry module, let us create a customized reference frame to use in setting up the rotation axis of the outer gear. Under Geometry > Reference Frames, click the New Reference Frame icon   and name it Center_OuterGear. Now, place its origin at X = -3.266 mm, Y = -0.2965 mm, Z = -41.7 mm, and accept the same orientation as the global origin.

To allow the mesh generation to proceed on-the-fly, you are required to set up the material point inside the fluid domain. For geometries with moving boundaries, like the one in this tutorial, you also must ensure that the material point will remain within the domain throughout the simulation. For this reason, we placed the material point next to the inlet boundary and away from any moving surfaces.

The coordinates of the Material Point are: X = -0.3 cm, Y = 8.5 cm, Z = -4.0 cm, with a Global Mesh Size of 2.5 mm with static refinements applied as indicated in Table 17.1: Mesh refinement settings. The Active property is set to Always for all the mesh controls.

Among the mesh controls there is an additional dynamic refinement named Gears of the type Gap Feature Control  , applied to the side of the gears facing each other: inner_gear_side and outer_gear_inside. 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 0.7 mm. This value should be slightly bigger than the local cell size before the gap refinement level of 1/8 is applied. So if the global mesh size is 2.5 mm and the local cell size is 1/4 of that (0.625 mm) the value of 0.7 mm is a valid estimate.

In the same editor panel, check the Enable Gap Model box to compensate for the under-resolution in the gap zones. A momentum sink term will be applied to account for the underpredicted wall shear stress and overpredicted 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 compressor, the best practice is to use the default value of 1.0. In this tutorial, we shrank the original inner gear CAD geometry to avoid potential surface intersection between the gears. Therefore, we set the Gears gap size scale factor to 0.3 and the *_bottomCase gap values to 0.5 to reduce flow leakage through those gaps in the simulation. When using simulation to guide gerotor design, this Gap Size Scale Factor also allows you to study the impact of gap size on simulation results without needing to modify the geometry itself.

See Table 17.1: Mesh refinement settings for a complete list of all the refinements.

The working fluid in this generic gerotor is oil, therefore navigate to the Models > Chemistry/Materials node, click the New Liquid and Vapor Pair icon   and add oil(l) and oil-vapor. Once you have selected your working fluid, you can either use the Forte library liquid properties or modify the database values. In this case, select User Defined Values for Liquid Properties, then select Override the Database Liquid Density, Viscosity, and Vapor Pressure with Constant Values. We set the Density to 882 kg/m3, the Viscosity to 2.047e-3 kg/m-sec, and the Vapor Pressure to 400 Pa. To make the working fluid more realistic, we have also added a small amount of air, therefore n2 and o2 are added as gaseous components.

Now, as shown in Figure 17.2: Liquid Properties panel, keep the default Ideal Gas and select the ZGB Finite-Rate Model method to model the Phase Change.

Figure 17.2: Liquid Properties panel

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:

Inlet: Defined as an inlet boundary  . To be able to consider liquids as part of the inlet flow, Create a new multiphase mixture as shown in Figure 17.3: Inlet flow composition, and allow the Liquid Phase Fraction to be 0.9999. Save the mixture. Then pick the inlet surface as the selected Location, set the Static Pressure to 1 atm, leave the Turbulent Kinetic Energy and Length Scale at their default values, and finally set the Static Temperature to 300 K.

Figure 17.3: Inlet flow composition

Outlet: Defined as an outlet boundary  . Pick the outlet surface as Location, set the Static Pressure to 5 atm and for the inlet boundary, leave the Turbulent Kinetic Energy and Length Scale at their default values.

Walls: Defined as a wall boundary  . Pick the bottom_case, exhaust, intake, side_case, and top_case as Location, apply the Law of the Wall as a Wall Slip Condition since turbulence is involved. Leave the rest of the editor panel at default values and disable the Heat Transfer check box (not of interest in this tutorial).

InnerGear: Defined as a wall boundary  . Pick the inner_gear_bottom, inner_gear_side, and inner_gear_top as Location, apply the Law of the Wall and disable the Heat Transfer check box, as for the previous walls. Now check the Wall Motion box and activate the Rotation option in the Motion Type drop-down menu. Use the Global Origin for the Axis Origin and the Z-Axis Direction with 2,000 RPM Angular Velocity. In the Movement Type, select the Moving Surface option.

Outer_Gear: Defined as a wall boundary  . Pick all the outer gear surfaces, outer_gear_bottom, outer_gear_inside, outer_gear_outside, and outer_gear_top as Location. Apply the Law of the Wall and disable the Heat Transfer check box, as for the previous walls. Now check the Wall Motion box and activate the Rotation option in the Motion Type drop-down menu. This time use the Axis Origin of the Center_OuterGear reference frame, and its Z-Axis Direction with 1,800 RPM Angular Velocity. In the Movement Type, select the Sliding Interface option. This option will allow the outer gear side to slide past the casing side. Therefore, in the Select Stationary and Sliding Surfaces, chose the following pair: side_case/outer_gear_outside.

In the Initial Conditions under Default Initialization, use the same settings as the inlet oil composition in Figure 17.3: Inlet flow composition. Set the Temperature to 300K, the Pressure to 1atm, the Turbulent Kinetic Energy and Length Scale to their default values.

Let the simulation to be Time Based and enter the Max. Simulation Time of 120 msec (4 revolutions). Leave everything else as default.

In the Time Step editor panel, set the Initial Simulation Time Step to be 1e-7 sec, and the Max. Simulation Time Step to be 5e-6 sec. Then, in the Advanced Time Step Control Options set the Fluid AccelerationFactor to be 0.5 and the Rate of Strain Factor to be 0.6.

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: Select Time in the Spatially Averaged Output Control and set the interval to 1e-6 sec, then choose the species of interest, if any. In this case, the Time Averaging Output is also enabled with the Specify Starting Time option set to 30 msec, to calculate the running time-averaged outputs at open and rotating boundaries. For a more meaningful average, the first revolution is discarded, and the averaging starts from 30 ms.

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.

Monitor Probes: Two pressure probes are created for this tutorial with an Output frequency of 1e-6s.