This tutorial will cover all the setup 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 scroll_compressor.zip file here .

Unzip scroll_compressor.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 from scratch. 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 five complete revolutions. As a guideline for your own simulations, this tutorial is estimated to take approximately 9 hours on a Linux cluster using an Intel 2.6 GHz processor and 168 cores.

This simulation uses Forte's on-the-fly automatic mesh generation (AMG) feature, which only requires the bounding surface geometry as an input and does not involve volume mesh generation ahead of the calculation. The surface geometry to be imported into Forte is in Fluent Meshing faceted geometry (.tgf) format, which was exported from the solid geometry created in SpaceClaim. Although the TGF format is used in this tutorial, several other formats are also allowed. See the Geometry Import section in the Forte User's Guide for details.

Since the scroll and casing geometries involve curved surfaces in 3-D and there are tiny gaps between the side surfaces of scroll and casing, the curved surfaces are required to be sufficiently smooth in order to avoid surface intersection during the rotation. When exporting the TGF file from SpaceClaim, we recommend that you choose the Fine option for the Facet Resolution of the TGF file. The Angle resolution should not be much larger than 4°.

Now let us import the surface geometry into the Forte Simulate user interface. Open the Geometry panel, click the Import Geometry   icon, select Surfaces from TGF file as the import option, and select the provided TGF file, Scroll_Compressor_Surface_Geometry.tgf. Ensure that the Invert Normals box is checked and accept all other default options on the Import Options wizard window.

The fluid domain in this case is formed by two watertight surface groups, which are the bounding surfaces of the two solids in SpaceClaim. The first group consists of “inlet”, “outlet”, “intake-port”, “discharge-port”, “static-scroll-end”, and “static-scroll-side”; the second group includes the two surfaces that form the orbiting scroll: “orbiting-scroll-end” and “orbiting-scroll-side”. Forte requires that the end surfaces of the orbiting scrolls be put inside the casing and away from the casing’s end surfaces by a tiny tolerance. In the provided geometry file, this tiny tolerance is 1 µm. By default, the gap between the orbiting scroll end surface and the casing end surface will not be meshed in the volume mesh. However, if the end gap sizes are physically large enough and it is desirable to model the flow leakage through them, we can force these gaps to be meshed by using the gap refinement controls that will be discussed later in Automatic Mesh Generation Setup.

In Forte, the normal vectors of the triangulated surface mesh are required to point towards the exterior of the fluid domain. In the .tgf file, the normal vectors point to the interior of the two watertight surface groups. When the .tgf geometry is imported, all the normal vectors are inverted. As a result, the surface normals of the orbiting scroll surfaces should be inverted again such that they point to the exterior of the fluid domain. To do so, multi-select (hold Ctrl and click) surfaces “orbiting-scroll-end” and “orbiting-scroll-side” on the Geometry node of the Workflow tree, and on the right-click menu, choose Invert Normals. You can double-check the normals of a surface by turning on Normals using the right-click menu.

Forte's automatic mesh generation requires you to specify a material point, a global mesh size that serves as the reference size for mesh refinement, and various refinement controls.

Material Point: The Material Point   should always lie inside the fluid domain throughout the simulation and should be located at least one unit cell length away from any boundaries. In this tutorial case, we choose to put the material point inside the discharge port: X = 0.0 cm, Y = 13.5 cm, Z = 30.0 cm.

Global Mesh Size: Set the Global Mesh Size to 0.2 cm.

Three types of refinement controls are used in this tutorial: Surface Refinement Depth  , SAM (Solution Adaptive Mesh)  , and Gap Feature Control  . Detailed mesh control parameters are listed in Table 15.2: Settings for Mesh Control refinements. The Active property is set to Always for all the mesh controls. For the Gap Feature Control, the Surface Proximity is set to 0.15 cm, and Enable Gap Model is turned ON.

The Gap Feature Control   is a mesh refinement control that is especially useful for handling the small gaps in compressors. This 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.

Forte does not require the gap zones to be finely resolved using tiny CFD cells. In this tutorial, the Cartesian cell size in the gap zone is 0.05 cm, which means that some of the gaps only contain a fraction of a Cartesian cell cut by the physical boundary. To compensate for the under-resolution in the gap zones, the Gap Model is used to apply a momentum sink term, 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 Gap Size Scale Factor 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 sample scroll compressor case, the smallest gap size is about two times of that in the actual compressor, therefore the gap size scale factor is set to 0.5 to reduce flow leakage through gaps in the simulation. When using simulation to guide compressor design, this gap size scale factor also allows you to study the impact of gap size on simulation results without the need of modifying the geometry itself.

As mentioned earlier, there is a 1 µm distance tolerance between the end surface of the orbiting scroll and the end surface of the casing (the surface is called “static-scroll-end”) on both ends. Forte will ignore this tiny gap by default. However, if the end gaps are large enough and it is of interest to model the flow leakage through them, you can use the Gap Feature Control   to mesh these gaps.

In Forte, a chemistry set in Chemkin format is used to define the properties of the working fluid. This scroll compressor is for refrigeration applications. The working fluid is R-410A, which is a mixture of R32 and R125. It will be modeled using the real gas model. Ansys Forte supplies a chemistry set for various refrigerants, called Refrigerants.cks, which is stored in the data folder of your Forte installation. To import this chemistry set, go to the Workflow tree and under Models > Chemistry/Materials, click New Import Chemistry   and select Refrigerants.cks in the data folder of the Forte installation. This chemistry set contains R32 and R125 as species. To create the R-410A mixture, click the Mixture   icon on the menu bar, select the Create new... option under gas_mixtures, and click the Pencil  icon. In the pop-up Mixture Editor window, click Add Species to add R32 and R125 and set both of their Mole Fractions to 0.5. To turn on the real gas model option, choose Real Gas as the Equation of State option on the Models > Chemistry/Materials panel.

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

Use the icons on the Boundary Conditions panel to add new boundary conditions. The boundary conditions used in this project are explained below:

Inlet: Defined as an inlet boundary  . For Composition on the inlet setup panel, select the R-410A mixture created earlier. Select surface inlet as the Location. Choose the Total Pressure option for Inlet type and set the pressure to 9.978 bar. Keep the default turbulence parameters for the inflow. Choose Total Temperature as the Temperature Option and set the temperature to 293 K.

Discharge: The discharge outlet should be defined as an inlet boundary   as well because we need the reverse flow condition to be explicitly defined. For Composition, select the same R-410A mixture. Select surface outlet as the Location. Choose the Total Pressure option for Inlet type and set the pressure to 33.853 bar. Keep the default turbulence parameters for the inflow. Choose Total Temperature as the Temperature Option and set the temperature to 373 K.

Static-walls: Defined as a wall boundary  . This boundary condition includes all static walls in this sample, but you can choose to split it into multiple wall boundaries if needed. Select surface intake_port, discharge_port, static_scroll_end, and static_scroll_side as the Location. Turn ON Heat Transfer and set Wall Temperature to 333.0 K.

Orbiting-scroll-wall: Defined as a wall boundary  . Select surfaces orbiting-scroll-end and orbiting-scroll-side as the Location. Turn off Heat Transfer to model this wall as adiabatic. Turn on Wall Motion and set Motion Type as Planetary Motion. Both the primary axis and secondary axis require an Origin and a Direction vector as the inputs. To facilitate the setup, let us create two reference frames for these two axes. Go to Geometry > Reference Frames, click the New Reference Frame  icon to create two new reference frames: primary-shaft and secondary-shaft. For reference frame primary-shaft, set the New Origin to (X = 0.0 cm, Y = 13.65 cm, Z = 25.0 cm); for reference frame secondary-shaft, set the New Origin to (X = 0.785 cm, Y = 13.65 cm, Z = 25.0 cm). Now go back to this boundary condition panel. By using the two reference frames for the Primary and Secondary Axes, the Origin and Direction of these two axes are simply the origin (X = 0.0 cm, Y = 0.0 cm, Z = 0.0 cm) and Z-axis (X = 0.0, Y = 0.0, Z = 1.0) of the corresponding reference frames. See the fully configured Forte project for details. To create an orbiting motion, the angular velocities of the primary rotation and secondary rotation should have the same magnitude but opposite direction. Therefore, set Primary Angular Velocity to 3000 RPM and set Secondary Angular Velocity to -3000 RPM. Note that the rotation direction follows the right-hand rule.

For Composition, select the mixture R-410A created earlier . Set Temperature to 350 K and Pressure to 9.975 bar. It is not critical to have well guessed initial conditions because the initial mixture can be quickly flushed out and overridden by steady operation conditions after 2 to 3 revolutions.

Simulation Limits: Choose the Time Based option to specify the Simulation End Point and set Max. Simulation Time to 0.1 s. This duration covers five complete revolutions for the primary shaft. (Time for each resolution can be calculated as 60/RPM s).

Time Step: Forte uses adaptive time step controls to adjust the actual time step size for each transient flow integration step. The user-specified max time step will be used if the time step is not subject to other constraints listed under Advanced Time Step Control Options. For rotating machinery simulation, the rule of thumb for choosing the Maximum Simulation Time Step is to have at least 10 time steps per degree of rotation of the fastest rotating motion in the system. Using this guideline, the Max Time Step can be estimated as 60/(RPM*360*10) = 1/(RPM*60) s, which gives 5.56E-6 s for RPM = 3000. In this tutorial, the Max Time Step is set to 5.0E-6 s. For the Advanced Time Step Control Options, typically it is acceptable to relax the Fluid Acceleration Factor and Rate of Strain Factor to achieve larger time steps without affecting the accuracy and stability very much. In this calculation, these two factors are set to 1.0 and 1.2, respectively. Both are two times their default values. It is risky to change the other control factors because relaxing them may cause the solution to become unstable.

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

Spatially Resolved: Use Time for the Output Timing Control option. Set Interval Based Output Control to output every 0.01 s, which corresponds to a half revolution. Turn on User Defined Output Controls and create a time list to save spatially resolved solutions at locations of interest. In the fully configured .ftsim file, the solutions are saved for every 5.56E-4 s (corresponding to 10 degrees of rotation) for the third revolution. For the Spatially Resolved Species list, select R32 and R125. For the Solution Variables list, select variables of interest. The minimum variable set should include Pressure, Temperature, VelocityX, VelocityY, VelocityZ, and Velocity Magnitude.

Spatially Averaged And Spray: Choose the Time option and set the output interval to 1.0E-5 s. Select species R32 and R125 for output.

Restart Data: Make sure Write Restart File at Last Simulation Step is checked ON. This option allows a restart file to be saved at the end of the current simulation. 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. This practice may help save CPU time spent in simulating the initial transient process. Turn ON Interval Based Restart and set the Time Steps between Restart Writing to 500. This type of restart file can help provide a recovery point if a long-running job was unexpectedly interrupted.

Monitor Probes: On the Monitor Probes setup panel, for the Inquiry Frequency, choose Time as the Frequency Option and set the interval to 1.0E-5 s. Click the New Probe icon   to add new monitor probes. In this tutorial, we will add three Geometric-based probes at different locations and one Boundary-Condition-based probe using the Discharge boundary.

The spatially averaged solutions are reported in CSV format in the Run folder (Nominal). Ansys Forte Monitor   is a convenient tool for displaying these averaged solutions. Launch Forte Monitor and open the .analysis directory of the Forte project to load the CSV files. Several line plot examples are shown in Figure 15.2: Line plots created in Forte Monitor. The parameters plotted include mass flow rate at the Inlet (open_boundary_flow.csv) and power of the orbiting scroll applied on the fluid (planetary_boundary_parameters.csv). In this example, the curves show that the simulation has largely reached a steady operation starting from the third revolution. The cyclic pattern started to repeat for each revolution thereafter.

Figure 15.2: Line plots created in Forte Monitor

Ansys EnSight is the preferred tool for visualizing the spatially resolved solutions. Launch EnSight and open the .ftind file to load the solutions. The .ftind file is a solution index file, which contains the records pointing to a group of .ftres files. The actual solution data are contained in the .ftres files. If you need to control which .ftres solution(s) to load in EnSight, you can truncate or concatenate the records contained in the .ftind files in a text editor. Refer to the Forte User's Guide for details.

It is worth noting that the end gaps between the orbiting end surfaces (surface “orbiting-scroll-end”) and the casing end surfaces (surface “static-scroll-end”) are not meshed using fluid cells in the current setup. Although these end surfaces are part of the surface solutions, solution variables are not properly defined or extrapolated on them, therefore, they should not be used in visualizing the solutions in EnSight. These surfaces are highlighted in Figure 15.3: Post-processing simulation results using EnSight. To show the solutions at these boundaries, you can create two clip planes (whose parent part is VolumeCells) instead. Figure 15.3: Post-processing simulation results using EnSight shows two clip planes created at Z = 27.7 cm and Z = 22.81 cm, respectively.

On the EnSight Part tree shown in Figure 15.3: Post-processing simulation results using EnSight, the Part VolumeCells is the one that contains the 3-D volume solutions. It can be used for creating clip-planes, iso-surfaces, particle traces, etc. Figure 15.4: Sample Forte simulation results on clip planes in EnSight shows pressure and velocity plotted on clip planes. In this example, the top two are XY clip planes (using VolumeCells as the parent) at Z = 26.5 cm, in which the mesh lines are shown as well; the bottom two are YZ clip planes at X = 0.0 cm.

Figure 15.3: Post-processing simulation results using EnSight

Figure 15.4: Sample Forte simulation results on clip planes in EnSight