ACU-T: 3400 AcuSolve-Flux Integration

This tutorial provides instructions for setting up, solving, and viewing results for simulation of a 2D cable for simple conduction analysis. In this simulation, the heated solid volume is used for conduction with the outer volume and comes with a flux value already calculated using another software. This tutorial is designed to introduce you to a new feature, the Electromagnetics Manager, wherein the flux is imported on to the heated volume in the form of a Nastran file.

The basic steps in any CFD simulation are shown in ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The following additional capabilities of AcuSolve are introduced in this tutorial:
  • Importing the heat flux using the Electromagnetics Manger in AcuConsole
  • Mesh extrusion from one surface to other surface
  • Use of the Variable Manager for defining all the variables in a single panel
  • Post-processing with AcuFieldView for plotting temperature contours
  • Creating or modifying 2D Plots in AcuFieldView

In this tutorial, you will do the following:

  • Analyze the problem
  • Start AcuConsole and create a simulation database
  • Set general problem parameters
  • Set solution strategy parameters
  • Assign material properties for the solid volume
  • Import the geometry for the simulation
  • Create a volume group and apply volume parameters
  • Create surface groups and apply surface parameters
  • Set global and local meshing parameters
  • Generate the mesh
  • Set the appropriate boundary conditions
  • Import Nastran file using the Electromagnetics Manager for importing Flux
  • Run AcuSolve
  • Monitor the solution with AcuFieldView

Prerequisites

You should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

Prior to running through this tutorial, copy AcuConsole_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract 2DCable.x_t and CABLE_EXAMPLE_MOD.nas from AcuConsole_tutorial_inputs.zip.

Analyze the Problem

An important step in any CFD simulation is to examine the engineering problem at hand and determine the important parameters that need to be provided to AcuSolve. Parameters can be based on geometrical elements, such as inlets, outlets, or walls, and on flow conditions, such as fluid properties, velocity, or whether the flow should be modeled as turbulent or as laminar.

Figure 1 shows a simple 2D cable problem wherein the inner cylinder is provided with a volumetric heat source of 1.46686 W and is in contact with the outer cylinder, the outer surface of which is maintained at a temperature of 20oC (293K).This problem forms the basis of a simple conduction analysis between two concentric cylinders. The only difference from the basic problem is that the heat source is calculated using another software called Flux and is provided using AcuConsole’s EMag (Electromagnetic) Manger to account for volumetric losses from Flux to AcuSolve.



Figure 1.
Flux is used to simulate electromagnetic components to determine static thermal loading. The calculated thermal load value is then provided to AcuSolve to define the volumetric heat load on the solid volume. AcuSolve can then be used to determine the behavior of the fluid surrounding the solid components like:
  • Fluid rotational effects
  • Material specific properties (temperature dependent, non-Newtonian)
  • Convection on the outer surface

Coupling of AcuSolve to Flux will also enable the inclusion of natural convection and forced convection effects into the thermal calculation of various electrical devices.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In this tutorial, you will begin by creating a database, populating the geometry-independent settings, loading the geometry, creating volume and surface groups, setting group parameters, adding geometry components to groups, and assigning mesh controls and boundary conditions to the groups. Next you will generate a mesh and run AcuSolve to solve for the number of time steps specified. Finally, you will visualize some characteristics of the results using AcuFieldView.

In the next steps you will start AcuConsole, and create the database for storage of the simulation settings.

  1. Start AcuConsole from the Windows Start menu by clicking Start > All Programs > Altair <version> > AcuConsole.
  2. Click the File menu, then click New to open the New data base dialog.
    Note: You can also open the New data base dialog by clicking on the toolbar.
  3. Browse to the location that you would like to use as your working directory.
    This directory is where all files related to the simulation will be stored. The AcuConsole database file (.acs) is stored in this directory. Once the mesh and solution are created, additional files and directories will be created within this directory.
  4. Create a new directory in this location. Name it Flux_Coupling and open it.
  5. Enter Cable as the file name for the database.
  6. Click Save to create the database.

Set General Simulation Parameters

In next steps you will set parameters that apply globally to the simulation. To make this simple, the basic settings applicable for any simulation can be filtered using the BAS filter in the Data Tree Manager. This filter enables display of only a small subset of the available items in the Data Tree and makes navigation of the entries easier.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.


    Figure 2.
  2. Double-click the Global Data Tree item to expand it.
    Tip: You can also expand a tree item by clicking next to the item name.


    Figure 3.
  3. Double-click Problem Description to open the Problem Description detail panel.
    Note: You may need to widen the detail panel from the default size by dragging the right edge of the panel frame.
  4. Enter Flux Sequential Cosimulation as the Title.
  5. Enter Cable Example as the Sub title.
  6. Set the Analysis type to Steady State.
  7. Set the Temperature equation to Advective Diffusive.
  8. Set Abs. temperature offset to 0 K.


    Figure 4.

Set Solution Strategy Parameters

In the next steps you will set parameters that control the behavior of AcuSolve as it progresses during the solution.

  1. Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
  2. Check that Analysis type is set to Steady State.
  3. Set the Max time steps to 100.
  4. Set the Flow flag to Off.


    Figure 5.

Set Material Model Parameters

AcuConsole has three pre-defined materials: Air, Aluminum, and Water, with standard parameters defined. In the next steps, you will create a new solid material type called Insulation to match the desired properties for this problem.
  1. Double-click Material Model in the Data Tree to expand it.


    Figure 6.
  2. Right-click on Material Model and select New from the context menu.
    A new entry, Material Model 1, will be created in the Data Tree under the Material Model branch.
  3. Rename Material Model 1 to Insulation.
  4. Double-click on Insulation to open the detail panel.
  5. Change the Material type to Solid.
  6. Set the material properties for Insulation as follows by navigating through the respective tabs in the detail panel:
    1. Density: 2702.0 kg/m3
    2. Specific Heat: 908.0 J/kg-K
    3. Conductivity: 0.8 W/m-K
  7. Save the database to create a backup of your settings. This can be achieved with any of the following methods.
    • Click the File menu, then click Save.
    • Click on the toolbar.
    • Click Ctrl+S.
    Note: Changes made in AcuConsole are saved into the database file (.acs) as they are made. A save operation copies the database to a backup file, which can be used to reload the database from that saved state in the event that you do not want to commit future changes.

Import the Geometry and Define the Model

Import the Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of 2DCable.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.
  1. Click File > Import.
  2. Browse to the directory containing 2DCable.x_t.
  3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
  4. Select 2DCable.x_t and click Open to open the Import Geometry dialog.


    Figure 7.

    For this tutorial, the default values for the Import Geometry dialog are used to load the geometry. If you have previously used AcuConsole, be sure that any settings that you might have altered are manually changed to match the default values shown in the figure. With the default settings, volumes from the CAD model are added to a default volume group. Surfaces from the CAD model are added to a default surface group. You will work with groups later in this tutorial to create new groups, set flow parameters, add geometric components, and set meshing parameters.

  5. Click Ok to complete the geometry import.
  6. Rotate the visualization to view the entire model.


    Figure 8.

    The color of objects shown in the modeling window in this tutorial and those displayed on your screen may differ. The default color scheme in AcuConsole is "random," in which colors are randomly assigned to groups as they are created. In addition, this tutorial was developed on Windows. If you are running this tutorial on a different operating system, you may notice a slight difference between the images displayed on your screen and the images shown in the tutorial.

Apply Volume Parameters

Volume groups are containers used for storing information about a volume region. This information includes the list of geometric volumes associated with the container, as well as attributes such as material models and mesh size information.

When the geometry was imported into AcuConsole, all volumes were placed into the "default" volume container.

In the next steps you will create volume groups for each volume in the model, assign volumes to the respective volume groups, rename the default volume group container, and set the materials and other properties for each volume group.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
  2. Expand the Model Data Tree item.
  3. Turn off the display of surfaces by right-clicking on Surfaces and clicking Display off in the context menu.
  4. Expand Volumes. Toggle the display of the default volume container by clicking and next to the volume name.
    Note: You may not see any change when toggling the display if Surfaces are being displayed, as surfaces and volumes may overlap.
  5. Right-click on Volumes and select New.
  6. Rename Volume1 to Solid.
  7. Rename the default volume group to SolidHeated.
  8. Assign the respective volumes to their volume groups.
    1. Right-click on Solid and click Add to.
    2. Select the volume shown in the figure below and click Done.


      Figure 9.
  9. When the geometry was loaded into AcuConsole, the complete geometry volume was placed in the default volume group. This default volume group was renamed to SolidHeated. In the previous step, you assigned a volume to the other volume group that you created. At this point, all that is left is the SolidHeated volume group


    Figure 10.

Create Surface Groups and Apply Surface Parameters

Surface groups are containers used for storing information about a surface, including solution and meshing parameters, and the corresponding surface in the geometry that the parameters will apply to.

In the next steps you will define surface groups, assign the appropriate settings for the different characteristics of the problem, and add surfaces to the group containers.

  1. Turn-off the display of Volumes by right-clicking on Volumes and selecting Display off .
  2. Expand Surfaces in the Data Tree and toggle on the display of the default surface container.
  3. Right-click on Surfaces and select Surface Manager.
  4. In the Surface Manager Dialog, click New six times to create six new surface groups.
  5. If you cannot see the Simple BC Active and Simple BC Type columns, click on Columns and select these two columns from the list then click Ok.
  6. Turn off the display for all the surfaces except for the default surface and rename to default surface to OuterWall.
  7. Rename the other surfaces and set the Simple BC Active and Simple BC Type columns as per the table shown below.


    Figure 11.
  8. Assign the surfaces to their respective surface groups.
    1. Click Add to in the row belonging to +ZInner.
    2. Select the planar surface shown in the figure below and click Done.


      Figure 12.
    3. Click Add to in the row belonging to +ZOuter.
    4. Select the planar surface shown in the figure below and click Done.


      Figure 13.
    5. Rotate the model to the opposite side.
    6. In a similar manner, select the -ZInner and -ZOuter surfaces.


      Figure 14.


      Figure 15.
    7. Assign the surface for InterfaceOuter.


      Figure 16.
    8. Assign the surface for InterfaceInner


      Figure 17.
    9. When the geometry was loaded into AcuConsole, all the geometry surfaces were placed in the default surface group container. This default surface group was renamed to OuterWall. In the previous steps, you assigned some surfaces to various other surface groups that you created. At this point, all that is left is the OuterWall surface group.


      Figure 18.
  9. Close the Surface Manager Dialog.

Assign Volume Parameters (Element Material Properties)

In this step you will set element material properties for the volume groups that apply globally to the simulation.
Note: You need to switch to BAS in the Data Tree Manager.

Solid

  1. Expand the Solid volume group in the Data Tree.
  2. Double-click Element Set under Solid to open the Element Set detail panel.
  3. Change the Medium to Solid.
  4. Change the Material model to Insulation.
  5. Leave the remaining parameters as it is.


    Figure 19.

SolidHeated

The SolidHeated group will have the same settings as Solid group. In order to not to repeat the step again, we can propagate the settings to that group as follows:

  1. Expand the Solid volume group in the tree. Right click Element Set under Solid and select Propagate.
  2. Select the SolidHeated volume group from the pop-up window and click Propagate.
    Note: You can ensure the settings are applied correctly by expanding the SolidHeated group and cross checking the element set conditions.

Assign Surface Parameters (Boundary Conditions)

In next steps, you will set boundary conditions for the surfaces that apply globally to the simulation. To make this simple, the boundary conditions applicable for any simulation can be filtered using the BC filter in the Data Tree Manager.

OuterWall

The OuterWall group defines the wall through which conduction takes place.

  1. Expand the OuterWall surface group in the Data Tree.
  2. Double click Simple Boundary Condition to open the Simple Boundary Condition detail panel
  3. Ensure that the Type is set to Wall.
  4. Change Temperature BC type to Value.
  5. Set Temperature to 293.0 K.


    Figure 20.

Remaining Groups

  1. Expand the +Zinner surface group in the Data Tree.
  2. Deactivate Simple Boundary Condition for this surface.

    All the remaining groups will have the same settings as +ZInner. In order to not to repeat steps, we can propagate the settings.

  3. Right click Simple Boundary Condition under +ZInner and select Propagate.
  4. Select all the other groups except OuterWall in the pop-up window and click Propagate.


    Figure 21.
    Note: You can ensure the settings are applied correctly by expanding the other surface group and cross checking the boundary conditions.

Define the Variables List

  1. Click the Variable List icon from the main toolbar.
    Figure 22.
    Tip: You can also click Edit > Variable List.
    The Variable Manager dialog opens.
  2. Click Add six times.
  3. Create six variables using the Name and Expression data shown below then click Close.


    Figure 23.
    Note: Type equal (=) or colon equal (:=) in the Expression column before entering an expression. The expression will be valid only if either of these two symbols are used. Equal to (=) calculates the value of the expression when defined and uses it, whereas colon equal (:=) recalculates the value of the expression if any relative variable is changed.

    The variables L, r, V, Q denote length of the cylinder, radius, area of the cylindrical surface, and heat flux respectively.

Assign Mesh Controls

Set Global Mesh Attributes

Now that the flow characteristics have been set for the whole problem, a sufficiently refined mesh has to be generated.

Global mesh attributes are the meshing parameters applied to the model as a whole without reference to a specific geometric volume, surface, edge, or point. Local mesh attributes are used to create mesh generation controls for specific geometry components of the model.

In the next steps you will set the global mesh attributes.

  1. Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
  2. Expand the Global Data Tree item.
  3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
  4. Change the Mesh size type to Absolute.
  5. Enter :=dr for the Absolute mesh size.
  6. Change the Mesh growth rate to 1.2.


    Figure 24.

Set Volume Mesh Attributes

Volume mesh attributes are the meshing parameters applied to a particular volume. You have the option to control the mesh size on a volume and define curvature refinement parameters like curvature angle and the curvature mesh size factor.

In the next steps you will set the volume mesh attributes.

  1. Expand the Model Data Tree then expand Volumes.
  2. Expand the Solid volume and activate the Volume Mesh Attributes check box.
  3. In the detail panel, change the Absolute mesh size to :=dr.


    Figure 25.
    Note: :=dr refers to the value of the variable dr, which was defined in the Variables Manager earlier. This means that the Solid volume group has an absolute mesh size of 0.0001m.
  4. The SolidHeated volume group has the same mesh parameters as the Solid group. In order to avoid repeating steps, you can propagate the settings of Solid.
    1. Expand the Solid volume group.
    2. Right-click on Volume Mesh Attributes and select Propagate.
    3. Select the SolidHeated group in the pop-up window and click Propagate.

Set Surface Mesh Attributes

Surface mesh attributes are applied to a specific surface in the model. It is a type of local meshing parameter used to create targeted mesh controls for one or more specific surfaces.

Setting local mesh attributes, such as surface mesh attributes, is not mandatory. When a local mesh attribute is not found for a component, the global attributes are used as the mesh generation control for that component. If a local mesh attribute is present, it will take precedence over the global setting.

In the next steps you will set the surface meshing attributes.

  1. Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
  2. Expand Model in the Data Tree then expand Surfaces.
  3. Expand InterfaceInner and activate the Surface Mesh Attributes check box.
  4. In the detail panel, set the Boundary layer flag to On.
  5. Change Resolve to Number of Layers.
  6. Set First element height to :=firstLayer.
  7. Set Total layer height to :=dr.
  8. Set the Growth rate to 1.2.


    Figure 26.
  9. The surface groups InnterfaceOuter and OuterWall will have the same settings as InterfaceInner. In order to avoid repeating steps, you can propagate settings.
    1. Right-click on Surface Mesh Attributes under Interfaceinner and select Propagate.
    2. Select the groups InterfaceOuter and OuterWall in the pop-up window and click Propagate.

Define Mesh Extrusions

Mesh extrusion is a feature that allows the generation of structured mesh in the entire volume or only on the surface. This feature extrudes the mesh on one surface to another surface and can also be used with other meshing features. In this case, we are going to extrude the mesh along the length of both the Inner and Outer cylinders from one end to the other.

Mesh Extrusion is available under the Model tree.

  1. Right-click on Mesh Extrusions and click New and repeat this step.
  2. Rename Mesh Extrusion 1 and Mesh Extrusion 2 to ZInner and ZOuter respectively.
  3. Double-click on ZInner.
    A Mesh Extrusion Dialog Box opens.
  4. Ensure that the geometry type is surface.
  5. Select -ZInner from the drop-down menu for Side 1.
  6. Select +ZInner from the drop-down menu for Side 2.
  7. Change the Extrusion options to All tets.


    Figure 27.
  8. Click OK to close the dialog.
  9. Similarly, repeat the same procedure for ZOuter. The final dialog should look like the image below.


    Figure 28.

Generate the Mesh

In the next steps you will generate the mesh that will be used when computing a solution for the problem.

  1. Click on the toolbar to open the Launch AcuMeshSim dialog.
    For this case, the default settings will be used.
  2. Click Ok to begin meshing.

    During meshing an AcuTail window opens. Meshing progress is reported in this window. A summary of the meshing process indicates that the mesh has been generated.



    Figure 29.
    Note: The actual number of nodes and elements, and memory usage may vary slightly from machine to machine.
  3. Visualize the mesh in the modeling window. Turn on the display of surfaces and set the display type to solid and wire.
  4. Rotate and zoom in the model to analyze the various mesh regions.

Compute the Solution and Review the Results

Transfer Heat Loss Using the Electromagnetics Manager

The Electromagnetics Manager is a tool designed for transferring the electromechanical heat losses from an EMag (Electromagnetics) output file to the appropriate element set in the CFD mesh. Flux is a simulation software used in the development and design of electrical devices. It incorporates simulation technology to accurately analyze a wide range of physical phenomena that includes complicated geometry, various material properties, and the heat and structure at the center of electromagnetic fields. The electromagnetics mesh and the element set of the CFD mesh on to which the data is transferred must have the same size and coordinates.

In this case, the heat load is already calculated from the Electromagnetics software and imported into the CFD mesh in the form of a .nas (NASTRAN) file. You do not need to calculate this value; it is provided directly with the input files. In the next steps, you will learn how to import this .nas file using the Electromagnetics Manager.

Note: Before importing the Flux values into the CFD mesh, make sure that the .nas file is in your working directory.
  1. From the main toolbar, click the Electromagnetics Manager icon .
    Tip: You can also click Tools > Electromagnetics Manager.
    The Electromagnetics Manager dialog opens.
  2. Click the Add.
  3. Change the name from SPM Motor 1 to Flux.
  4. Click Open next to Import. Select CABLE_EXAMPLE_MOD.nas from your working directory and click Open.
    This opens the Flux Total Heat Source showing the total heat source vs time step plot and the average step data at the bottom.


    Figure 30.
  5. Click OK to close the dialog.
  6. Click Transfer next to Transfer to Element Set.
    This opens the Volumes dialog.
  7. Select SolidHeated and click OK.


    Figure 31.
  8. Click Close to exit the Electromagnetics Manager.
  9. In order to confirm the heat source is correctly applied to the SolidHeated volume group, check the Element Set.
    1. Switch to BAS in the Data Tree Manager
    2. Expand SolidHeated under Volumes.
    3. Double-click Element Set to open the Element Set detail panel.
    4. Click Open Array.
      The heat source is updated for the node id.


      Figure 32.

      You can also see that the Total heat source in the Element Set detail panel is updated.

    5. Click Ok to close the Array Editor.

Run AcuSolve

In the next steps you will launch AcuSolve to compute the solution for this case.

  1. Click on the toolbar to open the Launch AcuSolve dialog.
  2. Click Ok to start the solution process.

    While computing the solution, an AcuTail window opens. Solution progress is reported in this window. A summary of the solution process indicates that the run has been completed.

    The information provided in the summary is based on the number of processors used by AcuSolve. If you use a different number of processors than indicated in this tutorial, the summary for your run may be slightly different than the summary shown.



    Figure 33.
  3. Close the AcuTail window and save the database to create a backup of your settings.

View Results with AcuFieldView

Now that a solution has been calculated, you are ready to view the flow field using AcuFieldView. AcuFieldView is a third-party post-processing tool that is tightly integrated to AcuSolve. AcuFieldView can be started directly from AcuConsole, or it can be started from the Start menu, or from a command line. In this tutorial you will start AcuFieldView from AcuConsole after the solution is calculated by AcuSolve.

In the following steps you will start AcuFieldView, create a boundary surface showing temperature and plot temperature vs the radius of the model.

Launch AcuFieldView

  1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
  2. Click Ok to start AcuFieldView.
    When you start AcuFieldView from AcuConsole, the results from the last time step of the solution that were written to disk will be loaded for post-processing.

Create a Boundary Surface Showing Temperature on the Surface

  1. Click Viewer Options.


    Figure 34.
  2. In the Viewer Options dialog:
    1. Deselect Perspective to turn off the perspective view.
    2. Click Axis Markers to disable the axis markers.
    3. Click Close.
  3. On the toolbar, click the Colormap icon .
  4. In the Scalar Colormap Specification dialog, click Background and select White.
  5. Close the Scalar Colormap Specification dialog.
  6. Click the Toggle Outline icon on the toolbar to turn off the outline display.
    Your display should now look like this.


    Figure 35.
  7. In the Boundary Surface dialog, ensure that Coloring is Scalar and all the Boundary Types are selected.
  8. Set the Display Type to Constant.
  9. Deactivate the box besides Show Mesh.
  10. From the toolbar, click to open the Defined Views dialog.
  11. Select +Z then click Close.
  12. Click the Colormap tab in the Boundary Surface dialog and select the Local check box to display the local range of values for temperature for the selected surface.
  13. Change the Max temp to 304.8 K and the Min temp to 293.0 K.
  14. Click the Legend tab and activate the check boxes for Show Legend and Frame.
  15. Enter (K) as the units for temperature in the Subtitle text.
  16. Change the Labels, Annotation, and Subtitle color to black.
    Tip: You can move the legend using Shift + left-click.


    Figure 36.

Create an XY Plot for Temperature vs Radius

In this section, you are going to create a plot and see how temperature varies along the radial direction between the two cylinders. For that take two points along the cross-section of the cylinders in radial direction. The figure below shows the two points along the radial direction from the inner cylinder to outer cylinder.


Figure 37.
  1. From the Visualization toolbar, click the Plot icon .
    The 2D Plot Controls and Plot Display dialogs open.
  2. In the Plot tab of the 2D Plot Controls dialog, click Create.
  3. Select temperature as the Left Axis Function.
  4. In the Paths tab, click Create and select Line Path (volume)....
  5. In the Edit Points dialog, enter the coordinate values for the two points as shown below.


    Figure 38.
  6. Click Calculate and OK to close the dialog.
    The Plot Display dialog is updated.


    Figure 39.
  7. Returning to the Plot tab of the 2D Plot Controls dialog, change the Horizontal Axis/Plotting Direction to Y. Click OK in the pop-up warning.
  8. Click Axes.
    The Horizontal Axis dialog opens.
  9. In the Horizontal Axis dialog:
    1. Change the Label to Radius (m).
    2. Change the Min value to 0.002.
    3. Change the Max value to 0.003.
    4. Change the Unit value next to Major to 0.0002.


    Figure 40.
  10. Click the Left Axis tab.
  11. Change the Label to Temperature (K).
  12. Change the Max value to 305 and the Unit value next to Major to 2.


    Figure 41.
  13. Click Close.
    The Plot Display dialog is updated once more.


    Figure 42.

Summary

In this tutorial, you worked through a basic workflow to set up a steady state simulation for a 2D cable problem. This problem was setup as a normal heat conduction problem where the inside solid volume was provided with a heat source. You started the tutorial by creating a database in AcuConsole, importing and meshing the geometry, and setting up the basic simulation parameters. Once the case was setup, the solution was generated with AcuSolve. Results were also post-processed in AcuFieldView by reading a dataset and viewing the temperature contours on the full geometry. New features that were introduced in this tutorial included the Electromagnetic Manager, which was used for importing a Nastran file that contained the thermal load applied to the SolidHeated volume, the variable manager, for defining all the variables in a single panel, mesh extrusion from one surface to the another surface along the length, reading a dataset in AcuFieldView, and finally, making 2D plots in AcuFieldView.