Usability: Applying the Template Simulation File

This tutorial demonstrates applying the template simulation file to another geometry.

  1. Select File > New.
  2. Near the top of the Create a File dialog, to the right of the Template field, click Select.
  3. In the Open dialog, navigate to the file QueryTutorial_TemplateFile.simt and click Open.
  4. In the Create a File dialog, click OK.
  5. Save the simulation as QueryTutorial_MultiplePipes.sim.
Import the next geometry and visualize it. You are importing a set of connected pipes.
  1. Import the connected pipes on which to run the simulation:
    1. Select File > Import > Import Surface Mesh.
    2. Navigate to the surface file pipeAssy.x_t in the foundationTutorials folder of the downloaded tutorial files.
    3. In the Import Surface Options dialog, accept the default settings and click OK.

    The complete geometry appears in the scene.



Before running the mesh pipeline, you must identify the upstream and downstream faces of the imported assembly. The Fill Holes operation requires that these faces be correctly assigned.
  1. Apply the inlet and outlet tags on the imported geometry parts:
    1. Expand the Geometry > Parts > Pipe 1 > Surfaces node.
    2. Right-click the Inlet node and select Tags > Set > Inlet End.
    3. Expand the Pipe 4 > Surfaces and Pipe 6 > Surfaces nodes.
    4. Multi-select the Outlet nodes in these Surfaces nodes, right-click one of them, and select Tags > Set > Outlet End.
  2. To run the mesh pipeline as far as Extract Volume, expand the Geometry > Operations node, right-click the Fill Holes, Imprint, and Extract Volume nodes in turn and select Execute for each.
You must assign the boundary conditions before running the Automated Mesh operation, as otherwise prism layers are generated across the inlet and outlet faces. By assigning boundaries first, the prism layer mesher only generates layers on the pipe walls.
  1. To assign the boundary conditions, apply the Inlet End and Outlet End tags to the respective faces within the Extract Volume part:
    1. Expand the Parts > Extract Volume > Inherited Parts > Fill Holes node.
    2. To the Pipe 1.Inlet node, apply the tag, Inlet End.
    3. To the Pipe 4.Outlet and Pipe 6.Outlet nodes, apply the tag, Outlet End.
  2. To generate the volume mesh, right click the Geometry > Operations > Automated Mesh node and select Execute.
  3. To review the boundary assignments of the parts, expand the Regions > Fluid > Boundaries node:
    • The Inlet boundary has one part surface assigned to it.
    • The Outlet boundary has two part surfaces.
    • The Wetted Wall boundary contains the rest of the parts.

    These assignments of part surfaces are correct because you prioritized the selection of them in the template simulation.

  4. To visualize the mesh, create a mesh scene.


Since the physics models were prepared in the template, you are ready to run the simulation.
  1. Click (Run) in the top toolbar.
    The Residuals display is created automatically and shows the progress of the solver.
  2. You can evaluate the design with scalar or vector scenes, or plots.
  3. Save the simulation.