Pre-Processing Workflow for a Fluid Channel with Solid Blockage in STAR-CCM+

Pre-Processing Workflow for a Fluid Channel with Solid Blockage in STAR-CCM+

Overview

This tutorial walks users through setting up a CFD simulation of a simple fluid channel containing a solid blockage using Simcenter STAR-CCM+. Building on the geometry created in Build a Flow Channel with a Solid Blockage in STAR-CCM+ 3D-CAD, it provides step-by-step guidance for each stage of the pre-processing workflow—covering Parts, Contacts, Regions, Interfaces, and Physics setup. By illustrating how these elements interconnect, the tutorial helps users gain a deeper understanding of how STAR-CCM+ organizes and manages pre-processing tasks, laying a strong foundation for more advanced simulations.

Parts

Create Fluid and Solid Parts using the geometry created in Build a Flow Channel with a Solid Blockage in STAR-CCM+ 3D-CAD.
  1. Multi-select Geometry > 3D-CAD Model 1 > Body Groups > Fluid and Solid. Right-click and select New Geometry Part…
    Figure 1
  2. In Part Create Options dialog select All CAD Edges for Mark Feature Edges and Fine Tessellation Density. Click OK. These settings are for demonstration only and do not represent best practices.
  3. Geometry > Parts are now populated with Fluid and Solid parts and Geometry > Contacts shows a Fluid/Solid conformal contact.
    Figure 2=

Contacts

Create Fluid periodic Contact between Periodic0 and Periodic1 Surfaces. Repeat this process for Solid part. These contacts and the contact populated from 3D-CAD to Part definition between the Solid and Fluid part will be used to create Interfaces when we create Regions.
  1. Create Fluid periodic Contact between Periodic0 and Periodic1 Surfaces. Multi-select Geometry > Parts > Fluid > Surfaces > Periodic0 and Periodic1. Right-click and select Create Periodic.
    Figure 3

  2. Repeat the previous step for Geometry > Parts > Solid > Periodic0 and Periodic1 surfaces. Contacts are now popular these Periodic Contacts. One for Fluid Part and the other for Solid Part.
    Figure 4

Regions and Interfaces

Create Fluid and Solid regions and their associated Interfaces.
  1. Multi-select Geometry > Parts > Fluid and Solid. Right-click and select Assign Parts to Regions…
    Figure 5
  2. Configure Assign Parts to Regions dialog as follows and click Apply:
    Figure 6
  3. Fluid and Solid Regions are created with populated boundaries and Interfaces. Rename Fluid/Fluid Interface to Fluid Periodic and Solid/Solid to Solid Periodic.
    Figure 7

Geometry Scene

Create a new Geometry Scene to visualize the Fluid and Solid Region.

  1. Right-click Scenes > New > Geometry.
    Figure 8 
  2. Click Scene/Plot in the upper left-hand corner of the Simulation Window.
    Figure 9
  3. Select Geometry Scene 1 > Surface 1 > Parts. Select all Regions and click OK.
    Figure 10
  4. Select Geometry Scene 1 > Surface 1 > Properties and set Color Mode to Distinguish Regions.
    Figure 11
    We can now visualize the two regions in the geometry scene.
    Figure 12

Boundary Conditions

Configure Fluid Region boundary conditions.
  1. Navigate back to the Simulation tree by Select Simulation on the top left corner of the Simulation Window.
    Figure 13
  2. Set Fluid Region boundary types. Select Regions > Fluid > Inlet and set Type to Mass Flow Inlet and Outlet to Pressure Outlet.
    Figure 14

Automated Mesh

Create a single automated mesh operation for Fluid and Solid parts.
  1. Right-click Geometry > Operations and Select New > Mesh > Automated Mesh.
    Figure 15
  2. Select Fluid and Solid Parts. Select Surface Remesher, Automatic Surface Repair, Polyhedral Mesher, and Prism Layer Mesher. Click OK.
    Figure 16
  3. Set the following mesh settings under Geometry > Operations > Default Controls:
    1. Base Size, 0.001 m
    2. Surface curvature, # pts/circle, 64
    3. Maximum Tet size, 1000% relative to base
    4. Post Mesh Optimization, enable Optimize Boundary Vertices and Optimize Cell Topology
  4. Disable Prism Layers inside the Solid Region. Right-click Customer Controls and select New > Surface Control.
    Figure 17
  5. Set Geometry > Operations > Automated Mesh > Custom Control > Surface Control > Parts Surfaces to Solid part and surfaces. Click OK.
    Figure 18
  6. Select Geometry > Operations > Automated Mesh > Custom Control > Surface Control > Controls > Prism Layer and select Disable.
    Figure 19
  7. Rename Surface Control to Solid Disable Prism Layers.
    Figure 20

Physics Continua

Create Fluid and Solid Physics Continua.
  1. Right-click Continua and select New Physics Continuum.
    Figure 21
  2. Right-click Models and click Select Models…
    Figure 22
  3. Select the following models:
    Figure 23
  4. Rename Physics 1 to Fluid.
    Figure 24
  5. Create another Continua and select the following models:
    Figure 25
  6. Rename Physics 1 to Solid.
    Figure 26
  7. Assign Fluid and Solid physics continuums to their respective regions.
    Figure 27

Execute Mesh

The volume mesh is now prepared for execution. 
  1. Click volume mesh icon along the top toolbar.
    Figure 28
  2. Examine the Output window. We to see the Periodic Interfaces are conformal.




    • Related Articles

    • Build a Flow Channel with a Solid Blockage in STAR-CCM+ 3D-CAD

      Overview This tutorial explains how to create a simple flow domain with a solid blockage using Simcenter STAR-CCM+ 3D-CAD parametric modeler. Domain Construct a basic flow channel that will define the domain. Right-click Geometry > 3D-CAD Models and ...

    • Introduction to Simcenter STAR-CCM+ Webinar

      What's in this webinar? SDA Software Director of Engineering Ted Blowe presents this webinar on Introduction to Simcenter STAR-CCM+. The following topics will be discussed: Understanding Simcenter STAR-CCM+: Simcenter STAR-CCM+ serves as a versatile ...

    • What's New in STAR-CCM+ v2302?

      What's in this webinar? SDA Software Engineer Ted Blowe presents this webinar on What's New In STAR-CCM+ v2302. During this webinar you will learn about some of the exciting new enhancements in the latest version of STAR-CCM+, including the following ...

    • Simulating Unsteady Valve Motion Using Overset Mesh in STAR-CCM+

      Introduction To simulate the motion of an unsteady valve in STAR-CCM+, the overset mesh plus DFBI (Dynamic Fluid Body Interaction) technique can be employed. This article provides a concise guide on setting up an overset mesh simulation, focusing on ...

    • Simcenter STAR-CCM+ Custom Installation using Siemens License Server

      Follow these step-by-step instructions to download Simcenter STAR-CCM+ with the new Siemens License Server: Install and setup Siemens License Server (saltd vendor daemon). Download the latest version of STAR-CCM+. Launch the installer. Review and ...