Get the Most Out of the ANSYS Fluent Task-Based Workflow

By Erling Eklund, Lead Software Developer, ANSYS

The new ANSYS Fluent experience enables engineers to perform computational fluid dynamics simulation using a task-based workflow. This ensures that anyone can take the right steps to set up a CFD simulation. Following some easy best practices within the workflow can make using ANSYS Fluent even smoother for both experts and novices.

Save PDF
fluid simulation with Mosaic meshing

"Expand the workflow by creating custom journals that can perform advanced Fluent operations tailored to a specific organization."

Creating a watertight geometry workflow for the pre-processing step of computational fluid dynamics (CFD) simulation is now easier than ever with the new ANSYS Fluent experience. You can access the workflow from the single-window Fluent interface or directly from ANSYS Workbench.

Employing a relatively complicated model as an example — air cooling of an electrical motor — unveils nine best practices to simplify the process even further.

TIP 1: FAULT-TOLERANT WORKFLOW FOR NON-WATERTIGHT GEOMETRIES

A fault-tolerant workflow is available to place a “wrapper” — a layer of mesh that covers up surface imperfections in the geometry — around non-watertight (“dirty”) geometries. This can be especially helpful in simulations of the external aerodynamics of a car, for instance, where there is too much detail to spend the time manually closing leaks in the geometry. This saves time while sacrificing only a little in simulation accuracy.

watertight workflow

The watertight workflow tree

 

TIP 2: CREATE AN OUTER FLOW BOUNDARY USING SHARE TOPOLOGY

For external flow simulations, like the air flow cooling a motor, create an outer flow boundary in ANSYS SpaceClaim by drawing a cube around the motor and using the Share Topology function.

Share Topology combines all overlapping faces between two solids into one face. It also resolves the intersection between the cube and any part of the motor. The flow volume is extracted as part of the Surface Mesh operation in Fluent. The volume takes the shape of the void between the boundaries of the cube and the motor.

advanced meshing options

Advanced options to speed up meshing

 

TIP 3: NAME THE ENTITIES IN ANSYS SPACECLAIM

In the geometry in SpaceClaim, include “fluid” in the name of the cube around the motor geometry. This automatically identifies it as a fluid region within the watertight geometry workflow. And, by adding descriptive strings to the names of other entities, like inlets, outlets and symmetry planes, it is easier for ANSYS Fluent to track them in the pre-processing stage and during simulation.

Share topology definition

Share Topology defines a flow region without Boolean operations.

 

TIP 4: USE NATIVE FLUENT FILES

When importing the CAD model into the Fluent task-based workflow, the software creates a native version of that file with a .pmdb extension. The next time the same model is imported, reading in the .pmdb file retrieves the geometry much faster than returning to the original CAD geometry.

Another advantage of working with the .pmdb file is that it is operating-system–independent, so working in Linux is possible if desired.

Fluent customer tasks

Running custom tasks in the workflow

 

TIP 5: SPEED UP SURFACE MESHING OF CFD GEOMETRY

Some surface mesh options can be toggled to make the meshing process faster. By labeling all entities — like “inlet” or “fluid” — in SpaceClaim (see Tip 2), the need to use zone separation to determine regions within the Surface Mesh is eliminated.

Also, turn off Check Self-Intersection. This operation checks the model for any overlapping faces. It is no longer needed thanks to the Share Topology function.

"Creating a mesh that is ready for CFD analysis now takes minutes when it used to take hours."

TIP 6: VERIFY CFD GEOMETRY FOR ANSYS FLUENT

During the surface meshing operation, Fluent defines boundary types to zones, and region types to volumes. These definitions are based on the entity names specified in SpaceClaim. For example, a boundary named "gas-inlet" is assigned a "velocity-inlet" boundary type.

As a best practice, verify that the boundary and region types are assigned properly before volume meshing. Change a boundary or region’s name and type as needed. Selecting multiple names and right-clicking changes multiple boundaries or regions into the same type. Just remember to click Update once all the boundary types are verified.

geometry verification

Click Update after changing the name or type of a zone when verifying the geometry.

 

TIP 7: USE MOSAIC FOR CONFORMAL VOLUME MESHING

When the volume meshing starts, Fluent makes a fine mesh at the boundary layers. However, maintaining a fine mesh throughout the bulk would be computationally expensive. Use Mosaic meshing technology to link optimal mesh types in the bulk and on the boundary.

First, add boundary layers in the Create Volume Mesh panel. These will only be added on fluid region walls. Then, access the full suite of conformal volume meshing methods, such as tetrahedral, hexcore, polyhedral and poly-hexcore. To use the latest Mosaic meshing technology, select poly-hexcore.

At this point, the standard watertight geometry workflow is complete, and the model can be meshed. It is still possible to insert additional tasks into the taskbased workflow if they are needed, like further refining the volume mesh. Tweaking some standard variables can control the mesh quality.

Expand the standard watertight geometry workflow by creating custom journals. These customized tasks perform advanced Fluent operations that are tailored to a specific organization. Contact ANSYS support to get the user commands needed to set up a custom journal.

Mosaic meshing

"Easy access to parallel processing speeds up Mosaic poly-hexcore mesh generation by up to a factor of 10."

TIP 8: SPEED MESH GENERATION WITH PARALLEL PROCESSING

Use parallel processing to speed up Mosaic poly-hexcore mesh generation by up to 10 times. Utilize up to 64 cores on either your laptop or a cluster, with no need for an HPC license.

fault-tolerant workflow

Fault-tolerant workflow uses a wrapper to speed meshing for non-watertight geometries. 
Geometry courtesy Technical University of Munich

 

TIP 9: EDIT AND SHARE THE MESHING WORKFLOW AT ANY TIME

Some of the biggest benefits of the watertight geometry workflow are the ability to save it, return to it and edit it at any point. Changing a task early in the task-based workflow is easy — even during the final stages of meshing the geometry.

When the workflow is satisfactory, save it and share it with team members. Use the task-based workflow for similar models to give team members a head start on meshing the next design iteration of the motor or other product.

The watertight geometry workflow can also be built into a script that runs the mesh through the Fluent solver. To create this script, use the Start Journal function. Fluent records the script as the workflow proceeds.

The new watertight geometry workflow is a significant timesaver. Creating a mesh that is ready for CFD analysis now takes minutes when it used to take hours.

Mosaic meshing

SAVE VALUABLE TIME

These best practices free up valuable time to work on solving engineering challenges rather than setting up the simulation tools to do so. Give them a try on a future fluids simulation project.

click below to start a conversation with ANSYS

Contact Us
Contact Us
Contact