Numerical Solution

Reference Values:

The drag is calculated by integrating the shear and pressure at the wall. The drag coefficient is then calculated by non-dimensionalizing the drag. The reference entities used in the non-dimensionalization are defined in the Reference Values panel in Fluent. Note that the "Reference Values" will not change your solution for the velocity and pressure at the cell centers. It will affect only the drag coefficient and any other non-dimensional quantities calculated from the solution. Watch the following video for demonstrations:

If you have used SpaceClaim to create geometry, refer to the steps below for Total Surface Area

1. Open Spaceclaim>Measure>Mass Properties
2. Note down Total Surface Area

Summary of Reference Values:

Numerical Solution:

Watch the following video for demonstrations:

Summary for the video:

1. Monitors -> Create -> Drag -> Print to Console -> wall_artery
2. Solution Initialization -> Hybrid Initialization -> Initialize

3. Calculation activities -> Create -> Solution Data Export -> Change File Type to "CFD-Post Compatible"
   Quantities for export:

   Quantities
   Static Pressure
   Total Pressure
   Velocity Magnitude
   x velocity
   y velocity
   z velocity
   wall shear

   * note that you need to export all three components of velocity in order to plot vector field in CFD-Post!

4. Create -> Particle History Export -> File Type to CFD-Post -> Select the injections -> Choose save directory
5. Run Calculation -> Time Step Size 0.01 -> Number of time steps 50 -> Max Iterations/time step 200 -> Hit "Calculate"!

If you are using ANSYS 19.2, refer to the steps below:

1. Setup > Reference values > Type in the values given in the above table
2. Report Monitors > New > Force Report > Drag > wall artery
3. Solution Initialization > Hybrid Initialization > Initialize
4. Calculation Activities > Create > Solution Data Export
5. Change file type to “CDAT for CFD Post and Ensight”
6. Select above mentioned quantities for export
7. Calculation Activities > Create > Particle Data History Export > Select both injections
8. Run Calculation > Time Step Size(s) 0.01 > Number of Time Steps 50 > Maximum Iterations/Time Step 200 > Hit Calculate

Before running the calculation, you should also create a monitor for the inlet velocity so that we can check that the UDF is working correctly in the Verification and Validation step.

1. Report Monitors > New > Surface Report > Area-weighted Average
2. Set Field Variable as Velocity > Velocity Magnitude
3. Select "inlet" under Surfaces
4. Make sure to check the box next to Report Plot
5. Give it a suitable name and click OK
   
   

Go to Step 6: Numerical Results

Go to all FLUENT Learning Modules