Non-Newtonian Fluid
Blood flow of FDA Nozzle
Download mesh Download simulation Link to youtube video
Introduction
FDA's Nozzle Challenge is a benchmark testing program for simulation validation organized by the U.S. Food and Drug Administration. In this program, experimental and simulation studies were conducted on small nozzles that reflect the characteristics of blood-carrying medical devices, and the following papers by Trias et al. were referenced.
Trias, Miquel, Antonio Arbona, Joan Massó, Borja Miñano, and Carles Bona. “FDA’s nozzle numerical simulation challenge: non-Newtonian fluid effects and blood damage.” PloS one 9, no. 3 (2014): e92638.
Based on the nozzle throat diameter, the Reynolds number is 500, and the non-Newtonian fluid viscosity uses the Carreau model.
Start BaramFlow and load mesh
Run the program and select [New Case] from the launcher. In the launcher, select [Pressure-based] for [Solver Type] and [None] for [Multiphase Model].
Use the given polyMesh folder. In the top tab, click [File]-[Load Mesh]-[OpenFOAM] in that order and select the polyMesh folder.
Geometry and mesh are as follows
General
For this example, we'll use default conditions.
Models
For this example, we'll use Laminar for turbulence.
Materials
Click the (+) in the Materials Configuration to add a waterLiquid.
Open the waterLiquid edit window and set the following settings.
- Name : blood
- Density : 1056
- Viscosity : Bird-Carreau
Click the Edit button next to Bird-Carreau and enter the coefficients as follows
- Zero shear viscosity : 0.0001515
- Infinite shear viscosity : 3.3144e-6
- Relaxation time = 8,2
- Power-law index = 0.2128
- Linearity deviation, a = 0.64
Cell zone Conditions
Double-click region0 to bring up the settings window. Select Material as blood.
Boundary Conditions
Set the boundary type and values as shown below.
- in : Velocity Inlet
- Velocity magnitude : 0.04607
-
outlet : Pressure Outlet
- Pressure : 0
-
wall, wall1, wall2 : Wall
- Velocity : No Slip
-
back, front : Wedge
Numerical Conditions
Set [Convergence Criteria]-[Pressure] and [Momentum] as 1e-6 for both
Initialization
Set the value for velocity and pressure as follows
- Velocity : (0.04607 0 0)
- Pressure : 0
Enter the value and click the Initialize button at the bottom. Then click the [File]-[Save] menu to save the case file.
Run
Change the values as shown below, and click [Start Calculation] button.
- Number of Iterations : 2000
- Save Interval : 500
When the calculation is started, you can see the graphs of Residuals as shown below.
Post-processing
Click the parview button in [External tools] to open the paraview.
Change [Coloring] to U.
To see a graph of velocity on an axis, select [Plot Over Line] from the Fileters menu.
For Line Parameters, enter (-0.1 0 0.001) for Point1 and (0.1 0 0.001) for Point2.
In the [X Axis Parameters], disable [Use Index for XAxis] and select [Point_X for the X Array Name].
In [Series Parameters], select U_X and click the Apply button to see the graph below.
Run 'Save Data' from the File menu to get the velocity along the axis as a data file. The figure below plots this data against the experimental results and the results for a constant viscosity.
