# Blood Flow - CFD Simulation

Source: https://help.sim-flow.com/tutorials/blood-flow
Last updated: 2026-10-14

[Video](https://help.sim-flow.com/tutorials/images/blood-flow.mp4)

## 1. Introduction

This tutorial focuses on a non-Newtonian fluid, specifically modeling blood using the Bird-Carreau transport model. We will use a time-variable inlet velocity profile to map the heart rate. Additionally, we will showcase the post-computation process of calculating wall shear stress and visualizing it through ParaView.

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/download-simflow/)

## 3. Create Case

Open SimFlow and create a new case named *blood flow*.

1. Click **New**
2. Provide name `blood flow`
3. Click **Create** to open a new case

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-blood_flow.png)

## 4. Import Geometry

Firstly, we need to Download Geometries[Inlet](https://help.sim-flow.com/tutorials/downloads/blood-flow/inlet.stl)[Outlet01](https://help.sim-flow.com/tutorials/downloads/blood-flow/outlet01.stl)[Outlet02](https://help.sim-flow.com/tutorials/downloads/blood-flow/outlet02.stl)[Wall](https://help.sim-flow.com/tutorials/downloads/blood-flow/wall.stl)

1. Click **Import Geometry**
2. Select all geometry files *inlet.stl* *outlet01.stl* *outlet02.stl* *wall.stl*
3. Click **Open**

![Blood Flow 02 Import geometry](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_02_Import_geometry.png)

## 5. Imported Geometry Units

The STL format does not contain the unit information, which is defined during the geometry export. Therefore, you must manually specify the correct unit after import. If we do not know the exported unit, we can estimate it based on the total size of imported geometries. The size is displayed next to the *Geometry size* label. In our case, the default unit meter is correct.

1. To confirm the default unit *meter*, press **OK**

![Blood Flow 02 unit](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_02_unit.png)

## 6. Geometry - Blood Vessel

After importing the geometry, it will appear in the 3D window.

1. Click **Fit View** to zoom in on the geometry

![Blood Flow 03 Geometry check](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_03_Geometry_check.png)

## 7. Display Geometry - Blood Vessel

We will change the color of the wall to distinguish it from the other geometries.

1. Select the *wall* from the geometry list or hold the `CTRL` key and click on the wall face
2. Click *Change Object Display Properties*
3. Select `green` color
4. Approve by clicking **OK**

![Blood Flow 04 Geometry color](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_04_Geometry_color.png)

## 8. Meshing Parameters - Inlet

In the *Hex Meshing* panel, we will change meshing properties associated with geometry objects. We want to apply the same settings to all geometries. We will set the parameters for the first surface and copy the configuration to the remaining geometries.

1. Go to *Hex Meshing* panel
2. Select the *inlet* component
3. Enable *Mesh Geometry*
4. Set *Refinement* to *Min 1* *Max 1*

![Blood Flow 05 Meshing Properties 1](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_05_Meshing_Properties_1.png)

## 9. Meshing Parameters - Copy

We want to apply the same settings to all geometries. We will copy the configuration from the *inlet* to the remaining geometries.

1. Select the *inlet*
2. Click *Copy Meshing Properties*
3. Select all the remaining faces as a target *outlet01* *outlet02* *wall*
4. Click **Copy**

![Blood Flow 06 Meshing Properties 2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_06_Meshing_Properties_2.png)

## 10. Base Mesh - Domain

Under the *Base* tab, we will define the domain of the background mesh.

1. Go to *Base* tab
2. Click on **Autosize**
3. Define the number of divisions
   *Division*`60``34``125`

![Blood Flow 07 Base Mesh](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_07_Base_Mesh.png)

## 11. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow inside the blood vessel, we need to place the material point inside the geometry.

1. Go to *Point* tab
2. Specify location inside the blood vessel geometry
   *Material Point*`0``0``-1e-03`

You can specify the point location from the 3D view. Hold the `CTRL` key and drag the arrows to the destination.

![Blood Flow 08 Material Point](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_08_Material_Point.png)

## 12. Start Meshing

Everything is now set up for meshing.

1. Go to *Mesh* tab
2. Press **Mesh** button to start the meshing process

![Blood Flow 09 Meshing](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_09_Meshing.png)

## 13. Mesh

After the meshing process, the mesh will appear in the graphics window. Use the scroll wheel on your mouse to zoom into the model.

![Blood Flow 10 Mesh](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_10_Mesh.png)

## 14. Check Mesh

Check the mesh quality and statistics.

1. Expand the *Options* list next to the default region
2. Select *Check* option
3. The check summary will be displayed in the command window. It also shows checking criteria.

![Blood Flow 11 Mesh check](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_11_Mesh_check.png)

## 15. Mesh - Boundaries

1. Set the following boundary types accordingly
   *inlet* *Patch*
   *outlet01* *Patch*
   *outlet02* *Patch*
   *wall* *Wall*

![Blood Flow 12 Boundaries](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_12_Boundaries.png)

## 16. Simulation Type

We want to analyze the transient flow of a non-Newtonian fluid to model the blood flow. For this purpose, we will use a single-phase, incompressible flow simulation.

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/pimpleFoam/01_single_phase@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/pimpleFoam/02_low_speed@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/pimpleFoam/03_transient@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/pimpleFoam/04_apply@2x.png)

## 17. Turbulence

Due to the small diameter of the vessel and high viscosity of the fluid, it can be assumed that the flow remains laminar.

1. Go to *Turbulence* panel
2. Make sure the *Laminar* model is selected

![Blood Flow 14 Turbulence](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_14_Turbulence.png)

## 18. Transport Properties

For demonstration purposes, we will model the blood as a non-Newtonian fluid using the Bird-Carreau model. We will operate on quantities divided by density and we do not need to specify the density. However, we have to take this fact into account during postprocessing.

1. Go to *Transport Properties* panel
2. Change *Transport Model* to *Bird-Carreau*
3. Set the parameters accordingly
   *\(\nu_0\) \({\sf [\frac{m^2}{s}]}\)*`3.3e-06`
   *\(\nu_{\infty}\) \({\sf [\frac{m^2}{s}]}\)*`1.32e-05`
   *\(K\) \({\sf [s]}\)*`0.6046`
   *\(n\) \({\sf [-]}\)*`0.3742`

![Blood Flow 15 Transport Properties](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_15_Transport_Properties.png)

## 19. Boundary Conditions - Inlet (I)

The flow in the blood vessels is oscillatory in time. We will define the inlet velocity using the time history of one oscillation period. To do so, we will use a table input option. The rest of the boundary conditions we will leave as default.

1. Go to *Boundary Conditions* panel
2. Select the *inlet* boundary
3. Set the *Velocity Inlet* character
4. Change the *Type* of the velocity to the *Fixed Mean Value*
5. Change the *Value [m/s]* to the *table*
6. Click on **Edit Table**

![Blood Flow 16 Boundary Conditions](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_16_Boundary_Conditions.png)

## 20. Boundary Conditions - Inlet (II)

We will use a predefined velocity profile from the external file.
We need to [Download Velocity Profileprofile.csv](https://help.sim-flow.com/tutorials/downloads/blood-flow/profile.csv) and import it into SimFlow.

1. Click on *Load Data From File*
2. Select the *profile.csv* file
3. Press **OK**
4. Loaded data will be presented on the chart
5. Press **Close**

![Blood Flow 17 Boundary Conditions Inlet](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_17_Boundary_Conditions_Inlet.png)

## 21. Initial Conditions

Before we start the simulation, we need to define the flow state at time zero. We will specify a constant velocity equal to ` 0.2 m/s `, which corresponds to the initial inlet velocity.

1. Go to *Initial Conditions* panel
2. Set the initial velocity
   *U*`0``0``-0.2`

![Blood Flow 18 Initial Condition](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_18_Initial_Condition.png)

## 22. Monitors - Boundary

We would like to monitor flow velocity at the outlet boundaries. The results can be later on used to calculate the volumetric and mass flow rates for each outlet.

1. Go to *Monitors* panel
2. Switch to *Boundary* tab
3. Expand *Fields* for the *outlet01*
4. Select the velocity field *U*
5. Repeat this step for the *outlet02* boundary.
   Selected fields will be visible next to the boundary names.

![Blood Flow 19 Monitors](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_19_Monitors.png)

## 23. Run - Time Control

We will set the time of simulation to match the inlet velocity time range. We also want the solver to automatically determine the proper time step. This should lead to good stability and potentially reduce simulation time.

1. Go to *RUN* panel
2. Set the *Simulation Time [s]* to `0.9`
3. Change *Time Stepping \(\Delta t[s]\)* to *Automatic*
4. Set initial and maximum time step (the solver will start computation with the initial value and adjust it in the next iterations, not exceeding the maximum value)
   *Initial \(\Delta t\) \({\sf [s]}\)*`1e-06`
   *Max \(\Delta t\) \({\sf [s]}\)*`1e-02`

![Blood Flow 20 Run Time Control](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_20_Run_Time_Control.png)

## 24. Run - Output

We can control how often results should be saved on the hard drive. We will write the results at the interval of ` 0.02 ` seconds. Note that only saved data will be available during postprocessing.

1. Switch to *Output* tab
2. Set the *Interval [s]* to `0.02`

![Blood Flow 21 Run Output](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_21_Run_Output.png)

## 25. Run - CPU

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to [Request 30-day Trial](https://license.sim-flow.com/trial)

Estimated computation time for serial mode: 1.5 hours

1. Switch to *CPU* tab
2. Click **Run Simulation** button

![run cpu serial](https://help.sim-flow.com/tutorials/images/run-cpu-serial.png)

## 26. Results - Outlet Velocity

Outlet boundary monitors are plotted on the charts next to the *Residual* tab.

1. Switch to *U on outlet01* tab
2. Click *Adjust Axes*
3. Set the range for X and Y axes:
   *X Min*`0`
   *X Max*`0.9`
   *Y Min*`0`
   *Y Max*`1.2`

![Blood Flow 23 Plot results](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_23_Plot_results.png)

## 27. Calculate Wall Shear Stress

Calculations are finished, but before we start postprocessing, we will calculate wall shear stress (WSS). It can be calculated as the multiplication of dynamic viscosity and velocity gradient next to the wall. WSS is a characteristic value in medicine, used for circulatory system disease identification. Too low values are the indicators of atherosclerosis, while the large WSS leads to the thickening of the vessel wall and increasing its diameter. This occurs when one vessel splits into two, like in our example.

1. Go to *Calculate* panel
2. Switch to *Wall* tab
3. Set the *Time Range* to *Full Time Range*
4. Set the *Wall Calculation* to *Wall Shear Stress*
5. Click on **Calculate**

![Blood Flow 24 Calculate WSS](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_24_Calculate_WSS.png)

## 28. Postprocessing - ParaView

After computations are finished, we can do a complex visualization of our results with ParaView.

1. Go to *POSTPROCESSING* panel
2. Click on *Run ParaView*

![Blood Flow 25 Postprocessing ParaView](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_25_Postprocessing_ParaView.png)

## 29. ParaView - Load Results (I)

Load the results into the program.

1. Select *blood_flow.foam*
2. Click **Apply** to load results into ParaView
3. After loading results, they will be shown in the 3D graphic window

![Blood Flow 26 ParaView Load Results 1 v2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_26_ParaView_Load_Results_1_v2.png)

## 30. ParaView - Load Results (II)

ParaView skips the initial time step by default. Therefore, we need to add the zero time to the simulation.

1. Uncheck *Skip Zero Time*
2. Click **Refresh**
3. Click **Apply**
4. Set the time or time step to `0`
5. Select the velocity *U* from the list

![Blood Flow 27 ParaView Load Results 2 v2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_27_ParaView_Load_Results_2_v2.png)

## 31. ParaView - WSS

To get the true value of the wall shear stress, we need to multiply SimFlow results by the density. Please remember that for the sake of this tutorial we have created a coarse mesh. We also model the vessel as rigid walls, whereas in reality, it’s hyper-elastic. Nevertheless, still we can identify the regions of extremely high and low wall shear stresses.

1. Select *blood_flow.foam*
2. Click *Calculator*
3. Expand the vector list in the calculator
4. Select *wallShearStress*
5. The selected vector appears in the equation. Now we will multiply the vector by the blood density `1060`
6. Set the result name to *WSS*
7. Click **Apply**
8. Select the wall shear stress *WSS* from the list
9. Play with the animation buttons to track the results of the analysis
10. Click on *Rescale to data range over all timesteps*

![Blood Flow 28 ParaView WSS v2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_28_ParaView_WSS_v2.png)

## 32. ParaView - Streamline (I)

Finally, we can take a look at streamlines.

1. Select *Stream Tracer* from the top menu
2. Select velocity *U* from the vectors list
3. Change Seed Type to *Point Source*
4. Type the center coordinate and radius of the sphere:
   *Center*`0``0``-0.0005`
   *Radius*`0.0007`
5. Uncheck the *Show Sphere*
6. Increase the number of points to `200`
7. Click **Apply**
8. Select the velocity *U* from the list
9. Click on *Rescale to Data Range*

![Blood Flow 29 ParaView Stream Line 1 v2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_29_ParaView_Stream_Line_1_v2.png)

## 33. ParaView - Streamline (II)

To show the geometry together with the streamlines, we will follow these steps:

1. Click on the eye next to *blood_flow.foam*
2. Select *Solid Color* from the list
3. Change the opacity to `0.3`

![Blood Flow 30 ParaView Stream Line 2 v2](https://help.sim-flow.com/tutorials/images/blood-flow/Blood_Flow_30_ParaView_Stream_Line_2_v2.png)

## 34. Advanced Postprocessing with ParaView

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculate volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, *Paraview CFD Tutorial - Advanced Postprocessing in ParaView*, in which we demonstrate some of the most commonly used postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)