SimScale CAE Forum

Step-by-Step Tutorial Session 3: Blood flow in a Carotid Artery Bifurcation


#1

Recording


Homework Submission


For your homework, your task is to simulate the blood flow through 3 different arteries, the first, with a healthy blood vessel with no calcification or blockage; the second, through a moderately calcified blood vessel and the third, through a severely calcified or occluded blood vessel.

The step-by-step tutorial below contains all of the steps for setting up the simulation in SimScale and visualizing the results.

To submit your homework assignment, please generate a public link of your project (Sharing a Project)

Homework Deadline: Sunday, February 18th, 11:59 pm CET

Submit your homework here

Introduction


In this exercise, we will focus on simulating the flow of blood as a non-newtonian fluid through a Carotid Artery Bifurcation. The simulations are performed for 3 cases - the first, with a healthy blood vessel with no calcification or blockage; the second, through a moderately calcified blood vessel and the third, through a severely calcified or occluded blood vessel. The results will show the differences in pressure, velocity profile, and the outlet flow through the 2 branches.

The image below shows an overview of the 3 different cases:

This tutorial presents a step by step approach for simulating the third case with 85% occlusion of the Artery. The first 2 cases can then be done by duplicating the setups and following similar steps.

Import Project


To start this exercise, please import the project into your workspace by clicking on the link below:

https://www.simscale.com/workbench?publiclink=04ca82d9-8440-462e-928e-bdcd4938f118

Mesh Generation


In the Mesh Creator tab, click on the geometry Case -3-85-pc-blocked

Then, click on the New Mesh button in the options panel.


Figure 2: Creating a new mesh from geometry

Select the mesh Type Hex-dominant parametric. Then specify the following parameters:

  • Number of cells in X-direction: 45
  • Number of cells in Y-direction: 150
  • Number of cells in Z-direction: 20
  • Number of computing cores: 16

Click Save to preserve the mesh settings

Figure 3: Base mesh cells and number of core selection.

After saving the Navigator is expanded with 2 new entries, called Background Mesh Box and Material Point which must be defined.

The Background Mesh Box defines the reference bounds of the base mesh. Enter the values as shown or use the default values:

  • Min X= -0.019
  • Min Y= -0.065
  • Min Z= -0.004
  • Max X= 0.013
  • Max Y= 0.0415
  • Max Z= 0.01

Click Save to preserve the mesh settings


Figure 4: Background Mesh Box settings.

The Material Point specifies the region that will be meshed. So, in this case, the point must be inside the body.
Enter the values:

  • Center X= 0.0025
  • Center Y= 0.001
  • Center Z= 0.0025

Click Save to preserve the mesh settings


Figure 5: Material point located inside the geometry to ensure internal mesh is created.

We will create a new geometric entity that will be later used for refinement of the narrow blocked region.

To create a New entity, click on Geometry Primitives and then the +New button on top to select a Cylinder entity.


Figure 6: Cylinder primitive creation

Enter the values as shown:

  • Reference Point (x): -0.01
  • Reference Point (y): -0.043
  • Reference Point (z): 0
  • Axis (x): 0.0055
  • Axis (y): 0.016
  • Axis (z): 0
  • Radius: 0.003

Click Save to preserve the mesh settings


Figure 7: Cylinder primitive settings.

We will now add the necessary mesh refinements for the previously created geometry sets and the geometry primitives.

Click on Mesh Refinements and click +New button to add a refinement.


Figure 8: Mesh refinement creation

Ref-surface

This refinement will be used to refine the surfaces for the complete solid geometry. Select the settings as follows:

  • Name: Ref-surface
  • Type : Surface refinement
  • Level Min : 2
  • Level Max : 2
  • Assigned entity Type: Volume
  • Entity: solid_0


Figure 9: Surface refinement settings and selection.

Click Save to preserve the mesh settings

To create another refinement, hover your mouse over Mesh refinements and right-click to select Add mesh refinement.

Figure 10: Additional refinement creation.

Ref-layer

The layer refinement is important to capture the behaviour near the wall. This will create layer cells following the surface curvature near the walls.

Add a new Mesh Refinement, and choose:

  • Type : Inflate boundary layer
  • Change Number of layers: 3
  • Keep the rest to default

Under the selection box, select the surfaces:

  • shell_0_face_0
  • shell_0_face_2
  • shell_0_face_3

Click Save


Figure 11: Layer inflation settings and assignements.

Ref-edges

The feature refinement will refine near edges. This is important to capture sharp corners.

Add a New Mesh Refinement, and choose Type as Feature Refinement

Give a Distance of 0.0005 and a Level of 3.


Figure 12: Edge Refinement settings.

Ref-volume-region

These regional refinements will refine the volume mesh. The first is for the entire inner region

Create a new Mesh Refinement enter the settings as follows:

  • Name: Reg-volume
  • Type : Region refinement
  • Mode : Inside
  • Distance : 1
  • Level : 1
  • Under Refined regions box select: solid_0

Then click Save


Figure 13: Region refinement settings for solid.

Ref-blocked-region

The next region is for the narrow blocked area. So create another ‘Mesh Refinement’ and enter the settings as follows:

  • Name: Reg-blocked
  • Type : Region refinement
  • Mode : Inside
  • Distance : 1
  • Level : 3
  • Under Assigned Geometry Primitive box select: Cylinder

Then click Save


Figure 14: Region refinement settings for blocked region.

Now click back on the main mesh Operation 1, scroll down to the settings panel to Mesh Quality controls and change the 3 parameters as shown and Save:

  • Max non-orthogonality angle [°]: 65
  • Max concaveness [°]: 70
  • Min cell volume [m³]: 1e-18
  • Note: This is important to get a good quality mesh.

Figure 15: Quality settings to ensure a high-quality mesh is produced.

The mesh settings are all prepared, so click the Start button to begin the mesh generation process. This will take about 5 minutes.


Figure 16: Starting a mesh operation.

Once the process is finished, the mesh is automatically loaded in the viewer.


Figure 17: Finished mesh.

Additional Meshes

Rather than creating meshes for Case 1 and Case 2 from scratch, it is faster to duplicate the mesh you’ve just created and then change the Base Geometry. To duplicate the mesh, just click on the Case-3-85pc-blocked mesh, then right-click and select Duplicate


Figure 18: Duplicating the mesh for other cases.

Then click on the duplicated mesh, rename the mesh to Case-2-60pc-blocked mesh, change the Base Geometry to Case-2-60pc-blocked and click Save. (click yes on the confirmation/warning message)


Figure 19: Change name and geometry of the duplicated mesh setup.

Then you will have to Re-assign the corresponding Refinement entities as before.

Figure 20: Re-assigning entities to refinements.

Once done go to Operation 1. Click Save and Start to generate the 2nd mesh.

Use the same methodology to create the mesh for Case-1-Normal. Once you have created all 3 meshes, proceed to the next section of the simulation setup.

Simulation Setup

For setting up the simulation switch to the Simulation Designer tab and select +New

Give the simulation a meaningful name: Turb-Steady-blood flow-85pc


Figure 21: Creating a new Simulation.

Select the analysis type: Fluid dynamics and Incompressible


Figure 22: Selecting Incompressible from the fluid dynamics category.

Set the Turbulence model as k-omega-SST and Steady-state. Then click Save.


Figure 23: Selecting turbulence model and defining steady state.

After saving, the Navigator now looks as shown below. Here the entries in Red must be completed.

Figure 24: Showing entries in the tree that need to be compleated.

Click Domain from the tree and select Case-3-85-pc-blocked mesh. Click the Save button. The mesh will then automatically load in the viewer.

Figure 25: Selecting the mesh under the domain entry.

Now we will create topological entity sets to group the faces together.

Click on the tree entry Topological Entity Sets.

Select the shown face from the viewer (left-click selection), then click the Create set button in the toolbar.

Name the set Common Carotid Artery Inlet.


Figure 26: Creating the inlet entity set.

Next, select the 2 shown outlet faces from the viewer, then again click Create set button in the toolbar.

Name the set Carotid Artery Outlets (it has 2 faces)


Figure 27: Creating the outlet entity set.

Select both entity sets in the viewer try on the right, right-click in the viewer, and invert the selection. Now create an entity set on the new selection, called *Walls.


Figure 28: Creating the entity set for the walls.

your selection should show all faces except inlets and outlets selected as depicted below.


Figure 29: Selection after the inversion.

Once done, you will have three sets with the shown number of faces:


Figure 30: List of entity sets with expected number of faces.

We now add a Fluid material (Blood). Select the Material item in the Navigator and click New


Figure 31: Creating a new material (Blood).

Specify the given properties to define the non-newtonian model for blood (for details see Documentation):

  • Viscosity model: Bird-Carreau
  • Viscosity at zero shear nu0 [m²/s]: 0.00005283
  • Viscosity at very high shear nuInf [m²/s]: 0.0000032547
  • k [s]: 3.313
  • n [-]: 0.3568
  • a [-]: 2
  • Density [kg/m³] = 1060

Now to assign this fluid to the mesh domain, select the available domain called region0 and click save.


Figure 32: Specifying the material Blood and assigning it to region0.

The boundary conditions define the flow variables at the boundary surfaces.

Click on Boundary condition and select +New.


Figure 33: Creating a new boundary condition.

Inlet

Select the Type as Pressure Inlet, and Type as Total Pressure

Gauge Total Pressure [Pa]: 1184

Pressure difference was taken using a known flow rate through a healthy artery and applied to the inlet to ensure pressure driven flow. Pressure can be applied to the inlet and zero pressure at the outlet since this is an incompressible flow simulation.

From the selection box, select the previously created Common Carotid Artery Inlet and click Save


Figure 34: Specifying the settings for the Pressure Inlet.

Outlet

Add another boundary condition, select the Type as Pressure Outlet and keep the other parameters as default. (here the zero value is only a reference)

From the selection box, select the previously created ‘Outlet set’ and click Save


Figure 35: Specifying the settings for the pressure outlet.

Artery walls

Lastly, add another boundary condition for the Artery walls.

Select the Type as Wall, velocity as No-slip and change the wall treatment to zeroGradient

From the selection box, select the previously created Artery walls topological entity set and click Save


Figure 36: Specifying the settings for the Artery Walls.

Under the Numerics item in the Navigator, make the following changes to improve the solution accuracy.


Figure 37: reducing the termination criteria for all residuals.

Under Simulation Control set the parameters as follows:

  • Start time value [s]: 0
  • End time value [s]: 4000 (these are basically iterations for steady state analysis)
  • Time step length [s]: 1
  • Write control : Timestep with Write interval (simulation time steps)=2000 (to save only the final solution)
  • Number of computing cores: 8
  • Maximum runtime [s]: 9000
  • Initialize with potential flow: false


Figure 38: Adjusting the Simulation Control Settings to ensure convergence is reached.

Result Control

Click on Result control and add a Surface Data result control Item. Change the name to Integrals and type to Area Integral. Set it to update every 10 iterations and select the Common Carotid Artery Inlet as the surface. This will measure the volume flow rate through the artery.


Figure 39: Defining the surface Integral result control item.

Simulation Runs

Click on Simulation runs and create a New run.


Figure 40: Creating a new run on the selected simulation.

The run should automatically start.

The simulation will take around 40 minutes to Finish. Once finished, the results can then be viewed.


Figure 41: Convergence plot of a finished run.

Additional Simulations

To set up the simulations for the other 2 configurations, you can duplicate the first simulation setup by right-clicking on the Turb-Steady-blood flow-85pc and select Duplicate. Then continue by selecting the appropriate mesh (Case-2-60pc-blocked mesh or Case-1-Normal mesh) under the Domain item in the Navigator and following the previous steps.

Post-Processing


To view the results, switch to the Post processing tab.

Click on Solution fields under Run1 in the navigation tree to load the results. This will take a minute or more depending on the internet speed. Once loaded it will be as shown in the figure below.


Figure 42: Bring a solution into the Post-processor viewer.

To visualize the internal region we will create 3 Slice filters.The parameters for each are given in the table below:

Table 1: Table of slice filter settings for slices 1, 2 and 3.

Slice Filter

To create a Slice filter, click on Run 1 and then the Add filter button. Select the Slice option.


Figure 43: Add a slice filter from the drop down list.

Wait for the filter to apply. Then enter the parameters for Origin and Normal as given in the table.

Uncheck the option Show Plane and click Apply

From the fields drop down (top-left corner) select U [point-data] to view velocity magnitude.


Figure 44: Slice filter 1 showing velocity magnitude.

Follow the same procedure to create the Slice 2 and Slice 3. After creating the 3 Slices, the results will look as shown below (Note: be sure to create each slice from Run 1):


Figure 45: Showing slices 1, 2 and 3 coloured by velocity magnitude.

To view the body walls, click again on Run 1 as shown and click the eye icon to turn it on.

From the fields drop down (top-left corner) select solid color

Then in the properties, under Representation, change Opacity to 0.3 and click Apply


Figure 46: displaying the geomitry as a transparend solid object to add context to filters.

Streamlines Filter

Click again on Run 1 (highlighted in blue) and Add filter to select Stream Tracer

Wait for the filter to apply. Then enter the parameters as below:

  • Center: 0.0025, 0.001 , 0.0025
  • Radius: 0.003

…and click Apply

Then from the fields drop down (top-left corner) select U [point-data] to view velocity magnitude.


Figure 47: Shows streamlines of velocity vectors coloured by velocity magnitude.

Compare the results from each configuration, what observations can you make?

Comparing Viscosity

To observe how viscosity is affected by the blockages, it is useful to compare the results side by side. This can be done easily in the online post-processor adding additional solutions to the view and transforming them.

Start by adding the solution for the 85pc blocked case, do this by selecting the solution fields.


Figure 48: Bring a solution of case 3 - 85pc into the Post-processing viewer.

Once it is in the viewer, add a slice that is identical in setup to the previously defined Slice 1.


Figure 49: Add a slice filter.


Figure 50: Change settings to those of slice 1 as was previously detailed.

Since viscosity is the field of interest this time, change the displayed field to nu.


Figure 51: Change the coloured field to be viscosity (nu).

Now an additional solution needs to be added, this time instead of clicking the solution field of the 65pc case, right click and add it to the viewer. You should now see both solutions in the same Post-Processing instance.


Figure 52: Bring in additional solution from case 2 - 65pc by right-clicking and adding to viewer.

Now add to that new solution the same slice as defined before. Change the display field once again to viscosity.


Figure 53: Add the same slice to the new solution.

Now we will add a new filter, transform moves the selected data in any direction, rotation or scaling. This is useful to reposition our results. Displace the results in the positive x-direction by 0.035m.


Figure 54: Add a transform filter to the new slice to display the solutions side-by-side.


Figure 55: Transform the solution in the x direction by 0.035m.

Do the above steps for the final solution for the normal artery without blockages, but this time displace it in the x-direction by 0.07m. This will show all solutions next to each other.


Figure 56: Rescale viscosity to the visible range.

Finally, we can save this state so that it can be re-used at a later date by clicking the Add State button, and a Post-Processing image can be created from the viewer by navigating to View and then clicking the image capture button.


_Figure 57: Displays all solutions side-by-side, save this sate with the save state button.


Figure 58: Save screenshot of the Post-Processing views.

What do these results say about viscosity in each of the cases? and how might this further affect the patient’s health?

Viewing Result Control Items

In the Post-Processor under the simulation run, there will be an area average item expand it and expanded the integral node also. View the integral for Uy, this represents the volume flow rate. Compare the final value to the other simulation runs.


_Figure 59: Integration Plot for velocity in the y direction, representing volume flow rate during the solution.

We can quickly create a plot from these values to compare the flow rates between the healthy and blocked arteries.


Plot 1: Shows the flow rates due to the defined pressure differences for each case.

What does this mean for health of the patient?

References


[1] The base CAD model for the Artery used in this homework session is provided by aaron from GrabCAD . It was modified and prepared for CFD analysis.


#3

Hi, Please notice that in simulation control screenshot, end time value is 4000 but in the writing, it is 2000. Maybe, the difference will not affect much more to the overall result however I just wanted to inform you. Btw I’m taking 2000.

Thanks for the great workshop and tutorial!
Best wishes!


#4

Thanks, @Eshqin, I’ll update the images shortly! :slight_smile:

Glad you are enjoying it!

Kind regards,
Darren

Update: Post processing images all show iteration 4000.

Update 2: Ah ok, sorry… text now also updated!


#5

Hi @1318980, I got the result but I think something is wrong here.

Well, for normal case max velocity is 0.327, for 60% occlusion case max vel is 0.7566 and for 85% occlusion case max vel is 0.4924. I expected max vel for 85% case because velocity in the narrow part should be higher than velocity in the large part.
Then, I thought that maybe, it is related to viscosity phenomena but even if it is related to viscosity then max velocities should be increased like normal case - 60% case - 85% case.

I get confused, can you please explain it to me?


#6

Hi @Eshqin, great question.

Consider these two Post-Processing images:


We can see that in the 85% case the flow is so restricted that the ‘easiest’ channel for the flow to go is down the unrestricted Artery, and the blocked channel therefore passes a much lower flow rate. In the 65% blocked Artery, this would still be the case but on a much smaller scale. This could be monitored if you wished by adding area integrals to both outlets also, allowing you to see how much of the flow is being gone through each artery. I would expect minor favouring of the unblocked artery for the 65% artery and a high favouring for the 85% artery, and I would expect the unblocked case to bare very similar flow rates.

Hope this helps,
Darren


#7

Oh man, @1318980 I think I got it. So, from my understanding, we can’t say that for the same fluid, maximum velocity among the three cases will be in the 85 % case because both area and flow rate are different in each case?
and attached images seems reasonable? right?


#8

Hi @Eshqin, yes I think you have it :slight_smile: the post-processing shots seem reasonable and very close to my results. Viscosity will play a part in this for sure, a more viscous fluid will make the resistance down the blocked side even greater.

Cheers,
Darren


#10

Hi, I am struggling to create the last bar graph. Do you have any tips on how to make it?
Thanks
Emily


#11

Hi @emalkin, The last bar graph is simply there to compare the results of all three simulations using the results control outputs. This was done outside of SimScale by simply creating a bar graph using the flow rates and case names in a spread sheet software. This isn’t required as part of the homework, but more to enhance the understanding of the values.

Let me know if I can help any more,
Darren


#12

Hi @1318980

How can we make complex geometries like in the case of above tutorial? I need to start a project on the topic “Transport of drug in the brain tissues”.

Thanks in advance

Regards,
Pankaj


#13

Hi @pankajkumar979, this particular geometry was taken from Grab CAD and modified for our purpose. I think in general geometries are created from scans in the form of STL’s. If you have access to scans then this might be your best bet.

This model was created from a scan, however I don’t know how detailed it is, or how much cleanup it might need: https://grabcad.com/library/brain-4

Hope this helps,
Darren


#14

Hi, I am hard-wired to the internet with a fast connection, and it seems to take too long to load results. Is this normal?
Are there any alternatives for post-processing? I see there seem to be other options such as Paraview? Do you have a tutorial on how to use this with Simscale results?
Thanks!


#15

Hi @croldanp, if it takes longer than 5 mins and you feel you have a good connection I would refresh the page. If this still doesn’t sort it, you can indeed download the results and analyse in Paraview.

This is probably a good place to start:

If you have any further queries feel free to reach out to me!
Darren


#16

Hi @1318980,

I found an opensource software simvascular, this can process MRI images and can turn it into a 3D geometry. lets see how this works out.

In this tutorial, why wall functions are not used? However, zero gradient does ensures that fluid does not passes through boundary. Is it because dimensions are small and fluid is non-Newtonian?

Thanks,
Pankaj


#17

Hi @pankajkumar979, by using zero gradient with a no-slip condition what we are actually doing is a full resolve of the boundary layer. This is because the desired Y+ value for the first cell is unlikely to meet the desired criteria for wall function (30-200). This is because of the fluid velocity and viscosity, and its effects on the thickness of the layer. There for the Y+ value is likely to be much lower, and therefore to maintain accuracy at the boundary we must solve it.

Hope this helps,
Darren