1 of 86

From CAD Creation to Post-processing: Stenosed Carotid Artery: Hemodynamics with Ansys Discovery & Ansys Fluent Softwares

Developed and curated by the Ansys Academic Development Team

Juan Doval

education@ansys.com

2 of 86

Learning Objectives

Intended Learning Outcomes
Knowledge and Understanding	Analyze and interpret hemodynamic results to understand their clinical significance in vascular disease Understand Mesh Quality and its acceptable ranges Locate poor mesh elements
Skills and Abilities	Know how to create an anatomically accurate straight stenosed vessel Apply Local Sizing in the mesh on areas of interest Set up and Solve non-Newtonian blood flow simulations
Values and Attitudes	Appreciate the importance of simulation accuracy when modeling physiological flows Develop critical thinking when interpreting CFD results in a biomedical context

Ansys software mentioned	Ansys Fluent®, a fluid simulation software Ansys Discovery™, a 3D product simulation software

3 of 86

This tutorial guides you through the complete workflow of creating, simulating, and analyzing blood flow through a stenosed blood vessel using Ansys Software. Starting with geometry creation in Ansys Discovery software, you'll progress through meshing with boundary layer refinement, setting up a physiologically accurate non-Newtonian blood flow simulation in Ansys Fluent software, and performing post-processing analysis of critical hemodynamic parameters.

The tutorial emphasizes practical aspects of biomedical CFD modeling, including implementation of Boundary Conditions, configuring non-Newtonian blood rheology models, and interpreting clinically relevant flow parameters through Post-processing such as wall shear stress distributions and recirculation zones. Special attention is given to the step-by-step CAD creation and Mesh Quality in the stenotic region to accurately capture flow separation, recirculation, adverse pressures and more, that occur in atherosclerotic vessels.

Through step-by-step instructions and detailed explanations, you'll develop a deep understanding of both the technical simulation workflow and the physiological significance of your results, bridging the gap between computational methods and biomedical applications.

/ About

4 of 86

Notes: This section provides additional context to support educators in teaching this material.

Content: Follow the step-by-step process outlined in the slides, using the screenshots from Ansys Discovery & Fluent software for guidance.

/ How To Use This Tutorial

5 of 86

Section 2 – CFD Simulation with the Ansys Fluent software

Meshing:

Local Sizing and Evaluate Mesh Quality.

Solver:

Laminar Model, Boundary Conditions, non-Newtonian Approximations.

Section 1 – CAD Creation with the Ansys Discovery tool

Main Features:

Sketching, Pull, Move, Blend, Named Selections and Exporting.

/ Overview

6 of 86

Section 1 – CAD Creation with Ansys Discovery Software

Main Features:

Sketching, Pull, Move, Blend, Named Selections and Exporting.

7 of 86

Section 1.1 – Dimensions

Parameter	Typical Values, Dimensions
Artery length	~50 - 100 mm
Normal diameter	6 - 8mm
Stenosed diameter	50% narrowing (3 mm)
Stenosis length	3 - 10 mm

45 mm

10 mm

Length = 100 mm

Give it a try and create the body yourself using these dimensions

Note: Make sure you create your Named Selections! Page 18 – 23

Step 0 consist of defining the desired model dimensions based on typical Carotid Artery size ranges.

Note: ‘Bold’ Parameters are the ones used for the tutorial

8 of 86

Start a Sketch by clicking in the ‘Design’ tab, the ‘Sketch’ button

Note: If Sketch is already selected, the plane Z will be the default plane. To change this, press the key ‘D’ and follow the steps:

Click the x-axis during plane selection for sketching

CAD

Section 1.2 – Sketching

9 of 86

In the ‘Design’ tab, Click the ‘Circle’

Click at the origin of the x-axis to start the sketching in the selected plane. Type 6 mm and press ‘Enter’

Leave ‘Sketch’ by pressing:

Section 1.2 – Sketching

10 of 86

Select the Tab ‘Measure’ and Click on ‘Measure’

Click on the Circle’s edge you just sketched. Check ‘Circle Diameter’ is equal to 6mm

Section 1.3 – Measure Tool (Bonus)

11 of 86

Click and Copy the ‘Circle’ pressing:

Paste the ‘Circle’ in the same position pressing:

Select ‘Move’ by pressing:

And drag in the x-direction by ‘press and dragging’ the ‘blue arrow’

Ctrl

When the dimension box appears, type 45 mm and press ‘Enter’

Section 1.4 – Move Tool

12 of 86

Section 1.4 – Move Tool

Click ‘Select’ in the ‘Design’ Tab and Repeat Steps 8-10 in the new surface that was moved

When the dimension box appears, type 5 mm (Mid Stenosis) and press ‘Enter’

13 of 86

Click ‘Select’ in the ‘Design’ Tab and Repeat Steps 8-10 in the new surface that was moved

When the dimension box appears, type 10 mm (Mid Stenosis) and press ‘Enter’

Note: for consistency, the Second Circle is the one copied and pasted

Section 1.4 – Move Tool

14 of 86

Click ‘Select’ in the ‘Design’ Tab and Repeat Steps 8-10 in the new surface that was moved

When the dimension box appears, type 55 mm

Note: for consistency, the Second Circle is the one copied and pasted

Section 1.4 – Move Tool

15 of 86

Click ‘Pull’ in the ‘Design’ Tab

Click the edge of the last Circle (3^rd from left to right)

Click the arrow normal to the edge and type -1.5 mm (To achieve a diameter of 3 mm, since the value given is pull on Radius)

Note: You can check the measure is correct (3 mm of diameter) by using the ‘Measure’ tab

Section 1.5 – Pull Tool

16 of 86

In ‘Pull’, Click the first ‘Circle’

Press the ‘Up to’ Box (Shown in red)

Click the Second Circle of 6 mm

Section 1.5 – Pull Tool

17 of 86

Click ‘Blend’ in the ‘Design’ Tab

Click the Second Circle of 6 mm, Third Circle of 3 mm and Fourth Circle of 6 mm holding:

Click the ‘Complete blending’ Green Check

Ctrl

Section 1.6 – Blend Tool

18 of 86

Repeat Steps 21-23 but from Firth to Fourth Circle (In that order)

Section 1.7 – Pull Tool 2

19 of 86

Click Select in the ‘Design’ Tab

Open ‘Named Selection’

Click the First Circle, Add a new Named Selection (Red Circle) and Change the name to ‘inlet’

‘inlet’

Velocity Inlet

Section 1.8 – Named Selections

20 of 86

Repeat Step 30 for the following surface:

‘wall.1’

Pre-stenotic wall

Section 1.8 – Named Selections

21 of 86

Repeat Step 30 for the following surface:

‘wall.2’

Post-stenotic wall

Section 1.8 – Named Selections

22 of 86

Repeat Step 30 for the following surface:

‘stenosis’

Stenosis’ wall

Section 1.8 – Named Selections

23 of 86

Repeat Step 30 for the following surface:

‘outlet’

Pressure Outlet

Section 1.8 – Named Selections

24 of 86

Make sure your Named Selections look like this:

If Yes, save your CAD model in your desired folder

Congratulations, your CAD model is completed!

End

Section 1.8 – Named Selections

25 of 86

Section 2 – CFD Simulation with Ansys Fluent Software

Meshing:

Local Sizing and Evaluate Mesh Quality.

Solver:

Laminar Model, Boundary Conditions, non-Newtonian Approximations.

26 of 86

Make sure ‘Meshing’ is selected

Toggle Double Precision

Meshing Processes → 2 or more

Solver Processes → 2 or more

Press ‘Start’!

Mesh

Section 2.0 – Launching Ansys Fluent Software

27 of 86

Successful Launch

Section 2.0 – Launching Ansys Fluent Software

28 of 86

Use Local Sizing: “Proximity" on the stenosis and post-stenotic walls. Cells per gap:

‘wall.2’ – Post-Stenotic Region: 15-20 cells per gap
‘stenosis’ – Throat Region: 15-20 cells per gap

Reasoning: These areas experience complex flow behaviors – high-velocity jets, recirculation zones, and potential turbulence. Boost convergence stability 15-20 Cells per gap ensures sufficient detail capturing. Since 20 cells in a gap of 3 mm and 6 mm will produce elements of approximately 0.15 mm and 0.30 mm, respectively. Why not 50? Mesh count scales approximately n³ in 3D, increasing total cell count by approximately (50/20) ³ = 15.6 times!

Refine Boundary Layers for capturing Wall Shear Stresses, and near-wall flow physics:

Layers: 5-10
Growth rate: 1.08

Reasoning: We want accurate near-wall flow modeling.

Section 2.1 – Mesh Specifications

29 of 86

Select Watertight Geometry

Import the Geometry:

Browse the geometry (Red Circle)

Section 2.2 – Mesh

30 of 86

Successful CAD import

Section 2.3 – Mesh Generation

31 of 86

Add local Sizing at the Throat ‘stenosis’

Change Size Control Type to ‘Proximity’,

And Cells Per Gap to ’20’

Click ‘Add local Sizing’ and make sure it displays at the workflow tree as shown below

Set Local sizing to ‘yes’ and follow the steps:

Section 2.3 – Mesh Generation

32 of 86

Add local Sizing at the post-stenotic region ‘wall.2’

Change Size Control Type to ‘Proximity’,

And Cells Per Gap to ’20’

Click ‘Add local Sizing’ and make sure it displays at the workflow tree as shown below

Section 2.3 – Mesh Generation

33 of 86

Generate the Surface Mesh using default values, by clicking ‘Generate the Surface Mesh

Check Surface Mesh Quality in the Console: Maximum Skewness: 0.47 (Good)

Section 2.3 – Mesh Generation

34 of 86

Successful Surface Mesh Generation

Section 2.3 – Mesh Generation

35 of 86

Describe the geometry:

Change Geometry type to ‘The geometry consists of only fluid regions with no voids’ and Click ‘Describe Geometry’
And ‘Change all fluid-fluid boundary types from ‘wall’ to ‘internal’ to ‘Yes’ to allow fluid to flow freely between all regions.

Section 2.3 – Mesh Generation

36 of 86

Update Boundaries:

Make sure the Boundary Types look like the picture below and Click ‘Update Boundaries’

Section 2.3 – Mesh Generation

37 of 86

Update Region:

Make sure the Region Types look like the picture below and Click ‘Update Regions’

Section 2.3 – Mesh Generation

38 of 86

Add Boundary Layers:

Change ‘Number of Layers’ to 5 and Click ‘Add Boundary Layers’

Section 2.3 – Mesh Generation

39 of 86

Generate the Volume Mesh:

Keep the default values and Click ‘Generate the Volume Mesh

End

Section 2.3 – Mesh Generation

40 of 86

Successful Volume Mesh Generation

Section 2.4 – Volume Mesh

41 of 86

Local Sizing Results using Polyhedral Mesh Elements (Default Value)

@ Stenosis ‘Throat’

Local Sizing ‘Proximity’

@ Inlet & wall.1

No Local Sizing

@ Outlet & wall.2

Local Sizing ‘Proximity

Section 2.4 – Volume Mesh

42 of 86

The mesh consists of a network of cells and nodes of various shapes and sizes. These cells serve as discrete control volumes where the governing Partial Differential Equations (PDEs) are solved to approximate the flow solution.

Meshing often presents a trade-off between accuracy and computational cost. A finer mesh provides more accurate results but requires more computational resources.

So, how can we make sure our mesh will provide accurate result while maintaining computational low. Keeping both time of simulation and mesh elements low?

Evaluating Aspect Ratio, Skewness and Orthogonality of the mesh elements, a conclusion can be made regarding the mesh capabilities to produces accurate results.

To expand further, a description of these parameters is provided, including their acceptable ranges and methods for obtaining these values within the Ansys Fluent software.

For more learning on Watertight Geometry workflow in Ansys Fluent Software

Section 2.5 – Mesh Quality Check

43 of 86

Aspect Ratio: Aspect ratio in mesh quality refers to the ratio of the longest edge to the shortest edge of a mesh element.

Skewness: Skewness in mesh quality refers to the deviation of a mesh element from an ideal shape. For example, in a 2D mesh, an ideal shape might be an equilateral triangle or a square.

Orthogonality: Orthogonality in mesh quality refers to the measure of how perpendicular the mesh elements are to each other.

Skewness of 0.00

Skewness near 1.00

Skewness of 0.50

Aspect Ratio of 1.00

Aspect Ratio >> 1

A = B

A >> B

Orthogonality of 1.00

Centroid to Centroid

‘ ’

Vector Perpendicular to shared cell face aligns with Centroid to Centroid line

Section 2.5 – Mesh Quality Check

44 of 86

Orthogonality	Range
Excellent	0.95 - 1.00
Very Good	0.70 - 0.95
Good	0.20 - 0.70
Poor	0.10 - 0.20
Very Poor	0.00 - 0.10

Skewness	Range
Excellent	0.00 - 0.25
Very Good	0.25 - 0.50
Good	0.50 - 0.80
Poor	0.80 - 0.95
Very Poor	0.95 - 1.00

Aspect Ratio	Range
Excellent	1 - 3
Very Good	3 - 5
Good	5 - 10
Acceptable	10 - 20
Very Poor	> 20

Aspect Ratio: Aspect ratio in mesh quality refers to the ratio of the longest edge to the shortest edge of a mesh element.

Skewness: Skewness in mesh quality refers to the deviation of a mesh element from an ideal shape. For example, in a 2D mesh, an ideal shape might be an equilateral triangle or a square.

Orthogonality: Orthogonality in mesh quality refers to the measure of how perpendicular the mesh elements are to each other.

Section 2.5 – Mesh Quality Check

45 of 86

Having established the criteria for a high-quality mesh, it is crucial to evaluate whether our mesh will accurately represent the underlying physics of the problem.

A thorough evaluation extends beyond simply examining quality metrics shown in the ‘console’.

So, in this section, you'll master the diagnostic tools in the Ansys Fluent tool that reveal the true quality of your mesh. We'll show you how to identify problematic elements and visualize exactly where they're located, empowering you to make informed decisions about mesh refinement. By learning these inspection techniques, you'll develop the critical skills to spot potential issues before they affect your simulation results and take precise corrective action only where necessary.

Since ‘Meshing’ is an art in itself, we recommend enrolling in the ‘Watertight Geometry Meshing in Ansys Fluent’ course for a deeper understanding of Ansys meshing tools.

Section 2.5 – Mesh Quality Check

46 of 86

As the first step, let's gather all mesh quality values for both the surface and volume mesh.

Surface mesh is usually inspected by looking at ‘skewness’. Previously, we collected this value from the console as 0.47.

The Surface Mesh will affect the Volume mesh as this elements propagate into the volume mesh. Meaning abrupt size transitions or highly skewed elements will generate low quality 3D mesh elements. Directly impacting the initial boundary of your volume mesh.

A perfect orthogonality means the angle between the line connecting cell centers and the face normal vector are parallel and therefore the reason we want to check for good skewness in the surface mesh.

Section 2.5 – Mesh Quality Check

47 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

There are two built in tools to collect data from the mesh quality and they can be found in the ribbon at the ‘Mesh’ sections:

Displays Mesh Quality Data in the ‘console’. For Example: Provides in the ‘console’ values such as Maximum Aspect Ratio

Displays Mesh Quality in the ‘window’. For Example: Locates and Highlights Minimum Orthogonality Elements within the mesh

Section 2.5 – Mesh Quality Check

48 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

Let's collect the ‘console’ data by clicking the arrow within ‘Check’ and click on ‘Perform Diagnostic Summary’

Check and Collect Mesh Quality Metrics from the ‘console’ on ‘Volume Diagnostics’

Check

Section 2.5 – Mesh Quality Check

49 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

From the values provided, we conclude:

Total Number of Cells is less that Student Edition limit: 119,087 < 500,000
Even the elements with the lowest 'Orthogonality Quality' fall within the 'Good' range: 0.30 < 0.61 < 0.70, confirming good mesh quality
The ‘Maximum Aspect Ratio’ falls within the 'Acceptable' range (10–20). However, further inspection is needed, as an Aspect Ratio averaging 5 or less is preferred for more complex flow structures

Output

Section 2.5 – Mesh Quality Check

50 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

Now, let's collect the ‘window’ data by clicking the arrow within ‘Quality’ and click on ‘Diagnostic Tools’

In comparison to previous tools, in this one we have the authority to pick which metric is displayed within the ‘window’.

Default measure is ‘Orthogonal’

Even though ‘Orthogonal’ quality has been proved to be ‘Good’ before let’s inspect where the ‘Minimum’ values are located

Section 2.5 – Mesh Quality Check

51 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

Close ‘Diagnostic Tool’, and in this case click on ‘Evaluate Volume Quality’

Section 2.5 – Mesh Quality Check

52 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

Output

This tool will provide: Maximum, Average and Minimum (poorest) Orthogonality.

For this case, the ‘console’ provides a list of 2 values: (0.61035289, 0.66035289). This are the elements with the poorest ‘Orthogonality’ in the mesh, and they are displayed in the window as Shown.

From this we conclude:

Orthogonal levels are ‘good’ across the mesh
Further refinement could be applied on the ‘stenosis’ region

Section 2.5 – Mesh Quality Check

53 of 86

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

Let’s go back to ‘Diagnostic tool’ and set the Measure as ‘Aspect Ratio’ for inspection and click ‘Draw’

‘window’ Output

‘console’ Output

End

Section 2.5 – Mesh Quality Check

54 of 86

Test: Find the location of mesh elements ranging

AR = (10-11.6343)

Hint: ‘Display’ → ‘Grid’ → ‘Select Quality’ → Metric?

Now, we need to collect the Volume Mesh Quality metrics by following these steps.

The ‘Histogram’ tool will provide:

A Quality (Aspect Ratio) vs Cell Numbers

From this graph we can see that a low number of elements exceed the 10 Aspect Ratio Mark. Which is ‘good’.

From the ‘console’ Output we can see that our mesh elements average an Aspect Ratio of 5.0759569 as we wanted

From this we conclude:

Further Refinement could be applied to reduce the maximum Aspect Ratio
Mesh is ready for the Solver

‘window’ Output

‘console’ Output

Section 2.5 – Mesh Quality Check

55 of 86

After checking our Mesh, and confirm we are ready to continue. We switch to the Solver by following the steps bellow

At the ribbon in section ‘Solution’, Click ‘Switch to Solution’

CFD

Confirm the Switch by Clicking ‘Yes’

Section 2.6 – Switch to Solver

56 of 86

Successful Solver Launch

Section 2.6 – Switch to Solver

57 of 86

A Transient Simulation will be used in this case since we will be studying the pulsatile nature of blood flow driven by cardiac cycles.

Boundary conditions are mathematical constraints applied at the of the computational domain to define how the flow behaves at these boundaries. Boundaries which we previously gave names (‘wall.1’, ‘wall.2’, ‘stenosis’, ‘inlet’ and ‘outlet’)

Boundary Conditions

Inlet(‘inlet’): Velocity inlet. Where we specify the velocity magnitude of the flow

Value:

During Systole: Sinusoidal waveform with 0.5 m/s peak velocities
During Diastole: Constant 0.1 m/s baseline flow

Outlet(‘outlet’): Pressure Outlet. Where we specify the static pressure

Value: 10,666-16,000 Pa (80-120 mmHg). Commonly seen in Adult Humans

Walls(‘wall.1’, ’stenosis’, ‘wall.2’)

No Slip condition: which describe how fluid behaves when it contacts a solid wall. Stating that fluid particles immediately adjacent to a solid have zero velocity relative to the boundary. (Amoo & Fagbenle, 2020)

Section 2.7 – Boundary Conditions Specifications

58 of 86

Section 2.8 – Viscous Model & Fluid Properties

59 of 86

Re in Normal Artery (D = 6 mm):

→ Laminar flow (since Re < 2300 for pipe flow)

Re in Stenosed Region (D = 3 mm):

Since flow continuity applies, velocity increases as the cross-sectional area decreases:

Now, calculating Re in the stenosis:

→ Laminar flow (since Re < 2300 for pipe flow)

Thus, the Carreau Model fits accordingly!

Section 2.9 – Flow Regime Verification

60 of 86

The Carreau Model is only available for laminar flow simulations in the Ansys Fluent tool, and this is because the model was developed specifically to capture the non-Newtonian, shear-thinning behavior of blood under low-to-moderate shear rates characteristics of laminar flow (Bodnar, Sequeira & Prosi, 2011). Whereas for turbulent flows, the dominant energy dissipation mechanism shift from viscous effects to eddy formation and dissipation, where non-Newtonian effects become less significant as high shear rates cause blood to behave more like a Newtonian fluid. But why?

At Low Shear Rates (low velocity gradients), red blood cells tend to aggregate and form rouleaux structures – stacks of cells resembling rolls of coins (Wagner, Steffen & Svetina, 2013). Increasing effective viscosity, and thus the thicker fluid behavior. Additionally, random orientations of such creates resistance to flow.
Whereas, for High Shear Rates (high velocity gradients), these aggregates break apart, and the deformable red blood cells gradually align with the flow direction (Bodnar, Sequeira & Prosi, 2011). Additionally, red blood cells gradually migrate towards the center of the vessel, where higher velocities are present. This cell partitioning creates distinct flow pathways where blood cells deform (elongate) and follow streamlined trajectories with minimal cross-stream interaction reducing effective viscosity

Section 2.10 – Viscous Model & Fluid Properties 2

61 of 86

Rouleaux Formation–to–Streamlining of Red Blood Cells

From Low–to–High Shear Rates

Velocity

Blood

Flow

High

Viscosity

Low

Viscosity

Rouleaux

Structure

Breakdown of Rouleaux

Streamlining

Section 2.10 – Viscous Model & Fluid Properties 2

62 of 86

In the ‘General’ Task Page. Set the ‘Time’ to ‘Transient’

Set the Viscous Model to Laminar by going on the ‘Setup’ tree and Click ‘Models’, ‘Viscous’, and ‘Laminar’ → ‘Ok’

Section 2.11 – Time & Viscous Model

63 of 86

Set the Material Properties by going on the ‘Setup’ tree and Click ‘Materials’, ‘Fluid ’, ‘air’ and follow the steps:

Section 2.12 – Fluid Properties

64 of 86

Set the Boundary Conditions by going on the ‘Setup’ tree and Click ‘Boundary Conditions’: Inlet(‘inlet’)

At the ‘Velocity Inlet’, Click the arrow at ‘Velocity Magnitude’ and select ‘expression and Click ‘f (x)’

Section 2.13 – Boundary Conditions

65 of 86

Copy and paste the function given within the yellow window as shown below. Refresh and Check the values are correct by setting a Min and Max, You can start with 0 [s] and 2 [s].

IF(mod({t},0.8[s])<=0.218[s], 0.5[m/s]*sin(4*PI*(mod({t},0.8[s])/1[s]+0.0160236)), 0.1[m/s])

Copy and Paste

Expression written by:

Chiyu Jiang, Cornell University

Modifications:

Cardiac Cycle Duration: 0.5 s → 0.8 s

UDF → Expression

Section 2.13 – Boundary Conditions

66 of 86

IF(mod({t},0.8[s])<=0.218[s], 0.5[m/s]*sin(4*PI*(mod({t},0.8[s])/1[s]+0.0160236)), 0.1[m/s])

Cardiac Cycle Definition: Total cycle duration: 0.8 seconds (75 BPM)

Systolic phase: First 0.218 seconds (27% of cycle)
Diastolic phase: Remaining 0.582 seconds (73% of cycle)

Flow Velocity Components: During systole: Sinusoidal waveform with 0.5 m/s peak velocity

During diastole: Constant 0.1 m/s baseline flow

Mathematical Structure

mod({t},0.8[s]): Creates a repeating time pattern every 0.8 seconds
IF( . . . <=0.218[s], . . . ): Separates systolic and diastolic phases
sin(4*PI*( . . . )): Generates a complete sine wave in the systolic period
+0.0160236: Phase shift, adjusting initial value of the sine wave

Section 2.14 – Velocity Inlet Expression Explained

67 of 86

Set the Boundary Conditions by going on the ‘Setup’ tree and Click ‘Boundary Conditions’: Outlet(‘outlet’)

Section 2.15 – Boundary Conditions 2

68 of 86

Set the Boundary Conditions by going on the ‘Setup’ tree and Click ‘Boundary Conditions’: Wall(‘wall.1’, ‘stenosis’ and ‘wall.2’)

Check both ‘wall.1’ and ‘wall.2’ for ‘No Slip’ Shear Condition

Section 2.15 – Boundary Conditions 2

69 of 86

Set the Boundary Conditions by going on the ‘Setup’ tree and Click ‘Solution’, ‘Initialization’. The Task Page will change, and select ‘Hybrid Initialization’ and Click ‘Initialize’

Hybrid Initialization provides a better starting point for complex flows, solving potential flow equations to create ‘more realistic’ initial values with respect to the geometry. Accounting for flow acceleration at stenosed, etc.

Section 2.16 – Initialization

Better initial velocity field: Unlike Standard initialization which uses constant values, Hybrid solves potential flow equations to create a more realistic initial velocity field that respects your geometry. For a stenosed vessel, this means the initialization already accounts for the flow acceleration in the narrowed region.

Faster convergence: By starting with a more physically realistic flow field, your simulation typically requires fewer iterations to reach convergence, saving computational time.

Improved stability: Complex geometries like stenoses create recirculation zones and high velocity gradients. Hybrid initialization better captures these features from the start, reducing the likelihood of divergence in early time steps of your transient simulation.

Better handling of pressure gradients: For a stenosed vessel, pressure gradients are significant. Hybrid initialization provides a more reasonable initial pressure field that accounts for these gradients, whereas Standard initialization would use a linear or constant pressure distribution.

Reduced initial transients: With pulsatile flow, you typically need to discard the first few cycles as the solution develops. Hybrid initialization often reduces these initial transients, potentially allowing you to reach a periodic state more quickly.

70 of 86

Now, we will create a XY-plane for the Post processing to inspect velocity contour mid plane

In ‘Setup’, Go to ‘Results’, and Right Click ‘Surfaces’, ‘New’ and Click on ‘Plane…’

Select ‘Method’ as ‘XY Plane’, and Click ‘Create’

Section 2.17 – Surfaces & Graphics

71 of 86

To generate the Velocity Contour, follow the steps:

In ‘Setup’, Go to ‘Results’, ‘Graphics’, and Click ‘Contours’, and follow ‘Change:’ steps:

Change:

Contour Name
Contours of
Deselect ‘Auto Range’
Set Min and Max Values
Select Plane in ‘Surfaces’
Save/Display

Section 2.17 – Surfaces & Graphics

72 of 86

Since we made our simulation in Transient, we want to generate an animation of the calculations for the 2 sec specified

In ‘Setup’, Go to ‘Solution’, ‘Calculation Activities’, and Click ‘Solution Animations’, and follow ‘Change:’ steps:

Change:

Name
‘Animation View’ to ‘front’
Select ‘Animation Object’
Ok

‘Preview’ shown in next slide

Section 2.18 – Animations

73 of 86

Preview of Animation

Section 2.18 – Animations

74 of 86

Change:

Create New Report Definition
Report Names
Field Variable
Select Outlet in ‘Surfaces’
OK

Now, we will create a XY-Plot for the Post processing to inspect Axial Static Pressure along x

In ‘Setup’, Go to ‘Solution’ at the Ribbon. Click on ‘Plot’, and follow ‘Change:’ steps:

Section 2.19 – Plots

75 of 86

Set the Boundary Conditions by going on the ‘Setup’ tree and Click ‘Solution’, ‘Run Calculation’. The Task Page will change, and

As we selected ‘Transient’ in ‘Time’. We are required to specify the number of Time Steps and its respective Size.

Time Step Size [s] of 0.01
Number of Time Steps

Section 2.20 – Run Calculations

76 of 86

Solution Converged ✔

Successful Simulation/Calculations

Section 2.20 – Run Calculations

77 of 86

Check the animation by going to ‘Setup’, ‘Results’, ‘Animations’ and Click on ‘Playback’. Select the ‘Animation Sequence’ and Click the play button

Section 2.21 – Animation Playback

78 of 86

Check the Animation!

Section 2.21 – Animation Playback

You can find the animation in Slide 82!

79 of 86

Check the Report!

End

Section 2.22 – Report Plot

80 of 86

/ Make a similar animation for Wall Shear Stress Contour vs Flow time

Wall Shear Stresses

Which is the tangential force exerted by blood on the vessel walls. Clinically, this may lead to rupture of the fibrous cap if mechanical stresses are large enough. Releasing plaque material and blood clots into the bloodstream in the case of atherosclerosis which may lead to heart attacks or strokes.

Notice any different Surfaces used?

Tip: To collect data for an animation that was not generated before running the calculations, you need to reinitialize the model and rerun the simulation after setting up the contour and animation.

Section 2.23 – Homework

81 of 86

Velocity Contour

The post-stenotic low-velocity region (depicted in blue) develops, and this region expands as the severity of the stenosis increases. In this area, mass transport is weak, and wall shear stress (WSS) is low, creating conditions that are highly prone to thrombosis in clinical settings. (Zhou, Lee & Wang, 2018)

The first 25 frames were used on the left, this accounts for the first

Of which the first 0.218 sec are the Systolic Phase.

Frame: 25

Frame: 1

Frame: 20

Frame: 15

Frame: 10

Frame: 5

Section 3 – Results

82 of 86

Section 3 – Results

Real–Time: 2 sec

Slowed by x4

Video–Time: 10 sec

83 of 86

Pressure @ Outlet Overtime

Section 3 – Results

84 of 86

Pressure @ Outlet Overtime

This plot shows the area-weighted average of absolute pressure at the outlet of your stenosed vessel over time, measuring approximately 111,990 Pa. This represents the combination of atmospheric pressure (101,325 Pa) and the specified outlet gauge pressure condition (10,666 Pa, equivalent to about 80 mmHg).

Key observations show:

Pulsatile pressure pattern: The graph shows clear periodic drops in pressure occurring at approximately 0.2s, 1.0s, and 1.8s, corresponding directly to your 0.8s cardiac cycle
Pressure drop magnitude: During each systolic phase, the pressure drops by approximately 3 Pa from the baseline.
Physiological correlation: Represents accurately how increased blood velocity during systole creates a localized pressure drop at the vessel outlet due to the Bernoulli effect and energy losses through the stenosis.
Quick pressure recovery: After each systolic phase, the pressure rapidly returns to baseline, which is consistent with the diastolic phase of your cardiac cycle

Section 3 – Results

85 of 86

Ansys Education Resources Feedback Survey

Here at Ansys, we rely on your feedback to ensure the educational content we create is up-to-date and fits your teaching needs.

Please click the link below to fill out a short survey (~7 minutes) to help us continue to support academics around the world utilizing Ansys tools in the classroom.

Feedback Survey Link

86 of 86

Use and Reproduction

The content used in this resource may only be used or reproduced for teaching purposes; and any commercial use is strictly prohibited.

Document Information

This lecture unit is part of a set of teaching resources to help introduce students to topics covering multiple physics areas.

Ansys Education Resources

To access more undergraduate education resources, including lecture presentations with notes, exercises with worked solutions, microprojects, real life examples and more, visit www.ansys.com/education-resources.

Feedback

If you notice any errors in this resource or need to get in contact with the authors, please email us at education@ansys.com