A Computational Fluid Dynamics Protocol for The Hemodynamic Analysis of a Microfluidic Model of Thrombosis

doi:10.21203/rs.3.pex-1411/v1

Method Article

A Computational Fluid Dynamics Protocol for The Hemodynamic Analysis of a Microfluidic Model of Thrombosis

https://doi.org/10.21203/rs.3.pex-1411/v1

This work is licensed under a CC BY 4.0 License

This protocol has been posted on Protocol Exchange, an open repository of community-contributed protocols sponsored by Nature Portfolio. These protocols are posted directly on the Protocol Exchange by authors and are made freely available to the scientific community for use and comment.

Version 1

posted

You are reading this latest protocol version

Thrombosis is both attributed to biochemical agonists and mechanical stresses applied to platelets. Whilst the effect of biochemical agonists has been extensively studied, the mechanosensitive factors remain poorly defined. Stenotic microfluidic channels mimic the narrowing vessels, providing the real-time observation of platelets under disturbed flow. Though the experimental analysis of platelets in disturbed flow confirms the mechanosensitive behavior of platelets, it cannot explicate detailed thresholds for platelet activation. Computational Fluid Dynamics (CFD) could be utilized alongside experimental analysis to characterize thresholds for platelet behavior under imposed shear stress. CFD simulations, however, are prone to uncertainties and errors which should be minimized to obtain compelling results. Hereby, we have presented a CFD protocol for researchers in the field of microfluidic and hemodynamic studies.

Computational biology and bioinformatics

Hemodynamic

Stenosis

Thrombosis

Computational fluid dynamics

Microfluidic

Computational Fluid Dynamics (CFD) harnesses mathematics and computer science to analyze fluid flow related problems. It is a powerful tool applied to various fields of research including battery optimization¹, heat transfer², pipe and valve design^3,4, electronic cooling⁵, meso-scale air pollution models⁶, food industry⁷, and biology⁸. Recently, CFD has been applied to simulate blood flow in microfluidic channels with embedded obstacles⁹. It represents the first step in revealing the hemodynamic profile within disturbed blood flow and allows it to be correlated with the results of real blood experiments, potentially revealing important information about the thrombotic response. In 2021, Zhao and Vatankhah et al. commenced work in this field, simulating blood flow within a stenotic microfluid device using ANSYS Fluent to investigate the effect of stenosis geometrical properties on blood flow¹⁰.

As commercially available CFD packages like ANSYS Fluent become increasingly accessible, hemodynamic researchers could benefit from applying them to their studies. However, such software can also generate coarse or even unrealistic results with inappropriate settings. To this end, this protocol aims to 1) help readers to replicate the studies completed in the paper by Zhao and Vatankhah et al; 2) aid the potential readers in better understanding of the results of CFD studies and 3) improve their CFD verification and validation skills.

ANSYS FLUENT version 2020 R1

Any version of ANSYS with the Fluent package included will suffice to carry out the following procedure. However, it is important to note that the following steps are specific to ANSYS 2020 R1.

In this research of stenosis microfluidic channels, the contractions were extensively investigated with particular focus on the shear rates and shear rate gradients present throughout the channel. This protocol will focus on replicating Figure 2A-D from the Zhao and Vatankhah et al paper¹⁰ (Fig. 1).

Establishing Geometry

To start with, open ANSYS workbench and drag the Fluent flow (FLUENT) module into the project window. The geometry setup would appear on the first row. Right click the Geometry tab and select Design Modeler. It is recommended to select “micrometer” as the default unit from unit tab before drawing the structure. Note the units cannot be altered after drawing commences. Pick the desired work plane and create a new sketch on it. The initial drawing should be completed in two dimensions (Fig. 2). The different channels utilized in the Zhao and Vatankhah et al paper¹⁰ can be modelled accordingly. Note that the fillet radius R5 is 5 µm in all cases. After completing the two-dimensional drawing, click Extrude to generate the three-dimensional concentric or eccentric stenosis model microfluidic channel.

Applying Mesh

In this step, the size and method of meshing are altered using the left-hand panel. To obtain the most accurate results, it is suggested to generate a relatively fine mesh that can still be constructed in a reasonable amount of time, this will vary based on the users’ PC specifications. An unnecessarily dense mesh will waste computational resources and prolong the calculation time. To this end, a delicate balance should be struck between the fineness and computational power usage. Notably, the region of interest shall be further refined, together with the complex areas where the flows would not simply be straight. In bulk regions with consistent flow, the coarse mesh can be used to save computational power.

For instance, the stenosis model appearing in Zhao and Vatankhah et al paper¹⁰ is generated by employing a general mesh size of 1.5 microns initially for the entire geometry using the hexahedral method. This general grid sizing is then refined and reduced in regions of increased flow complexity as demonstrated by the finer grid size on the curved faces of the model (Fig. 3). This finer sizing can be achieved by adding extra mesh size modules on faces or edges. For the stenosis channel, a “face sizing” module is applied on the stenosis area to reduce the mesh size to 0.4 microns. Using a 32 threads computer, this simulation had a computation time of 180 minutes. Once the mesh has been established, update the generated model to the ANSYS workbench before exiting the meshing software.

Adjusting Setup and Running Solution

Prior to entering the next step, it is important to ensure that double precision is being employed and that the correct number of solver processes for the CPU are being used. These can be modified by right clicking on setup and choosing “edit”.

Double click the “setting” tab in ANSYS workbench to open Fluent. Set the flow to be laminar from the left “Models” panel. Note in most microfluidic channels, the flow can safely be assumed to be laminar because of the low Reynolds number of the flow. Set the correct fluid medium by entering its density and viscosity. Note that common fluid, such as water, can be chosen from the ANSYS database directly. Table 2 of the main paper presents the density and viscosity values appropriate for each fluid. Having created the correct material the fluid in “Cell zone conditions” is set to be the material of the model (blood or water).

Boundary conditions should be defined on the previously named selections. For instance, the main paper defined mass flow rate at the outlet, which should be calculated using the equations in the main paper and entered into ANSYS outlet boundary condition. A zero-pressure inlet should be selected in this scenario. Conversely, when suing a “velocity inlet” or “mass flow inlet”, the outlet should be set as a zero-pressure. As such, if error messages appear when attempting to run the simulation, it is advisable to first check the boundary condition settings.

The residuals under the “monitors” tab should all be set to a convergence criterion of 1e-6 (Fig. 4A) before initializing the solution using the Hybrid Initialization method (Fig. 4B). In the “calculation” tab, the iteration steps should be set as a large number e.g., 5,000, to ensure that the simulation has sufficient opportunity to converge (Fig. 4C). Select the parameters of interest from “data file quantities” under the “calculation” tab. For the purposes of the Zhao and Vatankhah et al paper¹⁰, the strain rate was added (Fig. 4D). The simulation will automatically stop running when the solution converges, and all residuals are below the value of 1e-6. Another calculation is optional if the convergence criteria are not achieved after the first set of iterations are complete. The user should know whether their solution is likely to successfully converge after the first few hundred iterations as the graph of the residuals should display a decreasing trend (Fig. 5). In most cases, a smooth convergence of residuals indicates the simulation settings are properly implemented.

Attaining Results

Double click “Results” in ANSYS workbench to open CFD-Post. The top menu provides options to add contour plots, streamlines & volume renderings. The detailed settings for generating Figure 1 are described below.

The WSS contour on the walls can be plotted by clicking the “Insert” tab. In the pop up window, choose “wall shear stress” as the variable and “wall” as the location (Fig. 1A). To find a streamline passing through a certain point, define the point first by clicking on “Location” in the top menu bar and selecting “points”. Enter the location values x = 0, y = 80, z = 30. Then go to “Insert” > “streamline” and select the previous defined point as the starting location. Select the direction of the streamlines as “Forward and Backward”. In the color tab, select strain rate as the variable to be plotted by the color of the streamline (Fig. 1B).

To export data, click on the top menu and go to “File” > “Export”. Choose the previous streamline as the location, strain rate as the first variable and WSS as the second variable. Save the exported data to the desired location and plot them using other software (Fig 1C and D). It is worth noting that the strain rate gradient needs to be created by the user. First create an expression which calculates the dot product of the velocity and strain rate gradient vectors. For instance, “dot = (Strain Rate.Gradient X*Velocity u+Strain Rate.Gradient Y*Velocity v+Strain Rate.Gradient Z*Velocity w)”. Then divide the dot product by the velocity magnitude, such as “dot/Velocity”. Create a variable which has the value of the expression just created above and export data as aforementioned (Fig. 1D).

As an iterative method, CFD simulation generates a sequence of approximate values to converge to the exact solution. To this end, the verification and validation analysis are essential for CFD approaches.

Convergence criteria verification

The iterative procedure is considered completed when the residuals, the root mean square error of approximation between two successive iterations, of the governing equations is less than a certain threshold, defined as the “convergence criteria”^10,11. To ensure that the results obtained from the CFD analysis are independent to the applied convergence criteria, at least three simulations should be performed with different convergence criteria to confirm that the results are not dependent on the imposed convergence criteria. There is no certain rule to pre-assume the threshold. However, the convergence criteria that ensures the solution does not vary from the point required for laminar flow simulations within microfluidic devices is typically between 10^-6and 10^-7.

Grid sensitivity analysis

In CFD analysis, the domain of interest should be discretized into computational cells. Within each cell, the conservation laws of physics should be satisfied, where the mass of flow shall be conserved, and the rate of change of momentum should match the sum of forces applied to the cell¹². Therefore, the final solution would depend on the grid applied to the computational domain. Three simulations with three different grids should be carried out to indicate that the solution is not dependent to the selected grid. Note that the number of elements for each grid shall be significantly differentiable. For instance, the main paper increases 100% of element from medium and fine meshing grid. Importantly, the error between each grid should be less than 5%. At last, it is recommended that the convergence criteria analysis would be performed on the finest grid; a rule of thumb, the finest grid usually needs more iterations to converge.

Validation analysis

The CFD results shall be compared with available resources, e.g., analytical, computational, or experimental studies.

Using a 32 threads computer, this simulation had a computation time of 180 minutes.

1 Bortolin, S., Toninelli, P., Maggiolo, D., Guarnieri, M. & Del Col, D. in Journal of Physics: Conference Series. 012049 (IOP Publishing).

2 Hajabdollahi, H., Tahani, M. & Fard, M. S. CFD modeling and multi-objective optimization of compact heat exchanger using CAN method. Applied thermal engineering 31, 2597-2604 (2011).

3 Kulkarni, A., Roy, S. S. & Joshi, J. Pressure and flow distribution in pipe and ring spargers: Experimental measurements and CFD simulation. Chemical Engineering Journal 133, 173-186 (2007).

4 Li, X. G., Xu, S. M. & Li, H. CFD simulation of hydrodynamics of valve tray. Chemical Engineering and Processing: Process Intensification 48, 145-151 (2009).

5 Arularasan, R. & Velraj, R. CFD analysis in a heat sink for cooling of electronic devices. International Journal of the computer, the internet and management 16, 1-11 (2008).

6 Kadaverugu, R., Sharma, A., Matli, C. & Biniwale, R. High resolution urban air quality modeling by coupling CFD and mesoscale models: A review. Asia-Pacific Journal of Atmospheric Sciences 55, 539-556 (2019).

7 Xia, B. & Sun, D.-W. Applications of computational fluid dynamics (CFD) in the food industry: a review. Computers and electronics in agriculture 34, 5-24 (2002).

8 Yin, Y., Choi, J., Hoffman, E. A., Tawhai, M. H. & Lin, C.-L. Simulation of pulmonary air flow with a subject-specific boundary condition. Journal of biomechanics 43, 2159-2163 (2010).

9 Shahcheraghi, N., Dwyer, H., Cheer, A., Barakat, A. & Rutaganira, T. Unsteady and three-dimensional simulation of blood flow in the human aortic arch. J. Biomech. Eng. 124, 378-387 (2002).

10 Zhao, Y. C. et al. Hemodynamic analysis for stenosis microfluidic model of thrombosis with refined computational fluid dynamics simulation. Sci Rep 11, 6875, doi:10.1038/s41598-021-86310-2 (2021).

11 Zhao, Y. C. et al. Computational Fluid Dynamics Simulations at Micro-Scale Stenosis for Microfluidic Thrombosis Model Characterization. Molecular & Cellular Biomechanics 18, 1-10, doi:10.32604/mcb.2021.012598 (2021).

12 Versteeg, H. & Malalasekera, W. Computational fluid dynamics. The finite volume method, 1-26 (1995).

We thank Young No and Jacky He for help with the discussion, Xiaoying Li for help with figure improvement and Sydney Manufacturing Hub, Research and Prototype Foundry, Gregg Suaning, Nadia Court and Kevin Doan for support of our lab startup. This work was supported by Australian Research Council Discovery Project (DP200101970 – L.A.J. and Z.L.), NSW Cardiovascular Capacity Building Program (Early-Mid Career Researcher Grant – L.A.J.) and Sydney Research Accelerator prize (SOAR – L.A.J.), The University of Sydney Faculty of Engineering Startup Fund and Major Equipment Scheme (L.A.J.). Lining Arnold Ju is an Australian Research Council DECRA fellow (DE190100609), an honorary National Heart Foundation Future Leader fellow (102532), Faculty of Engineering Dean’s Research Award 2020 recipient.

Download PDF

Version 1

posted

You are reading this latest protocol version

A Computational Fluid Dynamics Protocol for The Hemodynamic Analysis of a Microfluidic Model of Thrombosis

Status:

Version 1

Abstract

Figures

Introduction

Equipment

Procedure

Troubleshooting

Time Taken

References

Acknowledgements

Associated Publications

Status:

Version 1

Privacy Policy

Terms of Service

A Computational Fluid Dynamics Protocol for The Hemodynamic Analysis of a Microfluidic Model of Thrombosis

Status:

Version 1

Abstract

Figures

Introduction

Equipment

Procedure

Troubleshooting

Time Taken

References

Acknowledgements

Associated Publications

Status:

Version 1

Privacy Policy

Terms of Service

Manage Cookie Preferences