Computational Fluid Dynamics Simulations of Blood Flow in a Cerebral Aneurysm

A precursor to the tutorial is the creation of a patient-specific vasculature model. In this demonstration, the tools Materialise Mimics, 3D Systems Geomagic Design X, and Altair HyperMesh were used to generate a tetrahedral volume mesh from MRA data.

1. Generate vessel centerlines for the model

1. Open the vmtk-launcher python GUI. In the PypePad, type: vmtkcenterlines -ifile [STL file saved to desktop].stl -ofile [STL name]centerlines.vtp
2. Select Run, Run all to load the data into the program. A new window will open that displays instructions and a rendering of the input model. Rotate the model and place the curser on each inlet location. Press the spacebar to place a seed.
3. After placing seeds on all of the inlets, press 'Q' to continue. Repeat the same placement of seeds for all outlets. After placing the outlet seeds, press 'Q' again and let the program run. This will save the centerline file to the desktop.

2. Data set-up in visualization software

1. Start the open-source visualization tool, ParaView (version 5.4.1 used in this procedure).
2. Select File, Open…, and locate the previously created files: the patient-specific volume mesh, centerline file(s), and the EnSight.case file(s). After clicking Ok, all data should be loaded into the interface.
3. From the bottom-left Properties table, select Apply. This command will load and read all the information a user has loaded or changed in ParaView. Highlight the volume mesh by clicking on its name within the Pipeline Browser to activate this selection.
4. Again, in the Properties table, scroll and change the Opacity value to somewhere between 0.2 - 0.5. Now, the centerlines and geometry renderings should be visible.

3. Remap 4D Flow MRI data with the volumetric mesh-grid and delete noise

1. From the top menu, select Filters, Alphabetical, ResampleWithDataset. A new window will open. Set the Source as the volume mesh and the Input as the EnSight.case file. Select Ok once these are set.
2. In the Properties table, select Apply to apply the filter.
3. As before, highlight the new ResampleWithDataset# name to activate it. Reduce the opacity of this new rendering as mentioned previously. In addition, change the centerline(s) from Surface to Points in the top menu.

4. Determine inlet and outlet flow boundary conditions

1. On the right side of the interface, next to maximize and minimize rendering options, select the Create View tool (square with vertical line). Select the SpreadSheet View option.
2. From the Showing dropdown box, select the centerline file(s). Only one type of file can be selected at a time. Cycle through the data, selecting various points to identify a location within each inlet and outlet.
3. Now, use the SpreadSheet View underneath Points to calculate the normal vector between two points near the same locations found in (4.2).
4. After finding the normal vector for each inlet and outlet locations, select Filters, Alphabetical, Slice. Make sure to activate the ResampleWithDataset# beforehand.
5. The Slice filter needs to appear beneath a new branch coming from ResampleWithDataset#. In the Properties table, set the plane Origin as the same XYZ point location for one of the two points used to calculate the normal vector. Use the normal vector from (4.3) to fill out the Normal values. Select Apply.
6. Highlight/activate the Slice# filter just created, and select Filters, Alphabetical, Surface Flow, and then Apply. Activate the new SurfaceFlow# item in the Pipeline Browser, and apply the Filters, Alphabetical, Group Time Steps, Apply.
7. In SpreadSheet View, open the GroupTimeSteps# data. Export this data to Microsoft Excel through copy and paste or use Export Spreadsheet.
8. In Excel, calculate the weighted values corresponding to the ratio of the flow rate at each outlet to the total inlet flow rate. Due to inherent noise and error of the 4D Flow MRI data, identify the smallest (generally having less reliable data) vessel to leave "open" to ensure the conservation of mass.
9. In CFD simulation software, transient flow waveforms are imported using read-transient-tables command; therefore, save the inlet flow data in a compatible, .txt format described in the online tutorials.

5. Set-up CFD simulations

1. Open CFD simulation software. Here we use ANSYS Fluent (version 18.1 described in this procedure as default). Choose File, Read, and Case…, and open the volume mesh .cas file used previously in ParaView. Display the mesh (this procedure uses a .cas file generated with Altair HyperMesh) by selecting Display…, Display.
2. It is importnat to scale the geometry to ensure the correct physical size of the model. Select Scale… and apply whatever unit conversion is necessary for the specific case then Close.
3. Select Materials, Create/Edit  to enter the material properties for blood. This tutorial uses physiologically relevant values of 1060 kg/s and 0.0035 kg/ms for density and viscosity, respectively.
4. Set the transient flow Boundary Conditions by prescribing either mass flow or velocity flow rates as a function of time for each inlet. Use the waveforms obtained from 4D Flow MRI measurement to prescribe the inlet boundary conditions. Outlets are given weighted values found in (4.8).
5. Under Solution, Methods, set the numerical schemes used for spatial and temporal discretization of the Navier-Stokes equations. For this procedure, use Coupled, which enables full pressure-velocity coupling, Least Squares Cell Based (gradient), Second Order scheme for pressure, Third-Order MUSCL scheme for momentum equations, and Second Order Implicit scheme for discretization in time. Ensure that the Time parameter in the top left has been set to Transient.
6. Under Solution, Initialization, select Standard Initialization. With all Initial Values set to 0, select Initialize. Now the program is set to run. Designate a solution folder to save results every Autosave Every (Time Steps) underneath Calculation Activities.
7. In the final steps, set-up the Time Step Size(s) under Run Calculation. Use the Excel boundary condition data in (4.7) to determine this value. Reducing the time step facilitates convergence and improves the accuracy of the numerical solution, while increasing the solution time. It is a good practice to run the simulation for at least three full cardiac cycles to eliminate the effect of the initial transients.
8. Finally, set Max Iterations for each time step between 300 - 500. The software will automatically stop the iterations at each time step once the convergence is reached and proceed to the following time step. The convergence can be improved by running a steady flow simulation with averaged velocity values and then using the results as the initial conditions for the pulsatile flow simulation. Select Calculate when ready to run the solver.
9. The software will run each iteration until convergence is achieved or Max Iterations causes the iteration to continue. The files will be automatically saved in the location from (5.5), and the solution data can be visualized in either ANSYS CFD-Post or ParaView software.