svMultiPhysics Simulation issues

[art-12-12-001]

I am unsure if anyone is experiencing the same issues as I am with running the new SimVascular version, specifically with the svMultiPhysics portion.

So I have already run multiple simulations with attempts to view the finished file in Paraview for post-processing. The issue is that the flow never seems to reach the outlet region. Specifically, I am simulating a model with two inlets merging into a single outlet, where both inlets have their own prescribed flows, and the outlet is a singular resistance value.

I have even attempted to re-simulate an old project I used with the older version of SimVascular, which used svSolver, that was successfully simulated, but when attempting it with svMultiPhysics, the same issue occurred, with the flow never converging and reaching the outlet.

I did notice that when I increased the number of time steps from 500 to 1000, both with the same time step size, the flow would spread just slightly more but still remain unconverged and within the region of the inlets. I have also attempted re-segmenting the model, reducing the resistance profile to 0, using flow files from SimVascular projects.

Below is my .xml file for the simulation:

<svMultiPhysicsFile version="1.0">

    <GeneralSimulationParameters>
        <Number_of_spatial_dimensions>3</Number_of_spatial_dimensions>
        
        <Number_of_time_steps>500</Number_of_time_steps>
        <Time_step_size>1e-3</Time_step_size>

        <Restart_file_name>results</Restart_file_name>
        <Increment_in_saving_restart_files>10</Increment_in_saving_restart_files>
        <Start_saving_after_time_step>1</Start_saving_after_time_step>
        <Continue_previous_simulation>false</Continue_previous_simulation>
        <Save_averaged_results>true</Save_averaged_results>
        <Save_results_to_VTK_format>true</Save_results_to_VTK_format>
        <Name_prefix_of_saved_VTK_files>results</Name_prefix_of_saved_VTK_files>
        <Increment_in_saving_VTK_files>10</Increment_in_saving_VTK_files>
        <Spectral_radius_of_infinite_time_step>0.20000000000000001</Spectral_radius_of_infinite_time_step>
        <Searched_file_name_to_trigger_stop>STOP_SIM</Searched_file_name_to_trigger_stop>
        <Simulation_requires_remeshing>false</Simulation_requires_remeshing>
        <Verbose>true</Verbose>
        <Warning>true</Warning>
        <Debug>false</Debug>
    </GeneralSimulationParameters>

    <Add_mesh name="remesh_new_0043-mesh-complete">
        <Mesh_file_path>remesh_new_0043-mesh-complete/mesh-complete.mesh.vtu</Mesh_file_path>
        <Add_face name="IVC_outlet">
            <Face_file_path>remesh_new_0043-mesh-complete/mesh-surfaces/IVC_outlet.vtp</Face_file_path>
        </Add_face>
        <Add_face name="left_inlet">
            <Face_file_path>remesh_new_0043-mesh-complete/mesh-surfaces/left_inlet.vtp</Face_file_path>
        </Add_face>
        <Add_face name="right_inlet">
            <Face_file_path>remesh_new_0043-mesh-complete/mesh-surfaces/right_inlet.vtp</Face_file_path>
        </Add_face>
        <Add_face name="vessel_wall">
            <Face_file_path>remesh_new_0043-mesh-complete/mesh-surfaces/vessel_wall.vtp</Face_file_path>
        </Add_face>
        <Domain>0</Domain>
    </Add_mesh>

    <Add_equation type="fluid">
        <Coupled>true</Coupled>
        <Min_iterations>1</Min_iterations>
        <Max_iterations>10</Max_iterations>
        <Tolerance>1e-4</Tolerance>
        <Backflow_stabilization_coefficient>0.29999999999999999</Backflow_stabilization_coefficient>

        <Density>1</Density>
        <Viscosity model="Constant">
            <Value>0.040000000000000001</Value>
        </Viscosity>

        <LS type="GMRES">
            <Max_iterations>10</Max_iterations>
            <Tolerance>1e-4</Tolerance>
            <Krylov_space_dimension>50</Krylov_space_dimension>
            <Linear_algebra type="fsils">
                <Preconditioner>fsils</Preconditioner>
            </Linear_algebra>
        </LS>

        <Output type="Spatial">
            <Velocity>true</Velocity>
            <Pressure>true</Pressure>
            <WSS>true</WSS>
        </Output>

        <Add_BC name="IVC_outlet">
            <Type>Neumann</Type>
            <Time_dependence>Resistance</Time_dependence>
            <Value>342</Value>
            <Profile>Flat</Profile>
        </Add_BC>

        <Add_BC name="left_inlet">
            <Type>Dirichlet</Type>
            <Time_dependence>Unsteady</Time_dependence>
            <Temporal_values_file_path>steady_left_iliac.flow</Temporal_values_file_path>
            <Profile>Flat</Profile>
            <Zero_out_perimeter>true</Zero_out_perimeter>
            <Impose_flux>true</Impose_flux>
        </Add_BC>

        <Add_BC name="right_inlet">
            <Type>Dirichlet</Type>
            <Time_dependence>Unsteady</Time_dependence>
            <Temporal_values_file_path>steady_right_iliac.flow</Temporal_values_file_path>
            <Profile>Flat</Profile>
            <Zero_out_perimeter>true</Zero_out_perimeter>
            <Impose_flux>true</Impose_flux>
        </Add_BC>

    </Add_equation>
</svMultiPhysicsFile>

[ktbolt]

@art-12-12-001 You do not have a boundary condition for the vessel_wall face.

Are the linear and nonlinear solves converging ? For fluid simulations we typically use <LS type="NS" >

[art-12-12-001]

@ktbolt Yes, both the linear and nonlinear iterations are converging. The histor.dat file shows that the nonlinear residual converges after 4 iterations, and the linear solve shows a ~30–40 iterations with a residual drop off of -90dB.
I redid the simulation with the vessel_wall having a Dirichlet BC, and it seems to fix my issue. Since the previous svSolver didn't require setting the wall BC, I assumed it would be the same for svMultiPhysics. I appreciate the help.

[ktbolt]

@art-12-12-001 There are indeed some important differences using svSolver and svMultiPhysics. Be sure to look at the svMultiPhysics tests for guidance although the tolerances used there are much too small.