Static Fluid-Structure Interaction (FSI) via Python-wrapper

Written by for Version Revised by Revision date Revised version
@rsanfer 7.0.3 @rsanfer 2020-03-04 7.0.3
At one glance:
pysu2 library
User Guide:
Build SU2 on Linux/MacOS
Static Fluid-Structure Interaction (FSI)


This tutorial uses SU2’s python wrapper and its native solvers for incompressible flow and solid mechanics to solve a steady-state Fluid-Structure Interaction problem. This document will cover:

  • Setting up a python script to run SU2
  • Extracting flow loads and structural displacements from two different python instances of SU2
  • Coupling the two instances

In this tutorial, we will solve the exact same problem as for the Static FSI tutorial. Please take a moment to familiarize yourself with that tutorial in case you haven’t yet.


You can find the resources for this tutorial in the folder python_fsi of the Tutorials repository. There is a python script and two sub-config files for the flow and structural subproblems.

Moreover, you will need two mesh files for the flow domain and the cantilever.


For this tutorial, you will need to use advanced features of SU2, in particular the python-wrapped version of the code which needs to be built from source.

This tutorial has been tested on a linux system with the following specs

Linux kernel 5.3.18-1-MANJARO
GCC compilers version 9.2.0
Open MPI version 4.0.2
Python version 3.8.1
SWIG version 4.0.1

compiling the code from source using the following meson settings

./ build -Dwith-mpi=enabled -Denable-autodiff=true -Denable-pywrapper=true

It requires an adequate setup of the system and a correct linkage of both the mpi4py and swig libraries. For questions, updates, or notes on the usability of this tutorials on different systems or configurations, please use the comment section below.

Mesh Description

The cantilever is discretized using 1000 4-node quad elements with linear interpolation. The fluid domain is discretized using a finite volume mesh with 7912 nodes and 15292 triangular volumes. The wet interface is matching between the fluid and structural domains.

Configuration File Options

We reuse the flow and structural config files from the Static FSI, with only very minor modifications.

First of all, SU2 will see each instance as a single-zone problem. Therefore, it is necessary to set the output appropriately in order to prevent overwriting files. For the flow config

SOLUTION_FILENAME = solution_fsi_steady_0
RESTART_FILENAME = restart_fsi_steady_0
VOLUME_FILENAME = fsi_steady_0

and for the structural config

SOLUTION_FILENAME = solution_fsi_steady_1
RESTART_FILENAME = restart_fsi_steady_1
VOLUME_FILENAME = fsi_steady_1

Next, we choose the output that we require to the history files. In this tutorial, we are interested on the drag coefficient of the cantilever once deformed. Therefore, for the flow config, we need to include the AERO_COEFF

CONV_FILENAME= history_0

while for the structural config it’s enough with the residuals

CONV_FILENAME= history_1

Finally, it is necessary to indicate the structural solver that the boundary solution will be used to update a fluid field. This is done by setting the config options

MARKER_FLUID_LOAD = ( feabound )
MARKER_DEFORM_MESH = ( feabound )

on the structural config file.

Applying coupling conditions to the individual domains

The key part of this tutorial is the python script to run the FSI problem. Please take a moment to evaluate its contents, as we will go through some of its most important aspects.

First, we will need to import the SU2 python library along with mpi4py, using

import pysu2
from mpi4py import MPI

We define the names of the config files required by SU2 using

flow_filename = "config_channel.cfg"
fea_filename = "config_cantilever.cfg"

We will exemplify the initialization of SU2 using the flow domain. First, we create a driver object using

FlowDriver = pysu2.CSinglezoneDriver(flow_filename, 1, comm);

which is analogous to the SU2 driver in the C++ executable. We use a comm that is imported from mpi4py


and the flow_filename previously defined. The 1 corresponds to the number of zones (remember, we consider each instance of SU2 to be independent).

Next, we need to identify the FSI boundary. We retrieve the list of all the flow boundary tags and their associated indices using

FlowMarkerList = FlowDriver.GetAllBoundaryMarkersTag()
FlowMarkerIDs = FlowDriver.GetAllBoundaryMarkers()

For the boundary FlowMarkerName = 'flowbound', we identify the corresponding index

if FlowMarkerName in FlowMarkerList and FlowMarkerName in FlowMarkerIDs.keys():
  FlowMarkerID = FlowMarkerIDs[FlowMarkerName]

and, finally, the number of vertices on the boundary is

nVertex_Marker_Flow = FlowDriver.GetNumberVertices(FlowMarkerID)

An analogous process can be followed for the FSI boundary on the structural domain. In this case, the boundaries are matching, so the number of vertices is the same.

We start the FSI loop and limit it to the same number of iterations required for convergence in the Static FSI tutorial

for i in range(17):

First, the flow solution is run

  stopCalc = FlowDriver.Monitor(0)

and the flow loads are recovered using

  for j in range(nVertex_Marker_Flow):
    vertexLoad = FlowDriver.GetFlowLoad(FlowMarkerID, j)

The flow_loads array now contains the loads in all the vertices of the flow FSI interface. Now, we need to set the flow loads to the FEA nodes. By construction for this case, the vertex IDs are matching for both meshes except for vertex 0 and 1, which are inverted. Therefore, we set the flow loads on the structural domain using

  for j in range(2, nVertex_Marker_FEA):

You can ensure the vertices are coincidental by the coordinates of the nodes using FlowDriver.GetVertexCoordX(FlowMarkerID, iVertex) and FlowDriver.GetVertexCoordY(FlowMarkerID, iVertex) for the flow domain, and FEADriver.GetVertexCoordX(FEAMarkerID, iVertex) and FEADriver.GetVertexCoordY(FEAMarkerID, iVertex) for the structural domain.

Next, the structural simulation is run with

  stopCalc = FEADriver.Monitor(0)

and the structural displacements at the feabound interface are retrieved using

  for j in range(nVertex_Marker_FEA):
    vertexDisp = FEADriver.GetFEA_Displacements(FEAMarkerID, j)

Finally, these boundary displacements are imposed to the flow mesh

  for j in range(2, nVertex_Marker_FEA):

Once the loop is completed, it only remains to write the solution of each domain to file using


Running SU2

Follow the links provided to download the python script and the two sub-config files for the flow and structural subproblems.

Also, you will need the two mesh files for the flow domain and the cantilever.

Execute the code using Python

$ python

The convergence history of each individual domain will be printed to screen, starting with the flow domain

|  Inner_Iter|      rms[P]|      rms[U]|      rms[V]|
|           0|   -4.799717|  -19.870540|  -32.000000|
|          10|   -5.421646|   -4.859176|   -5.558343|
|          20|   -6.200459|   -5.584293|   -6.120761|
|          30|   -6.852188|   -6.205093|   -6.958953|
|          40|   -7.502751|   -6.854100|   -8.034484|
|          50|   -8.316190|   -7.662838|   -8.492639|
|          60|   -9.153994|   -8.509430|   -9.696622|
|          70|  -10.119472|   -9.498203|  -10.117162|
|          80|  -11.035958|  -10.448171|  -11.143732|
|          90|  -11.613994|  -10.982943|  -11.842820|
|         100|  -12.264740|  -11.616077|  -12.556728|
|         104|  -12.684964|  -12.046580|  -12.778620|

followed by the structural domain

|  Inner_Iter|      rms[U]|      rms[R]|      rms[E]|    VonMises|
|           0|   -1.121561|   -2.706864|   -4.419338|  2.2876e+03|
|           1|   -1.708123|    1.269382|   -1.716845|  2.2429e+03|
|           2|   -2.583705|    0.631041|   -3.175890|  2.2237e+03|
|           3|   -2.508726|   -0.795411|   -5.686295|  2.0701e+03|
|           4|   -2.751613|   -1.306797|   -6.550284|  2.0544e+03|
|           5|   -3.147799|   -1.271416|   -6.914834|  2.0364e+03|
|           6|   -2.962716|   -2.664273|   -7.800357|  2.0171e+03|
|           7|   -4.083257|   -2.080066|   -8.553973|  2.0155e+03|
|           8|   -4.522566|   -4.400710|  -11.005428|  2.0149e+03|
|           9|   -7.252524|   -5.240218|  -14.876499|  2.0149e+03|
|          10|  -10.834476|  -10.711888|  -23.634504|  2.0149e+03|

After 17 iterations, both the flow and structural fields will be successfully converged,

|  Inner_Iter|      rms[P]|      rms[U]|      rms[V]|
|           0|  -15.808168|  -15.358431|  -15.769282|
|          10|  -16.714759|  -16.074145|  -17.174991|

|  Inner_Iter|      rms[U]|      rms[R]|      rms[E]|    VonMises|
|           0|  -11.937375|  -11.637725|  -25.999458|  1.8531e+03|
|           1|  -15.794016|  -11.636749|  -28.541279|  1.8531e+03|
|           2|  -16.165350|  -11.621837|  -28.528692|  1.8531e+03|
|           3|  -16.056047|  -11.608302|  -28.544055|  1.8531e+03|
|           4|  -16.156344|  -11.627675|  -28.565975|  1.8531e+03|
|           5|  -16.204699|  -11.633976|  -28.581277|  1.8531e+03|

Which correspond to the exact same residuals as for the last iteration on the Static FSI tutorial. This can be tested by running the latter with


which yields for its last iteration

|                     Zone 0 (Incomp. Fluid)                     |
|  Outer_Iter|  Inner_Iter|      rms[P]|      rms[U]|      rms[V]|
|          16|           0|  -15.808168|  -15.358431|  -15.769282|
|          16|          10|  -16.714759|  -16.074145|  -17.174991|
|                              Zone 1 (Structure)                             |
|  Outer_Iter|  Inner_Iter|      rms[U]|      rms[R]|      rms[E]|    VonMises|
|          16|           0|  -11.937375|  -11.637725|  -25.999458|  1.8531e+03|
|          16|           1|  -15.794016|  -11.636749|  -28.541279|  1.8531e+03|
|          16|           2|  -16.165350|  -11.621837|  -28.528692|  1.8531e+03|
|          16|           3|  -16.056047|  -11.608302|  -28.544055|  1.8531e+03|
|          16|           4|  -16.156344|  -11.627675|  -28.565975|  1.8531e+03|
|          16|           5|  -16.204699|  -11.633976|  -28.581277|  1.8531e+03|
|                        Multizone Summary                       |
|  Outer_Iter| avg[bgs][0]| avg[bgs][1]|MinVolume[0]|DeformIter[0|
|          16|  -11.228939|   -9.130581|  8.7338e-10|          44|

The displacement field on the structural domain and the velocity field on the flow domain obtained in fsi_steady_1.vtu_and fsi_steady_0.vtu respectively are shown below:

FSI Results1

FSI Results2

which is, as expected, identical to the result of the Static FSI tutorial. The convergence of the drag coefficient is as follows:

FSI Results2

The drag coefficient will be used as the objective function for the adjoint computation in the next tutorial.


If you are using this content for your research, please kindly cite the following reference in your derived works:

Sanchez, R. et al. (2016), ASSESSMENT OF THE FLUID-STRUCTURE INTERACTION CAPABILITIES FOR AERONAUTICAL APPLICATIONS OF THE OPEN-SOURCE SOLVER SU2, Proceedings of the VII European Congress on Computational Methods in Applied Sciences and Engineering. DOI: 10.7712/100016.1903.6597

This work is licensed under a Creative Commons Attribution 4.0 International License
Creative Commons Licence

Improve this page