Upon completing this tutorial, the user will be familiar with performing a simulation of internal, inviscid flow through a 2-D geometry. The specific geometry chosen for the tutorial is a channel with a bump along the lower wall. Consequently, the following capabilities of SU2 will be showcased in this tutorial:
- Steady, 2-D Euler equations
- JST numerical scheme in space
- Euler implicit time integration
Inlet, Outlet, and Euler Wall boundary conditions
The intent of this tutorial is to introduce a simple, inviscid flow problem and to explain how boundary markers are used within SU2. This tutorial is especially useful for showing how an internal flow computation can be performed using the inlet and outlet boundary conditions.
The resources for this tutorial can be found in the directory TestCases/euler/channel/ . You will need the configuration file (inv_channel.cfg) and the mesh file (mesh_channel_256x128.su2).
The following tutorial will walk you through the steps required when solving for the flow through the channel using SU2. It is assumed you have already obtained and compiled SU2_CFD. If you have yet to complete these requirements, please see the Download and Installation pages.
This example uses a 2-D channel geometry which features a circular bump along the lower wall. It is meant to be a simple test in inviscid flow for the subsonic inlet and outlet boundary conditions that are required for an internal flow calculation. The geometry is based on an example in Chapter 11 of Numerical Computation of Internal and External Flows: The Fundamentals of Computational Fluid Dynamics (Second Edition) by Charles Hirsch.
This problem will solve the for the flow through the channel with these conditions:
- Inlet Stagnation Temperature = 288.6 K
- Inlet Stagnation Pressure = 102010.0 N/m2
- Inlet Flow Direction, unit vector (x,y,z) = (1.0, 0.0, 0.0)
- Outlet Static Pressure = 101300.0 N/m2
- Resulting Mach number = 0.1
- There is also a set of conditions resulting in transonic flow in the config file
The channel is of length 3L, height L, with a circular bump centered along the lower wall with height 0.1L. For the SU2 mesh, L = 1.0 was chosen, as seen in the figure of the mesh below. The mesh is structured (rectangles) with 256 nodes along the length of the channel and 128 nodes along the height. The following figure contains a view of the mesh (coarser mesh shown for clarity):
Figure (1): The computational mesh with boundary conditions highlighted.
The boundary conditions for the channel are also highlighted in the figure. Inlet, outlet, and Euler wall boundary conditions are used. The Euler wall boundary condition enforces flow tangency at the upper and lower walls. It is important to note that the subsonic inlet and outlet boundary conditions are based on characteristic information, meaning that only certain flow quantities can be specified at the inlet and outlet. In SU2, the stagnation temperature, stagnation pressure, and a unit vector describing the incoming flow direction must all be specified (the density and velocity, or mass flow, can aldo be specified). At an exit boundary, only the static pressure is required. These options are explained in further detail below under configuration file options. If there are multiple inlet or outlet boundaries for a problem, this information can be specified for each additional boundary by continuing the lists under MARKER_INLET or MARKER_OUTLET.
Configuration File Options
Several of the key configuration file options for this simulation are highlighted here. Please see the configuration file page for a general description of all options.
Here we explain some details on markers and boundary conditions:
The 4 different boundary markers (upper_wall, lower_wall, inlet, and outlet) are each given a specific type of boundary condition. For the inlet and outlet boundary conditions, the additional flow conditions are specified directly within the configuration option. The format for the inlet boundary condition is (marker name, inlet stagnation pressure, inlet stagnation pressure, x-component of flow direction, y-component of flow direction, z-component of flow direction) where the final three components make up a unit flow direction vector (magnitude = 1.0). In this problem, the flow is exactly aligned with the x-direction of the coordinate system, and thus the flow direction vector is (1.0, 0.0, 0.0). The outlet boundary format is (marker name, exit static pressure). Any boundary markers that are listed in the MARKER_PLOTTING option will be written into the surface solution file. Any surfaces on which an objective such as Cl or Cd is to be calculated must be included in the MARKER_MONITORING option.
Some integration options:
For this problem, Euler Implicit time integration with a CFL number of 6 is chosen. Convergence is also accelerated with three levels of multigrid. We will discuss some of these options in later tutorials.
Setting the convergence criteria:
There are three different types of criteria for terminating a simulation in SU2: running a specified number of iterations (EXT_ITER option), reducing the density residual by a specified order of magnitude, or by converging an objective, such as drag, to a certain tolerance. The most common convergence criteria is the RESIDUAL option which is used in this tutorial by setting the CONV_CRITERIA. The RESIDUAL_REDUCTION option controls how many orders of magnitude reduction in the density residual are required for convergence, and RESIDUAL_MINVAL sets the minimum value that the residual is allowed to reach before automatically terminating. The user can set a specific iteration number to use for the initial value of the density residual using the STARTCONV_ITER option. For example, the simulation for the inviscid channel will terminate once the density residual reaches a value that is 6 orders of magnitude smaller than its value at iteration 10. Note, however, that SU2 will always use the maximum value of the density residual to compute the relative reduction, even if the maximum value occurs after the iteration specified in STARTCONV_ITER.
The channel simulation for the 256x128 node mesh will execute on a single workstation or laptop, and this case will be run in a serial fashion. To run this test case, follow these steps at a terminal command line:
- Move to the directory containing the config file (inv_channel.cfg) and the mesh file (mesh_channel_256x128.su2). Make sure that the SU2 tools were compiled, installed, and that their install location was added to your path.
- Run the executable by entering "SU2_CFD inv_channel.cfg" at the command line.
- SU2 will print residual updates with each iteration of the flow solver, and the simulation will finish after reaching the specified convergence criteria.
- Files containing the results will be written upon exiting SU2. The flow solution can be visualized in ParaView (.vtk) or Tecplot (.dat for ASCII). To visualize the flow solution in ParaView update the OUTPUT_FORMAT setting in the configuration file.
The following images show some SU2 results for the inviscid channel problem.
Figure (2): Mach number contours for the 2-D channel.
Figure (3): Pressure contours for the 2-D channel.
Please take a minute and complete a brief survey about your experience with this tutorial. Your feedback is anonymous and goes toward improving your experience with the software.