Introduction
We demonstrate setting up a CFD simulation using the example of analyzing the unsteady flow across a circular cylinder at a Reynolds number of 1000 subject to heat transfer effects as well as turbulence. The following aspects of Abaqus/CFD are presented in this example:
- Creating and meshing a CFD part.
- Creating Material/Section and Section Assignment
- Activating Temperature effects
- Activating Turbulence modeling
- Edit Keywords to output surface forces
- Visualizing contour and iso-surface plots
- Creating streamlines
The CFD models are set up such that the flow Reynolds number based on the cylinder’s diameter (rVd/m) is equal to 1000. A typical workflow for a CFD simulation using Abaqus/CAE is shown in figure below.
Figure 1. CFD simulation workflow in Abaqus/CAE
Fluid model
The Abaqus/CFD model representing the fluid domain is shown in Figure 2. The diameter of the cylinder is 0.1 m. The computational model dimensions have been chosen such that the inlet, outlet and far-field boundaries are far enough from cylinder’s surface to avoid any boundary effects. The inlet is placed 4 diameters away from cylinder’s center while the outlet is 12 diameters away. The far-field boundaries are each placed 4 diameters away from the cylinder center.
We will model the 2D flow across the cylinder. Since Abaqus/CFD only offers a 3D solver, we will model the through-thickness direction with one-element and impose appropriate symmetry boundary conditions on the faces in the through-thickness direction to recover 2D behavior.
Figure 2. CFD model
The model consists of 3564 hexahedral fluid elements (FC3D8) with one-element in the through-thickness direction. The CFD mesh used in the current workshop is very coarse and a finer near-wall mesh would be required to resolve flow gradients near the surfaces. However, the mesh used in the case presented here is adequate to show the development of the vortex street in the wake of the cylinder.
Material Properties
The fluid is modeled as an incompressible Newtonian fluid. The properties of the fluid are chosen to achieve a flow Reynolds number of 1000 based on cylinder’s diameter and the inlet velocity. The fluid density is chosen to be 1000 kg/m3, viscosity is 0.1 Pa∙sec, specific heat is 4180 J/kg/K and thermal conductivity is 0.6 J/m/sec/K.
Flow Solver
The Abaqus/CFD procedure invokes a transient incompressible laminar flow analysis. Automatic time incrementation based on a fixed Courant-Freidrichs-Lewy (CFL) condition is used. The Spalart-Allmaras turbulence model is chosen to simulate turbulence.
Boundary Conditions
For unsteady flow across a stationary circular cylinder, the following boundary conditions are applied to the fluid.
- Inlet: An inlet velocity of 1 m/sec, temperature of 283 K and kinematic eddy viscosity of 0.0005 is applied
- Outlet: An outlet boundary condition is specified with the fluid pressure set to zero.
- Cylinder surface: A no-slip/no-penetration wall boundary condition is applied at the cylinder surface subject to a surface temperature of 313 K. All velocity components are set equal to zero.
- Far-field: The far-field velocity is assumed to be equal to the inlet velocity (i.e., the x-component of velocity is set equal to 1 m/sec). This is a reasonable choice if the far-field boundaries are far away from the cylinder surface. Alternatively, a traction-free condition can be enforced (i.e., no BCs prescribed).
- Symmetry: The velocity normal to the symmetry planes (Vz) is assumed to be zero to constrain the out-of-plane flow.
The boundary conditions are depicted in Figure 3.
Figure 3 Boundary conditions for the CFD model
Initial Conditions
The following predefined fields are supplies to start the simulation
- Initial kinematic eddy viscosity of 0.0005
- Initial temperature of 283 K
The simulation is run for a total time of 4 s which is sufficient to reach steady state.
Results
The contour plots of velocity and pressure are sought, in addition to the streamlines of the velocity. Time history plot of forces in the x- and y-direction are also shown that is useful for calculation of drag and lift.
Video Demo
A detailed video of setting up the simulation from scratch and visualizing the results is attached herewith.
The CAE file is also attached!
