External Incompressible Flow

Generally, the exterior or “far-field” boundary must be at least 5 to 10 chords upstream and 10 to 20 chords downstream of the body. Higher Reynolds number flows will require far-field distances in the upper portion of this range.

It is important to transition the element sizes in the mesh quite substantially to conserve nodes. It is common for elements on the body surface to be several thousand times smaller than elements at the far-field. Lift and drag forces calculated by Autodesk Simulation CFD will be dependent upon the mesh size near the body.

Transitioning must be smooth for solution stability and accuracy, and care must be taken to avoid creating tetrahedral elements with very high aspect ratios. Sometimes embedding fluid volumes using mesh refinement regions around the object of interest is very useful for concentrating many elements around it. This approach helps transition the mesh from very small elements around the object to larger elements further away from the object.

For incompressible and subsonic compressible flow problems with subsonic inlets, velocity and pressure boundary conditions are applied on the far-field boundary as shown in the following figure. To aid convergence, it is useful to specify the velocity boundary condition around a greater portion of the flow domain than for pressure, as shown in the following figure:

Apply slip conditions to any surfaces that are not openings unless the boundary layer or ground effects are of interest against the wall.

If the object has an angle of attack relative to the flow, it is better to re-orient the calculation domain instead of the object. The domain orientation should be that the free-stream velocity and the domain sides are parallel:

Note that convergence will often be slow, and the monitor will show relatively flat lines well before the flow field is fully developed around the body. Subtle differences in the pressure distribution may not be visible by only reviewing the convergence monitor.

To adjust the Automatic Convergence Assessment to Tight, on the Control tab of the Solve dialog, click Solution Control. Click the Advanced button in the Intelligent Solution Control group. Move the slider to Tight.

Autodesk Simulation CFD has been used to calculate the drag on aerodynamic bodies with a very high degree of accuracy. Such drag is due almost entirely to form drag. Such calculations can be very sensitive to the applied conditions in the model, and care must be taken to represent the physics as carefully as possible. This sensitivity is not unique to Autodesk Simulation CFD, but is inherent to all CFD tools. Some suggestions to improve accuracy of the drag calculation include:

• The region around the object must be meshed with a very fine mesh. More streamlined bodies require the mesh near the stagnation point of the body to be highly refined to capture the rapidly changing coefficient of pressure.
• Change the turbulence intensity to 0.01 (from the default of 0.05) for wind tunnel analyses. This will more accurately represent the conditions in an actual wind tunnel.
• Reduce the turb/lam ratio to 10 (from the default of 100).
• Enable Automatic Layer Adaptation.
• Use the K-epsilon turbulence model for the first 1000 iterations, and then switch to the RNG model for an additional 1000 iterations.

To simulate the effect of altitude, we recommend that you consult tables of atmospheric data to identify the static pressure and temperature based on a geometric and/or geopotential altitude. From the pressure and temperature, the density of the air can be computed and specified as a constant property.

If properties are held constant (hence you are not solving for compressible or thermal effects) the density is the only parameter that needs to be modified on the Material Editor. Keep in mind that the actual effect that is simulated at different altitudes is that of the Reynolds number.