I have a discrepancy when simulating a wind tunnel experiment of a 2.7% scaled NASA CRM geometry as used in the wind tunnel.

I am trying to replicate exactly the wind tunnel model and flow conditions of the AMES Wind tunnel experiment of NASA CRM by setting the right mach number, static temp and pressures to match the measured tunnel values. At the moment, all the fluid properties match perfectly as described in the AMES experimental data.(density, Re etc)

Coming to the geometry, I have modeled the AMES tunnel wall boundaries and the scaled CRM geometries at the different angles of attack as tested in the papers. Wall boundaries are given the appropriate boundary conditions.

It is a static rigid model, not flexible.

A well refined mesh with a y+ of 40 was created and simulated in these conditions

Turbulence model chosen was SST K-omega, with all the methods set to 2nd order. (ANSYS Fluent)

3 Key observations were noticed:

  1. Shock position was slightly ahead (~5-10% x/c) compared to experiment
  2. Cp peak values were 10% over predicted
  3. Drag Coeff prediction was ~30% underpredicted compared to experiment (Lift Coeff was extremely good ~ <1%)

I have 2 theories for the discrepancy in drag:

  1. Unresolved boundary layer and hence effect of viscous drag is not being modeled
  2. Wind tunnel model is not rigid, and its aeroelastic bend twist coupling is causing delay of separation due to shock, but I don't get how drag would be higher in that case

What would be a logical next step in determining a good agreement with the experiment?

  • Any changes to the solver or flow properties I am missing?

*Also as a query, would it make sense to try running a sim of the full scaled model, in the transonic flow regime, with the same Re and flow conditions in cruise as well? I am not sure how it will be a good method to validate my wind tunnel setup. Would the maintenance of Re and Mach number be enough to make the transonic cruise case and scaled wind tunnel experiment comparable?

** In case you are wondering which papers I am trying to replicate, it is the validation of the transonic wind tunnel model of the CRM by NASA.

  • $\begingroup$ By CRM you mean the Common Research Model? The half-model of an airliner without tail? At what angles of attack? Sorry, but this question is far too unspecific and only allows speculation. If you want meaningful answers, please provide meaningful information. $\endgroup$ Commented May 24 at 19:36

1 Answer 1


First, have you done a grid resolution study? Not just the boundary layer, but everything? Shoot for a halving and doubling of your mesh (i.e. one coarse and one fine) and then try to apply Richardson extrapolation.

What wind tunnel corrections have been applied to the experimental data? Are you comparing to the raw or corrected data?

Exactly what wall boundary condition did you apply? Transonic wind tunnels typically have perforated or slotted walls that do not behave like a solid wall (viscous or inviscid).

How is the model supported? Did you model the sting?

No aircraft or wind tunnel model is truly rigid. They may have attempted to correct for some flexibility already, but that remains an area to question.

Many of the CRM models have been used as AIAA DPW cases. Those studies typically have summary papers where many sets of results are compared and discrepancies are investigated. You should find the most similar cases and study those.

  • $\begingroup$ Sorry, upvotes are limited to 1 per person. This answer deserves many more. $\endgroup$ Commented May 24 at 19:33

You must log in to answer this question.

Not the answer you're looking for? Browse other questions tagged .