[mazhar16823]

Hi everyone,



I am a little confused with the relation of lift coefficient with the Reynolds number. As, I did a comparison of lift/drag coefficients from CFD plotted against angle of attack (Re=0.3 million) with higher Reynolds experiment (Re=3 million).

The drag coefficient at higher Reynolds is lower than one in the CFD simulations which makes me assume that at higher Reynolds number flow becomes more energized such that it penetrates through the zone of high adverse pressure gradient consequently the drag is reduced.


However, the lift coefficient at higher Reynolds (experiment) is HIGHER compared to the CFD results. Could you please describe this behavior in light of following attached images?


Thanks for your time.

[sapujapu]

What turbulence model are you using? The experiment shows that at an AoA of 10deg, the flow begins to seperate from the airfoil. Are you sure that your turbulence model can accurately capture this separation? Most models are pretty bad at this.

[mazhar16823]

Originally Posted by sapujapu

What turbulence model are you using? The experiment shows that at an AoA of 10deg, the flow begins to seperate from the airfoil. Are you sure that your turbulence model can accurately capture this separation? Most models are pretty bad at this.

I used Gamma-ReTheta model. Another reason of discrepancy, could be the different Reynolds no? As experiment has Reynolds ten times higher than CFD;

[agd]

Ummm, yeah. The Re difference can have a very large impact on the results comparison. You ran CFD at a Reynolds number that is probably somewhere in the transitional range and compared to an experiment in which the flow is most likely fully turbulent. You are basically comparing apples and oranges.

[Bob Tipton]

I have been doing similar work on drag for that 6 months. In my case I am in the very high drag/low RN regime in H20 but some of what I have been finding may be helpful.

The distance to the analysis boundaries is critical. I'm finding that to get good correlation with experiment the work volume must be 20 x the model characteristic dimension on all sides, double that in the down stream direction.

I don't have a firm figure on that, but the usual advice of 6 to 8 x is much too small.

I wasted weeks pursuing an effect I thought was related to angle of attack to find that the change in angle was actually moving the model too close to the boundary.

Check you stagnation pressures in ParaView. If you want precise results NO pressure should be greater than free stream stagnation. If it is, then you're too close to the inlet.

As I said, I'm in a totally different regime.

Today I'm still fighting getting good correlations with reference shapes like a hemisphere.

[CFDfan]

Originally Posted by Bob Tipton

I have been doing similar work on drag for that 6 months. In my case I am in the very high drag/low RN regime in H20 but some of what I have been finding may be helpful.

The distance to the analysis boundaries is critical. I'm finding that to get good correlation with experiment the work volume must be 20 x the model characteristic dimension on all sides, double that in the down stream direction.

I don't have a firm figure on that, but the usual advice of 6 to 8 x is much too small.

I wasted weeks pursuing an effect I thought was related to angle of attack to find that the change in angle was actually moving the model too close to the boundary.

Check you stagnation pressures in ParaView. If you want precise results NO pressure should be greater than free stream stagnation. If it is, then you're too close to the inlet.

As I said, I'm in a totally different regime.

Today I'm still fighting getting good correlations with reference shapes like a hemisphere.

Could such large dimensions (producing good results) be just related to the fact that your fluid was H2O having much higher density that the air?

[Bob Tipton]

Yes.

The kinematic viscosity is about 15x higher for air and that would have a larger damping effect.

I did some experiments with doing my trade studies in air to speed things along - but results were more similar than I would have expected. The higher viscosity sped convergence but didn't seem to change the pressures or forces very much - in my case.

I found a video on doing these studies in Fluent in air and they were also using an extremely large analysis volume. IIRC 40m cube for a 1m model.

After many weeks of wasted runs I found that to get very good agreement I needed much larger volumes.

The higher the drag the more volume was required. This seems to be related to how much the flow is disturbed.

From an old experimental engineer -
Start with a huge volume.
Get good correlation.
Then start reducing the volume until the error is larger than acceptable.
Then increase it to the prior acceptable size.
If you expect the disturbance to increase during later changes, make the volume bigger.

Then you should have a working volume that can handle the range of your models and you can be _reasonably_ assured that it's your model producing the results and not the analysis conditions.

I found that each time I increased the volume my results came closer to actual experimental references. I was able to get within .7% for the Cd of a thin square plate normal to the flow. When I changed to solid hemisphere or a complete cube, I needed a bigger volume.

WATCH OUT for symmetry and the upstream distance. Use the full dimensions, not the 1/2 symmetric ones.


Your absolute volume will differ because of the difference in fluids, but the process is the same.


I'm still fighting this and I'm currently blocked because SHM fails to mesh my models correctly.

[CFDfan]

Thank you Bob for these insides, very educational. I am involved in electronic cooling and did just once the lift and drag coefficients of the "Ahmed body" I did that just to verify the correlation between the published experimental and the simulation results from scStream I use. I also used large computational domain but about 5 times smaller than yours. I also observed a difference in the results from a half (i.e. with symmetry) model and a full blown model.

You mentioned using also a semi-spherical domain. How large should it be to get good results

[Bob Tipton]

After lots of experimenting with boundary conditions, meshing and relaxation - I was able to reproduce the measured reference Cd of a solid hemisphere to within 0.020%.

It's not easy.

Key to a good solution are proper boundary conditions.

Ideally the inlet should be constant mass flow integrated over the entire inlet with zero gradients. Since this isn't available, I chose fixed velocity and zero pressure gradient.

The other boundaries should be zero gradient for all other properties.

Because the case was incompressible, there is always a back pressure at the inlet. This effects pressure and flow. I placed the inlet 10m ahead of a 0.7071m radius sphere.

Since a high drag body like a flat hemisphere facing into the flow creates a significant blockage, I placed the side and back boundaries 15 m away.

I then used simple grading in the perpendicular axes to concentrate cells near the model.

I also used a cylindrical refinement region centered on the target and finishing at the rear boundary.

Combined with moderately fine refinement of the model and edges this resulted in matching the published Cd of 1.17 with a value of 1.169766 which is exact to the published 3 figures.

HOWEVER

I did this case preparatory to doing Cd studies on research bodies. When I moved the case to a cloud service (KaleidoSim) it differed by 1.025%. Also the number of steps changed from 3600 to nearly 5,000 - with no sign of convergence.

I would love to hear from anyone with an insight as to why this happened?

The cloud and my laptop have the same OpenFOAM version number, number of cores etc.

[CFDfan]

Bob, what turbulent model did you use in your study?

[Bob Tipton]

SimFlow reports - RNG k-ε - RAS
It's an option in their UI.
I've got 40+ years in fluid dynamics, but only 6 months using the new CFD tools.
I did experiments with other methods and didn't get good results. That proves nothing because the cases were corrupted by other errors such as incorrect boundary conditions and meshing.

[Bob Tipton]

One other item.
The minimum pressure isn't achieved until the trailing vortex stabilizes. Since there is virtually zero mixing in the trailing vortex and all of the energy must be transferred by fluid shearing forces - it takes time for the vortex to 'spin up'.

This leads to a false convergence. The force graph declines over time and in some cases it appears that it's converged to a residual of 1e-4. If you use 1e-5 and let it run, the force gradually rises as the trailing vortex forms.

After a period of time, the true convergence occurs and the residual drops below 1e-5.

[CFDfan]

And you monitored the Y+ distribution I guess. If you remember, how was the Y+ roughly distributed in the 0.02% accuracy run?

By the way, congratulations for that amazing result. In my application area 5% accuracy is quite acceptable (mainly because the power dissipation in the components is very difficult to get with high accuracy) and the 0.02% accuracy you posted is mind blowing.

I am not familiar with the OpenFoam, but if it has adaptive meshing it should help a lot (at least in theory) with the accuracy.

[Bob Tipton]

My goal was to get an error < 0.5%. I'm trying to find out how high a Cd is possible from a real structure and some of my early figures were not credible. So I went back to 'calibrate' the analysis against standards.


I was shocked when I got the 0.020%. It's probably not reproducible.


I'm posting some pics that can help. I'm trying to concentrate the cells in the 'interesting' part of the flow.


I'm planning to do a set of videos. While it's good for the audience to not know the outcome, I need to. lol

[Bob Tipton]

Here's a second pic of the pressure distribution.
It shows why having a very large volume to the side is required.