[anachronist]

I originally posted this a couple years ago in Physics Forums but got no responses, then my life got distracted by other things. I reproduce the posting here, hoping someone can advise me on a path forward.

I am using SimFlow with OpenFOAM on Linux to try to evaluate the drag coefficient of a water rocket body, constructed from a 2-liter Coke bottle with a conical nose, traveling through air at 77 m/s.

This should be a simple axisymmetric problem. So I created a wedge mesh, set it up for incompressible flow with RANS k-ω SST turbulence, force monitoring in the x direction. Here's a picture of my model with my wedge mesh:



I have a fair idea of what the drag coefficient should be: somewhere between 0.1 and 0.2. But OpenFOAM reports orders of magnitude lower: 0.00058.

Why is this?

I'm a newbie when it comes to CFD. When I was taking college physics 37 years ago, I don't believe CFD even existed then; at least it wasn't taught. I chose SimFlow as an OpenFOAM front-end mostly to have a GUI and to shield me from drowning too much in the OpenFOAM documentation, which isn't written for newbies and assumes a high level of expertise already. SimFlow also has good tutorials on their website.

As far as I can tell from the OpenFOAM documentation, the wedge angle is 5 degrees by default, or 1/72 of a circle. Is there some adjustment I need to do, to account for this wedge size and the reference area? I'm using the circular area projected into the airflow as Aref and the overall length as Iref. Should I be using the projected area just inside the wedge, or the whole wetted area from nose to tail inside the wedge, and then multiply the result by 72 or something?

Another thing I don't understand is the absence of flow separation at the bottle taper. I'm pretty certain that a 2-liter soda bottle traveling at 77 m/s through air will have flow separation there. This is no airfoil! I've seen separation on small airfoils in actual wind tunnels at lower velocities than that. The separation at the nozzle collar and nozzle opening is expected, but I can't bring myself to believe that there's laminar flow over the bottle shoulder. Here's what I get (showing airflow moving left to right toward the open end of the bottle):



This has been a long slogging learning curve so far. Not just for SimFlow, but for the FreeCAD software I had to learn to create my model, as well as a lot of studying just to learn how to set up the problem and visualize the results. I'm happy that I got any result at all (that's an accomplishment in itself!)... but I am not believing what OpenFOAM is telling me. The drag coefficient is unrealistically low, and the flow lines look too smooth.

Does anyone have any advice on how to proceed?

[mAlletto]

How did you calculate the drag coefficient. From the order of magnitude of the error it can be you used the wrong area to calculate it.


Best


Michael

[sqek]

in openfoam, 2d cases are treated the same as 1-cell think 3d cases for the most part
So the force calculated (if you're using a 5 degree angle) will be the force on a 5 degree wedge of bottle, so 1/72 of the force on the whole thing.

The wedge angle is set when you generate the mesh, if you're using extrude2DMesh then look in your extrude2DMeshDict - there isn't really a default, and the documentation just says it should be small - so check what it is - from the image it looks smaller than 5 degrees

lref isn't used for drag coefficient, just for moment coefficients, so it should only be Aref that makes a difference, and Aref should be the actual meshed area, not the full circle area (presumably frontal area is most relevant here, so frontal area * wedge angle / 360)

As for the separation - sometimes 2D-like steady structures actually need a 3D/unsteady simulation to capture them - look at something like vortex shedding, where an oscillation leads to a massively wider wake, which gets captured accurately by unsteady simulations but not by steady ones

Or there's a chance you've got the free-stream or wall turbulence levels set too high, turbulent boundary layers resist separation more because the velocity transfer into the boundary layer is faster, and can resist the adverse pressure better - so with "I've seen separation on small airfoils in actual wind tunnels at lower velocities than that", separation is more likely at lower velocities (or lower Reynolds numbers) - look at the dip in Cd for a sphere at high speeds/Reynolds, where the turbulence in the boundary layer becomes strong enough to shift the separation point rearwards

Or there shouldn't be a separation - a Cd of around 0.1-0.2 means you'd expect a separation region with an area of 0.1-0.2*the frontal area, which is about what you're seeing

[arjun]

Originally Posted by anachronist

Another thing I don't understand is the absence of flow separation at the bottle taper.

Thats your source of very low drag.

The lack of flow separation in my OPINION is due to dissipative convection term. This you can actually test by refining the mesh very much. If by refining mesh a lot you get rid of this then it is the source.

You can also have this situation due to over production of turbulence, that adds viscosity and end result is similar to dissipation in convection term.

If i were you:
1. Refine the mesh
2. Get rid of turbulence model

Then if drag improves then check back by adding turbulence.

[mAlletto]

The drag coefficient is two orders of magnitude smaller than the one expected. The lag of separation does not justify this