Hi All,

I'm looking at computing the drag on a body within a confined turbulent flow. Normally, in order to resolve drag on a body I would use a low-Reynolds number turbulence model such as SST, with low values of y+ to resolve the boundary layers well. However, in this case I would also like to model the effect of surface roughness of the body on the drag coefficient to get a qualitative understanding of how roughness will alter the drag coefficients.

How could this be done in CFX? Can it be done?!

My understanding of the surface roughness model in CFX is that it only works with wall functions where y+ >> 1, and that it would therefore not be valid to use it with low y+ values. However if I do use larger y+ values I would not normally trust the drag values from CFD anyway. So what can I do?

Any thoughts or advice would be very welcome.

Best regards, andy2o

Hi,

The size of the surface roughness is usually of the order of y+=1 so meshes that fine are not physically meaningful for surface roughness simulations.

Normal wall functions with y+>13 are good under the conditions they were designed for and give good drag results. It is only when you need to resolve the turbulent boundary layer rather than modelling it that you would need a y+=1 mesh. So why do you say you don't trust the drag values for large y+ values? If used appropriately they are just as accurate as a y+=1 simulation.

If you want to model surface roughness with a turbulence model then you are forced to use normal wall functions. You cannot directly simulate the effects of surface roughness unless you want to head down the DNS path and the is unlikely to be a good idea.

Glenn Horrocks

Glenn,

Many thanks for your thoughtful reply.

I'm modelling 1/2 inch non-spherical 'balls' suspended in a circular pipe with fast turbulent water flow over them. The balls occupy a significant fraction (~80% by diameter) of the pipe. I expect I will see separation at the surface of the balls and a (perhaps unsteady) turbulent wake behind them. I need to consider a variety of flow rates but I am waiting for data and cannot estimate a Reynold's number just now.

My (perhaps incomplete) understanding, which I am very happy to revise, led me to believe that it would be hard to correctly predict the separation and wake with a wall function approach (y+>13). This leads me to prefer a y+=1 mesh with SST for this task.

Do you think, based on this limited information, that this is a scenario in which wall functions could be used? (I will try and perform a comparison between the two approaches when the job starts, but any information would be helpful for planning.)

Best regards, Andy20

PS: I certainly agree with your comments about direct simulation and DNS!

Hi,

The objects are 1/2 inch but how big is the duct? If they occupy a significant fraction of the pipe you might consider modelling them as a porous region. Or is the roughness on the surface of the objects?

Glenn Horrocks

Hi Glen,

The objects occupy about 60%-80% by diameter of the duct. Infact, to be more precise the pipe has 1/2 inch = 12.7mm internal diameter, and the objects vary between about 8-11mm diameter. Ideally, I need to find a way to assess the effect of surface roughness of both the objects and the duct wall on flow in the duct. The duct roughness is a result of surface mineral deposits and is generally modest, <0.1mm, but noticable, the object roughness is a design parameter.

The purpose of the calculation is to estimate the turbulent hydrodynamic drag force on the objects, so I cannot use porous medium approximations in this case.

Thanks again.

Best wishes, andy2o

Hi,

Do the objects move? What are you trying to get out of the simulation? Pressure loss, forces/stresses on the objects, object motions etc?

Glenn Horrocks

Hi Glen,

In answer to your questions:

1) In some scenarios, the objects will move. However, for now I'm happy to consider them to be stationary.

2) I'm looking for the force on the objects due to the flow of water in the tube.

Best regards, and thanks for your continued interest,

andy2o

Hi,

If the objects do not move then I assume you have a solid model of the pipe with objects in it and you have meshed it all. The fluid takes a circuitious path through the pipe.

If the objects move then you will have to wait for V12 where there is a submerged object model. That will allow you to model objects larger than the mesh size and have then coupled to the fluid flow. You cannot do this with either a lagrangian or eularian model as they both assume the objects are small compared to the mesh size.

Glenn Horrocks

Hi Glenn,

"If the objects do not move then I assume you have a solid model of the pipe with objects in it and you have meshed it all. The fluid takes a circuitious path through the pipe."

Exactly right! I'm happy with that. That's what I'll do. However, I'd still be very interested to know if (now that you have heard a load more details about the task) you consider that a wall function approach could be justified for this task? Or, with the new information would you agree with my original assertion that a y+=1 model is needed?

Obviously with a wall function approach I have the advantage that I can set values for the surface roughness easily in CFX boundary conditions. But: Would the results be meaningful? There are two options:

A) - If the wall function approach cannot be justified (for example if the separation and wake behind the objects would not be correctly resolved by wall functions) then it would be a pointless waste of time to use rough wall function models and I would should instead find a different method to assess the effect of roughness.

B) - If the wall function approach is OK for this flow, then that's great news for me, as I have an easy way of making a basic assessment of the effect of roughness on the flow field and drag forces.

So, any thoughts on which of (A) or (B) you belive based on the description of the task in the earlier posts of this thread would be still be much appreciated! I'm not of course seeking guarantees from you, as this is all my responsibility, but I would nevertheless welcome the opinions of any experienced analysts reading this.

Regards, Andy2o

Hi,

What is the Re number? If it is low turbulence then the integrate to the wall approach is likely to be more applicable. If high then the wall function approach is likely to be more applicable. If it is laminar or transitional then most likely a laminar model is needed.

Whatever approach is likely to be suggested I would run a validation case where you compare integrating to the wall to wall functions and compare to experimental results. That is the best way to be completely sure.

Glenn Horrocks

Can any one of you tell me how to apply different regions of roughnes on the blade with CFX? Many Thanks

Hi,

I think you can make surface roughness an expression so therefore you can define a function to vary the surface roughness. If it is simple (maybe a simple function of radius or just a simple patch) you can use CEL expressions to define it but if it is more complicated you will probably want to use a 1D or 3D interpolation function to specify it.

Glenn Horrocks

Can any one of you tell me how to apply different regions of roughnes on the blade with CFX? Many Thanks

Hi,

My post just above answered that question. http://www.cfd-online.com/Forum/cfx.cgi?read=30498

Glenn Horrocks