[Mason liu]

Hi, all,

I'm starting to estimate the drag force of cylinder-like body which axis is perpendicular to flow.

And recently I have a basic question about the Reynolds Number and Y-plus in external flow. Could you guys please kindly help me? Thank you all really. Details as below.

1) For example, flow through a finite length cylinder-like rod(the rod perpendicular to flow), how should we calculate the Reynolds number, ie use which size as length scale: diameter(D), length of rod(L) or flow-field size(W)? I think should use the diameter(D).
Length Scale.jpg

2) Use above estimated Reynolds number to calculate the Y-plus and calculation result gives bigger Y-plus on some wall-area where has high velocity region close to wall. And according to Y-plus's definition:
Y-plus=ro*frictional velocity*first cell height/dynamic viscosity
This definition seems tell us that for a uniform first cell height, Y-plus should be bigger on those wall-area which has high velocity region nearby(because this region gives bigger frictional velocity). Is this guess right?
External flow.jpg

3) If this is right. Then those Y-plus values on wall will vary with velocity nearby, so if we use a low-Reynolds number model(Like SST) and we need a Y-plus=~1, do we just need the maximum Y-plus on the wall around 1 or what? If this is true, then the method we used to calculate Y-plus based on Reynolds number seems not that accurate, the maximum Y-plus will be obviously bigger than what we expected. Because we use a normal velocity to calculate the Reynolds number, then Y-plus, but the actual flow will give local high velocity region, on those wall close to this region Y-plus will be bigger.

This really confused me long time.

4) And in flow simulation(like drag force estimate) do we need to guarantee all Y-plus value the same as what we need on wall? This seems extremely hard to realize. Usually we can only keep the first cell height same, does this acceptable?

My English is not good and expression may be not that clear, beg your pardon and really want to receive your guide. Thanks a lot all.

[ghorrocks]

1) The usual parameter is the cylinder diameter.
2) The usual approach is to aim for y+=1 (approx) at the maximum y+ point. Then use a constant first mesh spacing, so then all the other points will have y+<1.
3) See 2).
4) For flows like the Ahmed body the boundary layer does not need to be integrated to the wall so you might as well use standard wall functions. Then you can use a far coarser mesh. But the complication in bluff body flows like this is you have to handle the large scale flow unsteadiness - this is usually done with LES, DES, SAS or similar approaches. These approaches have quite different demands on wall boundaries.

[Mason liu]

Originally Posted by ghorrocks

1) The usual parameter is the cylinder diameter.
2) The usual approach is to aim for y+=1 (approx) at the maximum y+ point. Then use a constant first mesh spacing, so then all the other points will have y+<1.
3) See 2).
4) For flows like the Ahmed body the boundary layer does not need to be integrated to the wall so you might as well use standard wall functions. Then you can use a far coarser mesh. But the complication in bluff body flows like this is you have to handle the large scale flow unsteadiness - this is usually done with LES, DES, SAS or similar approaches. These approaches have quite different demands on wall boundaries.

Really thank you, horrocks,

Thank you for your confirmation, this make me some clear on this issue.

I have finished several simulation samples with the cylinder-like bodyone of them gives a some reasonable drag force value, it's about 6% compared to wind tunnel results. this sample's condition is [D=0.3m around, length L=1.4m, Domain size is large enough with 30mX20mX20m, Velocity in let with 36m/s around, SST model with auto wall function, turbulence 1%. INFLATION: first layer thickness=5e-5mm, 15 layers totally].

But you can see that the Reynolds number is about :7e5, so with Y-plus =1, the first layer thickness is about 0.009mm, but this 0.009mm can not give a good results. Only 5e-5mm can give a reasonable drag force value, within 6%.

this make me confused because this is not comply with what we know about SST model(need y-plus=1 is enough). This is also not comply with the below website about the boundary layer resolving,
http://www.computationalfluiddynamic...oundary-layer/

Could you please kindly give some comments, thanks a lot for your response.

[ghorrocks]

I have not read that link in detail so cannot comment on it.

But I think you will find that if you refine your boundary mesh to 5e-5 (which looks like y+=0.005) you are going to have round off problems and not converge well.

You may have said this, but why do you say you need the first layer at 5e-5?

[Mason liu]

Originally Posted by ghorrocks

I have not read that link in detail so cannot comment on it.

But I think you will find that if you refine your boundary mesh to 5e-5 (which looks like y+=0.005) you are going to have round off problems and not converge well.

You may have said this, but why do you say you need the first layer at 5e-5?

Thank you horrocks. Sorry for no reply in time beacuse the National Day.

• You mean that the simulation sample given the reasonable results was just got by chance? Actually this calculation is not converged well or have big round off errors? BUT from this simulation we saw some earlier separation than other simulation samples, this early separation may influence the drag force greatly and is what we expect.
• Another basic question: How can I find the round off problems, i don't know how to evaluate the round off errors. And about convergence, I just moniter the drag force, the residuals was below1e-5, is this enough?
• In some topics I saw some discussion about y+, y+ in Slover or solve y+, some like this. I'm not sure about those expression, I just use the variable 'Yplus' in CFD-Post processor for contour pattern on the body wall to see if my y+ match the turbulent model(For SST, y+=~1). Is the variable 'Yplus' in CFD-Post processor is the right value?

Thank you really.

[ghorrocks]

You mean that the simulation sample given the reasonable results was just got by chance?

No, I cannot say that as I have not seen the results. But there is a big risk of this occurring. If you have shown that this is not the case then it is fine.

How can I find the round off problems

Round off problems show up by numerical instability - which is an inability to converge. It is tricky to positively diagnose a simulation as having round off problems, but a few things which can help are:
* Single versus double precision
* Big changes in mesh size, time scale, velocity, pressure in a simulation.

Is the variable 'Yplus' in CFD-Post processor is the right value?

Yes.

[singer1812]

Going back to your first cell estimate and your body geometry. You stated that for 36m/s inlet and a 1.4m long body or D=0.3m, your first cell hieght for y+=1 is ~0.009m. Are you running this in air?

I think you miscalculated first cell height. I think your first hieght should be about 1e-7m to 1e-5m (you need to choose and appropriate travel length your BL will see), which is even smaller than the 5e-5m that you started seeing good values for Cl and CD. Did you plot your y+ on your body in Post? I would expect you might see values above 500.

Glenn, I have used first distant hieghts in the 1e-7m to 1e-9m range before. This is needed in supersonic+ flow with SST model in order to capture the aerodynamic coeffs correctly and to get the heat transfer nailed down.

Another important thing will be the total height of your prisms (if you used them). You need enough hieght and enough nodes in order to capture what that link you posted is telling you about.

[ghorrocks]

Glenn, I have used first distant hieghts in the 1e-7m to 1e-9m range before. This is needed in supersonic+ flow with SST model in order to capture the aerodynamic coeffs correctly and to get the heat transfer nailed down.

It is not the absolute value of the first cell height which is a risk but the y+ value it results in and the overall variation from the biggest to the smallest element in the domain. If y+ or the element size ratio is excessive then you risk round off causing convergence problems.

[Mason liu]

Originally Posted by ghorrocks

Round off problems show up by numerical instability - which is an inability to converge. It is tricky to positively diagnose a simulation as having round off problems, but a few things which can help are:
* Single versus double precision
* Big changes in mesh size, time scale, velocity, pressure in a simulation.
Yes.

Thank you horrocks, I'll check the Double precision & time scale in later simulation.

Originally Posted by singer1812

Going back to your first cell estimate and your body geometry. You stated that for 36m/s inlet and a 1.4m long body or D=0.3m, your first cell hieght for y+=1 is ~0.009m. Are you running this in air?

I think you miscalculated first cell height. I think your first hieght should be about 1e-7m to 1e-5m (you need to choose and appropriate travel length your BL will see), which is even smaller than the 5e-5m that you started seeing good values for Cl and CD. Did you plot your y+ on your body in Post? I would expect you might see values above 500.

Thank you singer, you may misread the unit I post, my calculation(0.009mm, ie 9e-6m) about first cell height with y+=1 is same to yours(you said about:1e-7m to 1e-5m ).

And I got a good value of drag force with first cell height=5e-5mm,totally 15 layers[Call this simulation sample as case#1], I plot the y+(Use variable 'Yplus') on body wall in Post and the max value is about 0.0361(Should be 5e-5/0.009*1=0.0056).

You can see that the y+=0.0361 is too small for SST, so I think if I want y+=~1, I should use first cell height=1/0.0361*5e-5mm=1.38e-3mm, take it as 1.25e-3mm for simplification and I finished another simulation[We call this as case#2]. This gives about half of the drag force, y+ is about 0.325(Not ~1), and flow field is different from case#1 obviously as below.
Case#1.jpg Case#1 y+.jpg
case#1
Case#2.jpg Case#2 y+.jpg
case#2

The max velocity near to body is different(43 versus 76), and flow separation is also different. In case#1 separation is early and there is lots of eddy near the body's side, in case#2 only eddy behind the body's back.

Obviously at least one case is very wrong, or both are wrong. What we know now is that case#1's results is good anyhow, and horrocks said this may have big round off error or not converge well, need to check.

Because of the capacity of my computer I don't want to try LES or other advanced turb model, I think SST may be enough for my drag force estimate(10% gap compared to wind tunnel is acceptable). For SST we need y+=~1, but I can't get a proper result. With y+=0.0361 I got the good value, is this really irrational??? but I think the flow in case#1 is some reasonable.

• And another issue: about some items in CFX-Solver Output File, as below.

Final average scale info:
+--------------------------------------------------------------------+
| Average Scale Information |
+--------------------------------------------------------------------+
Domain Name : Default Domain
Global Length = 1.4422E+01
Minimum Extent = 1.0000E+01
Maximum Extent = 3.0000E+01
Density = 1.1850E+00
Dynamic Viscosity = 1.8310E-05
Velocity = 1.9385E+01
Advection Time = 7.4399E-01
Reynolds Number = 1.8094E+07

Is this info above useful? For example the 'Reynolds number'=1.8e7, according to my calculation it's=1.2*36*0.3/(17.9e-6), about 7e5. And the 'global length', what dose this mean?

• Singer, another question to you, what do you mean by 'travel length' as below. Thank you.

Originally Posted by singer1812

I think you miscalculated first cell height. I think your first hieght should be about 1e-7m to 1e-5m (you need to choose and appropriate travel length your BL will see), which is even smaller than the 5e-5m that you started seeing good values for Cl and CD

Thanks a lot for your help, horrocks and singer. Look forward to receiving your guide.

[Mason liu]

Hi,
Glenn and Singer, could you please give me some advice about above simulation, I have been really confused on those results for a long time.

Any comments from anyone are deeply appreciated. Thank you.

[ghorrocks]

For SST we need y+=~1

Incorrect. SST can work with normal wall functions as well. So SST works with any reasonable y+ value.

Final average scale info:

Ignore these numbers if they confuse you. They are just calculated using things like the cube root of the volume to give a length scale and other gross generalisations. It is just there as a rough estimate, and you should calculate these numbers properly using physically relevant parameters to do it properly.

Calculation of drag on a body like this will depend greatly on the Reynolds number. At low Re the flow is laminar. After turbulence transition the flow sheds a vortex street and so you should model this with SST and try to resolve the vortex street. As the Re increases then the vortex street gets more chaotic and a DES/LES approach may be required. And as the Re increases again the vortices become small enough that a standard RANS turbulence model becomes applicable.

So the turbulence model you use - and the entire modelling approach - depends on what flow regime you are in. Have you established what flow regime you are in and what level of resolution you need to model the regime correctly?

[Mason liu]

Glenn, thank you very much.

Originally Posted by ghorrocks

Ignore these numbers if they confuse you. They are just calculated using things like the cube root of the...

Yes, thank you, I just read this(the cube root thing...) in other thread yesterday.

Originally Posted by ghorrocks

Calculation of drag on a body like this will depend greatly on the Reynolds number. At low Re the flow is laminar. After turbulence transition the flow sheds a vortex street and so you should model this with SST and try to resolve the vortex street. As the Re increases then the vortex street gets more chaotic and a DES/LES approach may be required. And as the Re increases again the vortices become small enough that a standard RANS turbulence model becomes applicable.

So the turbulence model you use - and the entire modelling approach - depends on what flow regime you are in. Have you established what flow regime you are in and what level of resolution you need to model the regime correctly?

Thanks a lot, this is really helpful to me. Seems that with Re number increasing, we should use 'laminar model'->'SST'->'DES/LES'->'standard RANS(k-e)'. Do we have a Re region that suit for above model? like below table(What are the Re value of a,b,c,d).
Re [0~a] [a~b] [b~c] [c~d]
Model [laminar] [SST] [DES/LES] [standard RANS]
And my Re is about: Re=ro*U*L/dynamic viscosity =1.2*36*0.3/(17.9e-6)~=7e5, what model should I use???

[ghorrocks]

You will have to research this yourself to find the transition Re numbers. It also depends on what you are trying to do - if you are looking for high accuracy and you have lots of computer resources you might tend towards LES, if you are limited in resources you might tend towards RANS.

Also note SST is a RANS approach.

This paper (http://ctr.stanford.edu/ResBriefs01/wang.pdf) describes some modelling of Re=10^6 flows which looks close to your application. It suggests your Re=7e5 is in the regime where they used LES as you are above the region with a coherent wake structure, but the individual turbulent eddies are still big enough to have significant effects.

I would start your work using RANS (ie SST), and possibly a turbulence transition model. See how close you get to the correct result and then consider LES/DES/SAS.

[Mason liu]

Thank you Glenn.

I'm not that familiar with CFD theory, and what do you mean by 'turbulence transition model', is that a certain turbulent model???

Originally Posted by ghorrocks

I would start your work using RANS (ie SST), and possibly a turbulence transition model. See how close you get to the correct result and then consider LES/DES/SAS.

I think recent days I have run in a mess about this simulation and loss the normal rhythm. I need to do a systemic sensitivity analysis about the Domain size, Mesh density, First cell height, turbulent model(ie SST or what) and so on.

Do we have a common order of those items above to do a systemic sensitivity analysis? Firstly with which one and secondly with which one...?

I think the order should be like: Domain size->Mesh density->turbulent model->First cell height.

Really appreciated for your guide.

[ghorrocks]

Turbulence transition model is and add-on model to the SST model which allows it to model laminar to turbulent transition.

It is not too important which order you do the sensitivity analyses in, it is very good you are doing them - you will learn a lot. It is especially useful if you have a good benchmark experimental or simulation result to compare against, so you know when you are on target. The paper I quoted might be good for that.

[Mason liu]

Hi,

I use a 2D-like(i.e. extrude one layer) simulation to estimate the drag of an rod in CFX.

The residuals(include the turbulent residuals) continue to fluctuate like below picture. But the drag went into a steady state.

WP_20141031_00_52_27_Pro.jpg
WP_20141031_00_52_18_Pro.jpg

What's maybe the reason for this? Mesh? Time step? I changed time step within a large region, but no big difference.

Can some one give me any suggestion? Thanks, any comments and tips are highly appreciated.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[SB123]

Originally Posted by ghorrocks

It is not too important which order you do the sensitivity analyses in, it is very good you are doing them - you will learn a lot. It is especially useful if you have a good benchmark experimental or simulation result to compare against, so you know when you are on target. The paper I quoted might be good for that.

• so you can do a temporal study on a low quality mesh to save computational resources?

• also, if/when doing a mesh study, and production has a variation of Re numbers, i would assume it's important to hit in all flow regimes ie sub critical, critical and super critical to make sure the mesh can handle most everything that will be modeled on it. is this fair to say?

[ghorrocks]

The temporal study needs to be able to resolve the important flow features. So the mesh needs to be fine enough that the important flow features are resolved. So the process is iterative - you do a temporal study, then you do a mesh size study. Then your initial temporal study may need updating on the new mesh, so you repeat the temporal study.... and then you consider if this has implications for your mesh.

So theoretically they are all coupled, but in reality the coupling is fairly weak. So you can usually home in on a good mesh/time step/convergence criteria fairly quickly, and once you have found that you can do the studies about that point and check it is OK.

Likewise, for your question about regimes - you need to repeat the study whenever new flow phenomena occur, or they occur on significantly different length or time scales.