Modelling flow around a Smooth Cylinder - Drag coefficient HELP
 

Hi there,

I am using STAR-CCM+ as part of a university project and my first step is to ensure that the software outputs values near to what is experimentally accepted for a basic shape so I can trust the solutions later on with regard to how I set the simulation up.

The problem is I have modeled a smooth cylinder in a flow and I am getting a drag coefficient that is much less than expected.

Background:

The cylinder is in a cuboid volume large than itself to prevent interactions from walls etc. The volume is wider than the cylinder which itself has length 0.4m and diameter 0.2m.

I have calculated Re (rho x v x D / mu) as Re = (1000 x 0.1 x 0.2 / 8.8871E-4) = 2.22E4

I am using a fine mesh in the wake and physics models:
Gradients
IAPWS-IF97(Water)
K-e turbulence
Liquid
Realizable k-e two-layer
Reynold's-Averaged Navier-Stokes
Segregated Flow
Segregated Fluid Temperature
Steady
3D
Turbulent
Two-layer all y + wall treatment

The inlet face of the fluid volume is a velocity inlet with velocity set to 0.1ms-1 and the outlet is a pressure outlet, all other are walls including the cylinder with a no-slip condition and smooth surface.

The theoretical Cd for this reynolds number is around 1.3 but the program outputs a value of 0.28.

Is there anything obvious I am missing for such a discrepancy? Should I make the fluid volume the same width as the cylinder to reduce the effects on the end faces (surely they don't contribute that much)?

Please help!

Sorry this is rushed.

What is your Wall y+ on the cylinder surface?

It seems that the experimental Cd that you are looking at is for a long cylinder, am I right? In order for that Cd to be applicable, if my memory serves well, you need to have an aspect ratio (length to diameter ratio) of over 10. In your case, this aspect ratio is 2, so the end effects are not negligible.

I think the drag coefficient for a smooth sphere is around 0.5, so your drag coefficient should be somewhere in between 0.5 and 1.3, but probably you can find a better value for short cylinders.

The other comment is also very important to pay attention to: make sure the y+ value near the wall is appropriate for the model that you are using. For a Reynolds number of 1e4, try having y+~1 at the wall, and use a low-Re turbulence model.

As both comments above stated, check your wall y+. How many prismlayers are you operating with?

Thank you so much for your swift responses posters above!

This probably sounds silly but would you explain the y+ thing? (I really am new to the CFD scene).

With regard to the cylinder length I believe the experimental values are graphed for an *infinitely long* cylinder such that your comment would make a lot of sense and I will try that.

Also may I assume using a low-Re model at Re<~2000 and a high-Re for 1e5?

Many thanks,

~Asa

I have prism layers set to 3 based purely on some tutorials I've completed?

Wall Y+ is just a nondimensional number to help you determine if your mesh sufficient to describe the near wall velocity profile. You can read more about that here.

Now I would suggest to increase from 3 prism layers to 5-6. What is your set thickness?

Ah I see, thank you.

If you mean the Prism Layer Thickness, it is set at 33.3% of base 0.025m (so 0.008325m).

Try reducing it to 10%. Run the simulation and keep cheking on your wall Y+ values on the cylinder walls in a scalar scene. Values should be as close to 1 as possible, preferably lower.

Looking at the values now, 8mm seems a bit large for the boundary layer!

After running an exploratory simulation, it seems that my wall Y+ values are anything from 5-11.

Hi everyone,

Just to let you know where I'm at in case you have any further suggestions.

I've run the original cylinder (short, low aspect ratio) with the following modifications:

1. Thinner prism layers
2. 6 prism layers
(with the effect of lowering y+ to below 1)
3. low-re k-e turbulence model
4. low y+ model

Unfortunately I have to report that this has done very little and the value is pretty much the same.

I shall move on to a long thin cylinder.

At this point I would also ask what determines the turbulence model to be selected as I will need to comment on this formally?

How large is your fluid domain?

0.8m high, 1.5m wide and 1.0m deep.

This sounds kind of small for a cylinder with diameter of 0.2m. Are you sure you are not getting any reflections from the walls?

Looks good. I would set walls of the domain to a "slip" condition, you don't really need velocity gradient calculated on them, it will speed things up a little. How many iterations have the simulation been run for? Could we get a look at the residuals?

Also I am not really a fan of K-Epsilon when it comes to large separations, try the K.Omega model instead it may yield better results in this case.

Okay thank you, could you clarify what you mean by large separations?

Also can anyone comment on when to choose what turbulence model?

what is it that gives you that expectation on range for the C_d so large, the pressure relief on the short aspect ratio?

Large seperation, as in the flow has separated from the body, where pressure drag dominates over skin friction drag

K-omega turbulence model handles this separation better
k- epsilon is the standard turbulence model and doesn't handle seperated flows very well. there's plenty of literature out there, there's also a thread on here that compares the two, including different wall treatments... search k-omega k-epsilon (or variations thereof)

as for y+ values, there is a STEVE article that explains how to capture values of ~1, check there