[PoliPro]

Hi,

I simulated a simple incompressible air flow through a small pipe (diameter = 1 mm) with StarCCM+ in order to verify the pressure losses along it.
The values of pressure loss I obtained are quite higher (60%) than the analytical ones.
The mesh is good and the turbulence model I used is the k-epsilon.
Any suggestions?

[SKK]

What is the Reynolds number of your flow? Is it turbulent or laminar?

[PoliPro]

We can consider a Reynolds number of 600, so the flow is laminar.
I've already simulate that case with laminar model but result doesn't change.
I'd prefer to use turbulent model in order to validate it for the next application with sharp geometry variations.

[SKK]

Are you using high or low Reynolds number turbulence model? What is your y+ values? In laminar case, how does the profile compare with Blasius's profile?

All failing, I would recheck the analytical solution to see if radius and diameter got extra 1/2 somewhere. This is a very common mistake and with 60% difference this is a very probable cause.

[vishyaroon]

I'm not surprised. One of my co-workers was trying something very basic like this (not sure whether it was pressure drop or laminar Nu values) and he could not get it to match analytical values.

Adapco should post some simple validations like this either in their web-page or the tutorials.

[PoliPro]

I am using an high Reynolds model.
Wall y+ is unfortunately < 15 and I know that it should be between 30 and 150.
I have not yet compared the profile I obtained with the Basius one, I will do...
No diameter/radius errors.

Next step is to change the turbulence model from k-epsilon to k-omega.
I could also try with a 2D model, in order to accelerate the process, what do you think?

[SKK]

When you say you have tested Laminar model and the results do not change, do you mean the pressure drop does not change? That does not sound right.

Performance of turbulence models vary for different geometry depending on which model you are using. For example, Launder-Sharma model is one of the best model for a flat plate boundary layer simulation. This is mainly because the constants and formulation for each models are derived and validated against different kind of flows.

Test with increasing y+ and see if that helps. Both the production and dissipation terms are very large in the log law region of 30<y+<100. The low y+ may result in high shear stress you are getting as du/dy would be much larger. Having said that, generally skin friction results when simulated are not much better than 30% off the analytical solution.

k-w models are much better in modeling adverse pressure gradient situations. It might be a good idea to test these, especially since you are using turbulence to model laminar flow.

It might be a good idea to test a simple model, ie a flat plate model to validate the turbulence models.

[monkaeydadde]

There is something called laminar flow hydrodynamical and thermal development or entry lenght problem. The growth of the boundary layer along the pipe create a situation where the heat transfer coefficient and the friction factor vary along the pipe. These 2 parameters vary until a certain lenght is reached. This lenght is called entry lenght and is where the boundary layer at oppisite radius reach each other. I suggest you to have a look at this book :
laminar flow forced convection in ducts by shah and London two of the most important researchers in the field. Using CFX doesnt require only ICT skills but also a strong background!