CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   calculating pressure coefficient on airfoil surface (http://www.cfd-online.com/Forums/main/105632-calculating-pressure-coefficient-airfoil-surface.html)

calculating pressure coefficient on airfoil surface

Hi every one I am modeling an airfoil in an incompressible low Re flow! I set pressure in my outlet boundary condition as 1. I also set velocity in x and y direction at inlet. my question is when I solve the flow for example for a 10 degree angle of attack and when the flow reach a steady state condition, Are all the far field boundaries and inlet boundary supposed to have a pressure as same as the outlet boundary(it means 1)? if I want to calculate pressure coefficient, am I allowed to use P_out=1 instead of P_infinity or not? otherwise which pressure must be used for P_infinity for calculating pressure coefficient on the airfoil surface? Thanks for any word in advance!

 mb.pejvak August 4, 2012 21:07

I recommend you to read "Computational Fluid Dynamics Principles and Applications" by J Blazek. in chapter 8, I think you can find answer of your question.

I checked this book, in chapter 8 of this book the method which must be used to set the boundary condition at inlet or outlet for subsonic or supersonic flow is explained! it is not my question?!!! I don't have any problem with setting the boundary condition, my problem is that when I solve the flow over airfoil, and the solution is steady, can I expect the boundaries to have the same pressure as that which is set in outlet or not? if not, why this is so? because in most of the books and papers P_infinity which is needed to calculate Cp is set from upstream, it means inlet pressure! Is inlet pressure different from that of outlet?

 truffaldino August 5, 2012 03:55

Why do you care so much about absolute value of the pressure coefficient? Adding a constant (shift) to the pressure coefficient does not change total forces/ moments.

When your computation domain is infinite, the inlet and outlet pressures are the same. For finite size domains the shift in the pressure coefficient is inverse proportional to the domain size, (or the domain size squared, I am not sure).

Quote:
 Originally Posted by truffaldino (Post 375420) Why do you care so much about absolute value of the pressure coefficient? Adding a constant (shift) to the pressure coefficient does not change total forces/ moments. When your computation domain is infinite, the inlet and outlet pressures are the same. For finite size domains the shift in the pressure coefficient is inverse proportional to the domain size, (or the domain size squared, I am not sure).
I know that this shift doesn't have any effect on lift or drag, but I am comparing my pressure coefficient results. So a shift matters here. My problem is that, because the flow is viscous and low Re(viscosity is important) we have loss in the flow, why the pressure in inlet and outlet is the same? Well, you mean that if for example my domain is 20c farther, I must consider a shift in pressure coefficient which is inversely proportional to domain size?!

 truffaldino August 5, 2012 07:38

Quote:
 Originally Posted by mahzad (Post 375431) My problem is that, because the flow is viscous and low Re(viscosity is important) we have loss in the flow, why the pressure in inlet and outlet is the same?
Take as an example viscous flow past flat plate: the flow is viscous but the pressure is constant far away from the plate (or simply constant everywhere for boundary layer approximation/equations).

Quote:
 Originally Posted by mahzad (Post 375431) Well, you mean that if for example my domain is 20c farther, I must consider a shift in pressure coefficient which is inversely proportional to domain size?!
Yes, and for 20c domain it could be quite negligible. To have an idea about the shift value you could compare values of inlet and outlet pressure in your simulations, i.e. their difference divider by rho v^2/2

Quote:
 Originally Posted by truffaldino (Post 375437) To have an idea about the shift value you could compare values of inlet and outlet pressure in your simulations, i.e. their difference divider by rho v^2/2
So you mean that, in case of any differences I can add (p_out-p_in)/(rho*V^2/2) to the Cp values over the airfoil surface?

 truffaldino August 5, 2012 09:22

Quote:
 Originally Posted by mahzad (Post 375440) So you mean that, in case of any differences I can add (p_out-p_in)/(rho*V^2/2) to the Cp values over the airfoil surface?
No, this will give you an idea of value of relative error if you take p_out as p_infinity

Quote:
 Originally Posted by truffaldino (Post 375447) No, this will give you an idea of value of relative error if you take p_out as p_infinity
ok thanks, another question is that when my solution reach a steady state condition, the pressure is not exactly 1 at inlet, it's for example 1.12 and also it is not 1.12 at every node on inlet boundary, it decreases and reach to 1 as the nodes get farther from the node which has a pressure of 1.12 . If I want to use inlet pressure as P_infinity for calculating Cp,can I average the pressure at inlet nodes? Is it correct? or it is better to use a greater domain, the problem with the use of greater domain is that it increases my grid size and the amount of calculation needed!

 truffaldino August 5, 2012 10:49

It is not a good idea to average pressure at inlet, the error is rather determined by the maximal difference. Try to increase domain (it does not cost much computational time if you are using unstructured grids on outer part of the grid with spacing increacing towards the outer boundaries)

Quote:
 Originally Posted by truffaldino (Post 375454) It is not a good idea to average pressure at inlet, the error is rather determined by the maximal difference. Try to increase domain (it does not cost much computational time if you are using unstructured grids on outer part of the grid with spacing increacing towards the outer boundaries)
My grid is completely structured, and so it would take me a long time specially for unsteady modeling.Anyway thanks, I'm deeply grateful to you for your help dear! your information was really helpful to me!

 mb.pejvak August 5, 2012 20:30

Hi;
One of my problem is in this area. in Fact, I want to apply constant pressure as a outlet boundary condition in structured grid with collocated arrangement. I used dummy cell to do it, but I can not find out how ap should be calculated? (ap=L/ape; ape=(ap+apE)/2) ap is coefficient of main cell and apE is coefficient of neighbor cell (there is dummy (guest) cell ), my problem is calculating apE, because ap=
Σ an and in guest cell, we don't have an, or I don't know how to calculate it.

 michujo August 6, 2012 03:05

Hi Mahzad, if your problem is how to calculate the pressure coefficient over the airfoil, why don't you use the inlet velocity as the reference value? Then you'll come up with something like this:

where p is the pressure over the airfoil, and and are the density and velocity imposed far upstream (which you know becase you have set them).

What do you guys think?
Cheers.