Compressible flow inlet not matching boundary conditions

[stefann]

I have a 2D compressible flow model of three stationary airfoils (one stage of a turbine). I have periodic boundaries on the top/bottom (Y+ to Y-), symmetry Z+/Z- of the fluid domain, imposed inlet with velocity/temperature/pressure set, and subsonic outlet with pressure defined.

Even long after stable convergence (25 000 iterations). When I plot a line through the entire domain from X- to X+, the inlet results do not match the applied boundary conditions:

--> Velocity is lower than input
--> Pressure is higher than input
--> Temperature is slightly higher than input

The outlet pressure is correct to the applied boundary condition.


Any ideas what's going on here and why the inlet results do not match the applied conditions?

[stefann]

Has anyone looked into this or noticed his behaviour?

[Yvan Fournier]

Hello,

No one has had this issue before to my knowledge.

If you do not provide details as per the forum recommendations, and explain by how much your conditions differ from what you expect, it will be hard to say more.

Regards,

Yvan

[Erwan Le Coupanec]

Hello,

As the previous post underlined, your case is hard to comment given the lack of details, but nevertheless you should keep in mind when analyzing a profile (if this a profile you had set in the GUI for example), that the values you obtain are cell values, there is no interpolation and you won't get any boundary values.

Regards,

Erwan

[stefann]

Hi:

I created a really simple test case of a 0.2m cubed domain with periodic y and z boundaries to show you what I mean. See attached cube.tar.gz

Inlet boundary conditions:

Code: Select all

Imposed inlet
V = 500 m/s (normal to inlet)
P = 500 000.0 Pa
T = 1200.0 K

Outlet boundary conditions:

Code: Select all

Subsonic Outlet
P = 250 000 Pa

I have monitor points (to check convergence) at the inlet, outlet and in-between. Here are the results up to 15 000 iterations:

Monitoring points - Pressure results.

As you can see, the pressure appears to have converged.


The inlet pressure (red line - 1) looks off despite the monitoring point being exactly at the x value at the inlet. I agree that this has something to do with averaging with the downstream values (which decreases along the domain) but it shouldn't be like this. Afer all, the applied boundary condition is exactly at the same location as the monitoring point - shouldn't these values agree?

A bigger problem though is the outlet pressure (blue line -2). How can it be ~380 000 Pa if the applied outlet pressure boundary condition is 250 000 Pa? This isn't even close.

Here is a plot of pressure along X in the domain to see what is going on:

Pressure along X in center of domain.

Yeah... no way there is a 250 000 Pa outlet pressure.


So what exactly is going on here?



Stefan

[Erwan Le Coupanec]

Which version of Code_Saturne are you using ?

[Erwan Le Coupanec]

About the pressure at the inlet, the value doesn't seem strange actually since, as I said, what you see is the nearest cell center value and not the value on the boundary.

Regards,

Erwan.

[stefann]

I am using version 3.3.2.

Regarding pressure at inlet - we do many turbine blade profile assessments. One criteria that is often used is to determine the the loss coefficient . This is defined by the average total pressure difference upstream and downstream of the blade cascade, measured over one pitch, and the dynamic head upstream. Total pressure = static + dynamic pressures.



We need the values at the freestream inlet and outlet values. If the results are coming back slightly inside the domain (at the cell centres) then these won't yield a correct answer. I could use the applied boundary conditions, but I wouldn't be able to get or as these are calculated values and as you said, I would be getting these results from the cell centres where the other values are directly at the boundary.

I know that other codes it is possible too get the nodal results instead of the cell centres. Is there a way to access this in Code_Saturne? Maybe you can think of a workaround to access the boundary values (similar to getting the wall values?)


Regarding pressure at outlet - I don't think that this can be explained by cell centre averaging as it is not even close to the exit pressure boundary condition.


Thanks


Stefan

[Erwan Le Coupanec]

Hello Stefann,

Since you use an imposed inlet condition, the Dirichlet value of the pressure at the inlet is really what you give, whereas at the outlet, by using the subsonic outlet boundary condition, you enable the resolution of a Rieman problem (in which the pressure you give is imposed as "right" state, and the last cell values are imposed as "left" state). The aim of this is to find in which state your boundary is (possibly the left state (supersonic outlet), an intermediary state (expansion wave for example), etc...).

The subroutine solving this problem is implemented in the file src/cfbl/cfther.f90 and is called in src/cfbl/cfxtcl.f90 (l.514),

Code: Select all

call cf_thermo_subsonic_outlet_bc(bval, ifac)

If you want to see the value of the pressure right at the boundary, you can it print out as follows

Code: Select all

write(nfecra,*) 'pressure at outlet boundary face', ifac, ': ', bval(ipr,ifac)

(insert this code line just after the call).

Hope this helps,
Erwan.

[Erwan Le Coupanec]

By the way, your demo test case is 1D. I suggest you use a 1D mesh as well to speed up the calculations and make it easier to analyze the results (especially if you start printing out some boundary faces values).

Regards,
Erwan.