Centrifugal fan

[ZachJa]

Thank you,
unfortunately, there is just q_v = 1.0; in my examples list. Is there smth missing and list should be larger?

List with predefined symbols is full ie:

q_v: volumic flow rate

Predefined symbols:
x: X face's gravity center
y: Y face's gravity center
z: Z face's gravity center
dt: time step
t: current time
iter: number of iteration

Useful functions:
cos: cosine
sin: sine
tan: tangent
exp: exponential
etc.

Is there another place to look for MEI examples?

[Yvan Fournier]

Hello,

How would you write the expression you need in the C language, assuming t is the time and q_v the volumic flow rate ?

Regards,

Yvan

[ZachJa]

Hello,
tried different ways, but all the time have got "syntax error", could you please help to set an expression where q_v is from 1 to 10 and depends from time?
Thank you!

[Yvan Fournier]

Hello,

Could you list the syntaxes that failed ?

Did yout try things like

Code: Select all

q_v = 0.1*dt;

Or, more complex:

Code: Select all

if (t < 10.0) {
  q_v = 0.1*t;
}
else {
  q_v = 1.0;
}[/quote]

Regards,

Yvan

[ZachJa]

Hello, thank you.
yes it should work - but results are not realistic.

I started with fixed inflow to look for problem.
inflow is 0.026 m3/s directed normally to inlet, estimated k and epsilon for this geometry using empirical formulas, put 10 time steps with 0.01 s interval. Simulation is finished normally but results are not realistic: pressure distribution is jumping...
XML: https://www.dropbox.com/s/rvicvd7qyg08k ... 1.xml?dl=0
MED result file: https://www.dropbox.com/s/idz9ln3g6cdid ... s.med?dl=0
What could be the problem? Could it be because of mesh (I think it is good enough) or smth wrong in setup?

If I run 20 steps simulation - I have an error "Jacobi: error (divergence) solving for k".

Thank you for help.

[Yvan Fournier]

Hello,

Could you also post the "listing" file ? Did you check the CFL (Courant) number's evolution in that file ?
You probably have a too large time step, but I can't check without the recommended info.

Regards,

Yvan

[ZachJa]

Hello,

I do not know what range is acceptable for CFL, so, listing is here:
https://www.dropbox.com/s/2qiiy7d2uhxf1cy/listing?dl=0

thank you!

[Yvan Fournier]

Hello,

CFL recommendations may be found in the documntation "best practices" section, page 3 (http://code-saturne.org/cms/sites/defau ... meters.pdf).

You should try to avoid a max CFL greater than 5 or 10. After 1 time step, you are already at 26000, then things get worst, so you need to divide your time step by at least 1000 or even 2000).

Regards,

Yvan

[ZachJa]

thanx a lot,
I decreased time step and results are realistic now.

is it possible to get mean pressure values at inlet and outlet (ie not just specific points but for whole patch inlet and outlet)?
I added mesh of inlet and outlet into output control:
https://www.dropbox.com/s/eqyc2xlaoqvrh2j/1.1.png?dl=0
but there is no data to monitor when I open it for post-processing:
https://www.dropbox.com/s/25iei5e3g80oqs5/1.2.png?dl=0
just regular data output for overall fluid domain:
https://www.dropbox.com/s/4648dbc8sfnjs81/1.3.png?dl=0

thank you!

[Yvan Fournier]

Hello,

I can't access Dropbox from the office. Did you check the the "inlet" and "outlet" meshes with a writer in the GUI ? Is the "auto" box checked ? Also check cs_user_parameters.f90 to see how to activate postprocessing of a cell-defined variable on the boundary.

With user subroutines, you could compute the mean pressure on the inlet and outlet (using cs_user_extra_operations fro example). Another option not requiring user subroutines is to integrate it with ParaView or EnSight once you manage to have it on the "inlet" and "outlet" output meshes.

Regards,

Yvan