Hi all!

If I wish my result is fully developed flows, how can I achieve this? Do I need build the domain, such as the duct, long enough, so I can hope that the region sufficiently far from the inlet is what I need? Thank you!

Best regards!

Miko

Yes, unless you know the fully-developed profile. if you do, you can specify this as a function on your inlet.

Hi Louwrens!

Thank you again! According to physical analyse, we can know that the flow should be fully developed flows if the region is far from the orifice. I am wondering what did you mean. What kind of function can I specify on the inlet? You mean the velocity profile?

>What kind of function can I specify on the inlet? You mean the velocity profile?

Yes, you can specify the velocity profile on the inlet using CEL, then you dont have to model a long entrance. You'll have to be sure that this is the "correct" velocity profile of course, and this you'd get from previous experimental data, for instance. otherwise you can specify one of the analytical profiles (ie quadratic for laminar flow, some form of power law for turbulent)

I think you can have two approaches:
1) The easiest one: Create a duct with a long length (L/D > 40 should be enough) and use a medium grid size, not too refined. And then you extract all required information on your post-processor.
2) Not so trivial: Create a small L/D duct, note that D is constant in your case, I think L/D < 1 should do, and set both "inlet-outlet" as periodic pairs. You can use a reasonable mesh size over the duct area and just 3 ou 4 nodes on the axial coordinate. Provide the required momentum source, paying attention on the correct mass flow(Re number), and you'll get your fully developed flow.
The differences between those two? This first one is more computer and the second is more human time consuming. The results should be the same if you have the same grid size on the duct section.
Regards, cfd guy

Hi Louwrens and cfd guy!

Thank you!

I think cfd guy's idea is suit for me. But I also have an idea: I will use User Fortran Subroutine to import the data of velocity profile at certain place from the first calculation as inlet velocity. I will continue doing so untill the velocity profile is stable. IS such doing right?

Best regards!

Miko

Hi CFD guy, using your second method, is the periodic inlet / outlet, when specifying the momentum source, do you need to use a function or something like that ? or do you specify constant momentum throughout the model ? Bob

Hi Bob,


Unfortunately, I've been specifying a constant momentum source through the domain. I keep correcting it until I reach the correct massflow or Reynolds number. But you can use functions or generate scripts to do this for you.


cfd guy

CFD Guy, I'm sure you could do something clever with perl to itereate to your required mass flow rate ? Do you then extract the velocities K and Epsilon to use as your inlet conditions ?

Yeah, you should do some scripting in complex flows. It's up to you. :P


Answering the second question: Yes.