CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Pressure drop specification (http://www.cfd-online.com/Forums/cfx/19370-pressure-drop-specification.html)

Swapnil December 12, 2002 12:46

Pressure drop specification
 
Hi all,

In my geometry, i have periodic bounday condition with inlet and outlet acting as periodic pair.Thus, i can't define any inlet or outlet B.C. on the inlets and outlets. I want to define pressure drop in the domain. How can i define the value of pressure drop ?

Thanks, swapnil.

Holidays December 12, 2002 14:17

Re: Pressure drop specification
 
Source terms, momentum sources or resistances will drive the flow. This issue to control them so as to balance the flow.

Neale December 12, 2002 21:09

Re: Pressure drop specification
 
Search the archives for this. The topic has come up many times before on how to do this in CFX-5.

Neale

Swapnil December 15, 2002 12:20

Re: Pressure drop specification
 
Hi Neale and holidays,

Thanks for the reply.

Yaa, i know that for defining a pressure drop you have to define a Momentum source term or resistance coefficient. But for that one needs a subdomain(i believe).

In my geometry there is no subdomain. How can i define a pressure drop in the absence of a subdomain?

For example (a simple one and analogus)if you have a pipe and you want to define the pressure drop in the pipe. The pipe is acting as your domain. There is no subdomain here.

In my geometry (triangular duct), i have periodic boundary condition at inlet and outlet. so i can't define any B.C. on these boundaries and that's why i am defining pressure drop.

Regards, Swapnil

Sharks December 15, 2002 13:42

Re: Pressure drop specification
 
Swapnil

There are two solutions to your problem in CFX-5:

1) You can create a subdomain which is the entire geometry of your domain (use the same geometric solids). This allows you to specify momentum sources in combination with inlet/outlet bcs as per Neale's suggestion.

2) Use inlet/outlet bcs and employ user fortran to make the variables of interest (velocity) periodic. One way of doing this is to write the variables at the "exit" to an external file, and then read these values in to specify the "inlet".

Hope this helps,

Sharks


Swapnil December 15, 2002 22:25

Re: Pressure drop specification
 
Hi sharks,

Thanks for the reply. When i contacted CFX Support for this problem, they suggested me the way out that you suggested as second possibility ( using user Fortran) They called it custom periodic boundary condition and they also sent me an example of the fortran routine. But they don't have the db file for this type of particular example(custom periodic B.C.). Do you have a db file for this type of example? Let me know. If any body else has worked on specifying periodicity through user subroutines let me know.

Thanks and regards,

Swapnil.

Holidays December 16, 2002 08:06

Re: Pressure drop specification
 
1) is easy to test (this is what I meant in my previous post by the way.

Michael Bo December 16, 2002 08:22

Re: Pressure drop specification
 
Shift to STAR-CD! They have it as a default option where mass flow can be specified directly on periodic boundaries.

Neale December 19, 2002 20:41

Re: Pressure drop specification
 
Yes, but then you have to use a solver that sucks and a terrible user interface. No thanks to that suggestion.

Neale

Neale December 19, 2002 20:48

Re: Pressure drop specification
 
Swapnil, I think you may have misunderstood subdomains slightly. You don't need user fortran for this. Follow the suggestion of Sharks:

1) Make your entire domain a sub-domain in addition to being a "Fluid Domain".

2) Setup a momentum source term on the subdomain, which happens to be the entire domain. Set the momentum source to the required pressure drop.

3) Setup a translationally periodic condition on the two ends of the pipe.

4) Iterate on step 2 until you get the mass flow rate you desire. You can make a good estimate for 2 by using the Hagen-Pousille (sp?) rule if laminar and use the Moody diagram if turbulent.

There is no need to mess around with user fortran to do this.

Neale



All times are GMT -4. The time now is 12:57.