p@B=p@A ,is this possible in CFX?
Hi,all
I want to use the pressure distribution on boundary A to the other boundary B. Namely: p@B=p@A notice: The two boundaries is nodenode GGI connection. Is this possible in CFX? thanks in advance. frank 
Re: p@B=p@A ,is this possible in CFX?
That is what a GGI does.

Re: p@B=p@A ,is this possible in CFX?
Don't worry, GGI passes the pressure from one boundary to another boundary, But It seems to me that your problem is something else. You may probably want to see the continuous pressure contour ( No demarkation between two boundaries) then it may not be possible during initial runs, but If you run it for long time then you wil find that GGI worked perfectly.
Mehul 
Re: p@B=p@A ,is this possible in CFX?
Thanks your replies,Cyclone and Mehul.
The two domain in my problem are fluid domain and solid domain. An addition variable has been defined in solid domain whose value at the interface(solid domain side) will depend on the pressure at the fluid domain side. But for the solid domain GGI side, I can not use the pressure data for the fluid domain side. So, this question came out like this. would you say something in detail about this? Thank you! frank 
Re: p@B=p@A ,is this possible in CFX?
Ah. Is it that you want to transfer a pressure load to the solid? This can be done by setting up a structural analysis on the solid in ANSYS and passing the pressure as a boundary condition or setting up an FSI analysis by defining Fluid Solid interface boundary conditions in each code.
If this is not the case, then what do you want with the pressure? CycLone 
Re: p@B=p@A ,is this possible in CFX?
Thanks for your reply at first, CycLone.
The solid domain in my question, in fact, is a kind of porosity material. I have two tasks on this porosity material: modeling gas diffusion behavior and temperature distribution across it. But now I find I am on a tree. If I set the porosity material as fluid domain, modeling diffusion behavior is possible but getting the temperature across the porosity material is impossible. On the other hand, if I use it as a solid domain, modeling the temperature distribution is possible, but gas diffusion across the domain is impossible. What I plan to do is creating an "transition diffusion" additional variable for the solid domain by which I maybe model the gas diffusion behavior in solid domain. So this method should obtain gas diffusion and temperature at the same time. But how to define the interface boundary between these two fluid and solid domains? An idea come to my mind: defining a mass sink for the fluid side at GGI (depending on Pressure) and the same quantity mass source for the AV at solid side. I find that at solid side, the cfx system don't allow me to use the pressure at the fluid side at GGI. Pls enlighten me. frank 
Re: p@B=p@A ,is this possible in CFX?
Hi Frank,
CFX does not currently support porous CHT, but it is possible to make this work and it doesn't require any User Fortran. Set up your domain as a porous domain and create a vlumetric Additional Variable for your temperature, Tsolid, with units [K] (or [R]). In the fluid domains, leave the Tsolid variable off. In the porous domain, define it as either "Diffusion Equation" or "Poisson Equation", the only difference is that the Diffusion Equation formula includes the transient term. Add a subdomain within your porous domain and include the entire porous domain mesh. Within the subdomain, add a sourcesink pair to remove energy from the fluid energy equation and add an equal and opposite amount of energy to the Tsolid AV. This will essentially be a volumetric equivalent of a heat transfer coefficient. If you refer to the manual, you will see that the energy equation in a solid is identical to a diffusion equation. By comparing the two, you should be able to figure out what the appropriate diffusion term, boundary conditions, etc. need to be. Good luck. CycLone 
Re: p@B=p@A ,is this possible in CFX?
What a good ideal! Cyclone. I will try this method at once. Thank you very much!

Hello,
I read that you have a problem with the usage of pressure of the fluid domain in porous domain. I have a similar problem where i try to use one variable like pressure calculated in one domain in an expression to other domain. Can someone tell me how to do that? Thanks 
All times are GMT 4. The time now is 03:03. 