How to extract results from a previous simulation and use them as BCs?

Question: Fluent simulation of a system of components was performed.
How do I extract the results on certain interior zones and apply
them as BCs for the subsequent analysis of an individual component?
Mesh size of the 2 CFD problems is different-is that an issue?

Answer: Use "Profiles" feature in fluent. No problem if the meshes are different (fluent will automatically interpolate).

As an illustration of the above problem, see attached images "all.gif"and "single.gif":
"all.gif" (see <a target=_blank href=""></a> ) shows 3 pipes (~ a system),
"single.gif" (see <a target=_blank href=""></a> ) shows a single pipe in the middle (~ a component);
It is desired to extract solution at zone A from the 3-pipe-system analysis and apply those values as BCs for the analysis of the pipe-2 only.

Step-by-Step Method:
1. read the "all system" case & data file into Fluent
2. select File>Write>Profile...>Define New Profiles;
select desired zone(s) under Surfaces: for example, zone "A";
select desired field variables under Values: for example, velocity magnitude.
click on Write, specify a name for the .prof file.
3. read "single component" case & data file into Fluent
4. select File>Read>Profile... select the desired .prof file
5. apply the profile as boundary condition: for example, click on Define>BC
select zone A, click on Set, under Velocity Magnitude select
velocity-magnitude profile
6. initialize, and iterate as usual.

Attached "all-A_velocity.gif" (see <a target=_blank href=""></a> ) and
"single-A_velocity.gif" (see <a target=_blank href=""></a> ) illustrate that the Profile feature is grid independent.

For additional information consult Fluent documentation 6.26 on Profiles, and 3.14 on Grid Interpolation.

Show Form
No comments yet. Be the first to add a comment!