I want to do a transient simulation where I have flow in a domain for a while, then suddenly a valve or door opens into a new domain allowing flow to pass through. Should I set up the simulation with both domains modelled and a wall between the two, and then perform a restart with the wall removed at the appropriate time?

Generally speaking, yes, people tend to start off with the 2-domain scenario and have something like a domain interface between the two with the 'conservative interface flux' options removed, or just a wall. The at the 60s point, you stop and change the CCL to allow flow through and then restart. This way there is no issue about the initial conditions to each domain, just the mechanics of controlling the flow between the two. You could also run it as one long simulation with a resistance and heat sink at the 'door' which disappears to zero at the right time.

However, this is sometimes not efficient. The other option would be to model the 2 domains separately in different simulations, and then bring them together in a new simulation. The way to perform this is to use Profiles to initialise each domain. Load each separate domain solution into Post in turn, and then choose File/Export. Choose the Type to be BCprofile and the location should be the domain name. Make sure you use the Global coord system and conservative values, and the profile type should be Custom. Then select the relevant primitive variables to your domain. ie: Pressure, temp, Velocity u/v/w, Turbulence k and e and maybe even material components. Then you write out the file for each domain. Then in Pre, load your 2-domain model, place a domain interafce between the two, then select Tools/Initialise Profile Data and select the profile files (each in turn). They may have the same name so you may need to rename the first or the second will just overwrite it. Then for each domain choose Domain Initialisation on the domain form and fill in all the fields with the profile references. These will be expressions of the form:
U = myprofile.Velocity u(x,y,z)
V = myprofile.Velocity v(x,y,z)
Temp = myprofile.Temperature(x,y,z)
and so on. If you want to check the syntax, select an inlet and edit it and check the 'use profile data' box and click to Generate Values with the appropriate Profile selected. It will then fill in all the boxes on the Boundary Details tab for you and you can see what they look like.
The only drawback with this option is that these profile data files may be quite large if you have a lotof nodes. It may also be quite slow to start up the 2-domain simulation as it does all the interpolation. It should work though, and is more flexible as it allows different meshes for the 2-domain comapred to each single domain, and allows you to modify the profile files (from different setups) without having to redo any interpolations onto def files and so on.

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