Internal Airflow through a building

When using CAEDIUM Builder to simulate air flow through a building, how do I create the geometry to represent individual rooms and ensure that there is a single face representing a wall as opposed to the two super-imposed faces I get when I either subtract or intersect?

Thanks

[Edit: Based on an email exchange]

Your rating: None Average: 1 (1 vote)

No Zero-Thickness Walls

[Edit November, 7, 2011: Caedium RANS Flow can now deal with zero thickness (or double sided) walls]

We don't currently support zero-thickness double-sided walls in Caedium,
instead you'll need to use a box with a nominal thickness to represent the
wall and then subtract it from your air flow solid model.

Solver singularity

I've managed some sort of workaround for now, which is so far so good.

Unfortunately, I am unable to run the solver successfully. A brief synopsis of the problem setup - an IT room with computers to study different ventilation strategies. I have 3 inlets and 2 outlets and want to just run an airflow simulation first before introducing heat transfer.

At present, I keep getting the following error messages:

-----
Warning:
RANS Flow failed
Solver singularity: DILUPBiCG: Solving for epsilon: solution singularity

Warning:
RANS Flow failed
Solver singularity: DILUPBiCG: Solving for Ux: solution singularity

Warning:
RANS Flow failed
Solver singularity: DILUPBiCG: Solving for Ux: solution singularity
Warning:
RANS Flow failed
Solver singularity: DILUPBiCG: Solving for epsilon: solution singularity
-----

I have played around with my initial conditions to no avail (using both the fixed value, Turbulent Intensity & Length Scale for U, k & e in the flow Physics as well as reference values).

What am I missing?

Possible solver singularity causes

Glad to hear you've got your geometry configured.

Possible causes of solver singularities:

  1. Your units are off, e.g., you modeled your geometry in millimeters (though Caedium registered them as meters), but assigned your velocity in m/s.
  2. There are poor element shapes in your mesh. Try visualizing Vol Ratio on your volume and see if it's the case. For more on mesh viz try: "View a Mesh"
  3. You haven't assigned all your boundary conditions (bc) - it's easy to miss assigning walls. My strategy is to first make everything a wall and then assign other bc types such as inlets, outlets, and symmetry local. If you want to see a visual indicator try changing the color of the face and making it non-transparent after each bc assignment.
  4. Your reference values are not realistic, so check your reference velocity (U), turbulent intensity (k), and turbulent length scale (epsilon). Select Volume then visit Property Substance->Properties->Reference.
  5. Your relaxation factors are too aggressive, try reducing them - especially p. Select Volume then visit Property Substance->Solver->Relaxation Factors. For more on relaxation factors try "Relaxation Factors in RANS Flow Solvers"
  6. If there isn't a dominant flow direction, try setting the initial velocity to zero.

Trending Now