blower modeling in Fluent

(1) Mesh Size

Don't under-resolve the blower. Make sure you have enough cells to adequately resolve all of the relevant geometry (e.g. blades, hub and shroud surfaces, etc.). Typical blower models may range in size from about 0.5 million to 2 million cells.

(2) Inlets

If the inlet to the blower is a pipe, and the pipe is aligned with the center of rotation of the rotor, include the inlet and rotor in a *** single *** MRF zone. This eliminates an interface between the inlet and rotor. As a rule I like to keep the number of interfaces to a minimum.

If your flow comes from the ambient, create a hemispherical volume and connect this to your rotor volumes, again placing both volumes into a single zone. You can make the bottom (flat) of the hemisphere a wall or symmetry (to mimic an inviscid wall) if you prefer.

(3) Interfaces

I like to use non-conformal interfaces so that I can go to a sliding mesh model if necessary. Make sure to ensure that the mesh resolution is about the same on the matching grid interfaces.

(4) Meshing

It is usually easiest to model the complex geometries associated with the blower rotor zone with tets. If you use non-conformal interfaces, you may be able to model the casing (which is often a simpler geometry) with an all hex mesh. Prisms on wall surfaces is probably only warranted for off-design cases, where severe separation needs to be predicted accurately.

(5) Solver Settings

* Use the Absolute Velocity Formulation.
* Use node-based gradients with tet meshes.
* Use Presto! for pressure discretization otherwise Standard is OK.
* Try to use Second-Order discretizations for Momentum and turbulence (you can use first order for turbulence of stability is an issue).
* SIMPLE is usually fine for Pressure-Velocity coupling

(6) Boundary Conditions

I *** always *** prefer setting the flow rate and predicting the pressure rise in fan simulations. This is the most stable configuration. You can set the pressure rise and predict the flowrate, but this is less stable. I would only do this if you want to predict the "free delivery" point, where the exit pressure is set to atmospheric pressure (and the fan is delivering its maximum flow).

Accordingly, use a velocity inlet and pressure outlet, or if you like you can use a pressure inlet with a velocity boundary condition at the outlet (with the velocity vector pointing out of the domain).

(7) Sliding Mesh

In some cases, the "frozen rotor" approach will not given the proper rise through the blower. In such cases, you should use the sliding mesh approach to predict the flow.

As a rule of thumb, choose about 1 - 2 degrees rotation per time step. You may need a smaller time step if you have a very fine mesh at the interface.
With the standard (subiterative) scheme, about 20 subiterations per time step is usually adequate.

With Fluent 6.2, you have the option of using the Non-Iterative Time Advancement (NITA) scheme. My experience to date has show that the NITA scheme can be a lot more efficient that the standard scheme in terms of overall CPU time.

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