I have fluid domain which is to be solved in STAR. It has one part to be sationary and other is rotating. What solver can be used for it. I request also the details of differencing scheme to be used while solving these problems if multiple reference scheme is used.

Hi Raja, based on my experience with fan-simulations I can recommend the following: 1. axial fan: the implicit mrf works well. in combination with higher order shemes the results are ok 2. radial fan: don't use the implicit mrf! It doesn't work in STAR when your pressure gradient over the interface is too high. They seem to work on it, but .... So, you have to use the explicit mrf. The convergence is poor, but finaly there is a solution, which looks quite well. Use 2nd order shemes with relaxation 0.6 for velocities and 0.1 for pressure. Maybe, you have to set the update frequency (in the explicit mrf panel to 2 or 3 for the first 20 - 100 iterations. Hope this helps,Thomas

Hi Thomas,

having unfortunately no experience with fan simulations I want to initiate one. Right now I am thinking of the right combination of boundary conditions. If my fan operates in a large free space my first guess would be that the borders of my fluid domain should be pressure boundaries with 0 Pa with the fan lying in the center of the domain. Do you think this bc's are adequate for that case or will this result in strange inflows to the domain preventing periodic solutíon.

Thanks for your opinion,

Tom

Hi Tom,

sorry for the late response, but I have been out of the office last week. Well, pressure boundaries should work. I would recommend to use the switch: ENVIRONMENT ON for your 'outlet' pressure boundary. This should work fine. If you are not interested in the mass flow rate for a given rotational speed of the fan, or better say: If you know the mass flow rate from measurements and your are only interested in the velocity, or pressure distribution, I would recommend to use an inlet-bc with the appropriate mass flux and a pressure-bc for the outlet. This will decrease calculation time significantly! If you obtain a strange flow field from that (sometimes this can happen - numerics!) you should try to start with inlet-pressure as boundaries and then do a restart (with new boundary-types!!) with pressure-pressure after, let's say 100 or some more iterations.

And as mentioned earlier: you shouldn't use the implicit mrf. Do a transient calculation or use the explicit mrf. This will end in much higher calculation times, but the solution will be much better.

Hope this helps,

Thomas

Thomas,

thanks for your answer !

I think that I can not use inlet bc, because the inflow in my domain is determined by the fan performance and is not known in advance. (?)

So if I use pressure_in=0 and pressure_out=0 would you expect to get a periodic and stable solution after some revolutions of the fan ?

Could you give some words to the switch: ENVIRONMENT ON

What is done by that option ?

Regards,

Tom

Hi Tom,

when doing a transient calculation with pressure-pressure-bc you should obtain a periodic solution after 5-6 rotations. You should try to use larger timesteps for the first rotations in order to keep calculation times low.

The 'environment on' switch treats the pressure of the ingoing flow at your boundary as total pressure and not as static pressure (see manual). This should help a get a better solution, when using 2 pressure-bc with p=0.

Regards,

Thomas