hello,every one I want to simulate a impeller. I specified three domains. the domain round the impeller as rotating domain,the entrance part and the outlet part as stationary domain. there are two frozen rotor interfaces,which can connect this three domains.

but my teacher told me, that I can specify a complete rotating domain (from inlet to outlet), the stationary wall of the fluid channel as counter rotating wall specified. at this rate cfx can caculate without interface.

I want to ask, whether this two kind of domain setting are same?? can get the same result??

thanks very much for answer!!!

i don`t think it is right way,it is not just problem of boundary.it is of basic modeling.shortly saying .there is centrifugal force and coriolis force in so calling "rotating domain"

Regards

wayne

Why do you want to use Frozen rotor? Is it an transient problem?

Hi Blazer,

What your professor suggested is correct. If your inlet and outlet parts are annular segments (i.e. no inlet vanes or diffuser vanes), then they can be included as part of the rotating frame and a counter-rotating wall can be applied to the hub and shroud.

If your mesh is coarse you may not get the same solution. When solving flow in a rotating frame of reference, the numerical diffusion will result in "false swirl", which is a tendancy for the flow to be driven in the rotating direction. You can see this effect if you model a straight pipe in a rotating frame with counter rotating walls, which should be equivalent to flow moving through a stationary pipe. In the stationary frame the flow will begin to swirl as it moves through the pipe.

Using the Alternate Rotationg Model will reduce this swirl (it is on by default if you use the turbo set-up mode), but refining mesh will also help.

So what university are you at?

-CycLone