CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   filter question (https://www.cfd-online.com/Forums/cfx/24318-filter-question.html)

 istvan July 27, 2007 11:53

filter question

Hi, I have to simulate a tap, but at the vater inlet there is a filter, to filter out contamination from water. Is there an easy way to do this, withot modelling the filter geometry? Thanks: István

 Robin July 27, 2007 16:54

Re: filter question

Are you modeling both sides of the filter, or is it just at the outlet?

-Robin

 istvan July 28, 2007 14:10

Re: filter question

Thanks Robin. There is water flowing through a tap (valve). There is a filter built in close to the inlet of the tap. I would like to ask, if it possible somehow to put a surface where the filter is, and to set the loss coefficient across this surface. Istvan

 Robin July 30, 2007 09:07

Re: filter question

Yes. If the filter is at the inlet, define it as an [i]Opening<\i> and use the [i]Static Pressure<\i> option. In the details panel you will find a check box for defining the loss coefficient. Enabling this option makes your specified pressure a reference pressure and the actual static pressure a function of this, the loss coefficient and the local flow rate.

Alternatively, if the inlet is upstream of the filter, split your grid (in CAD or when you create it in ICEM CFD) at the filter location and put a [i]Domain Interface<\i> at this location (note that you don't need separate domains to add a domain interface and the grid can still be 1:1). With version 11 you can specify a pressure drop at this interface, so just define you pressure drop as a function of the local speed and a reference pressure using CEL expression.

Regards, Robin

 istvan July 31, 2007 11:45

Re: filter question

Thank you very much. I'll try the second alternative. BR/István

 All times are GMT -4. The time now is 04:22.