CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Question regarding " Check isolated regions=f" (http://www.cfd-online.com/Forums/cfx/21297-question-regarding-check-isolated-regions-f.html)

UW May 27, 2005 15:55

Question regarding " Check isolated regions=f"
 
Hi, all, When I use MFR to model a rotating turbine, I was asked to set expert parameters " check isolated regions=f" otherwise I can not run it. Do we have to do so? Anyone has the similar experience? What might cause this?

THX in advance!

hannah May 27, 2005 16:44

Re: Question regarding " Check isolated regions=f"
 
I met this kind info. before when my model had seperated solids. Mainly because when you connect your two models together using interface some dimension cannot match very well. You can check your geometry in the build to make sure the dimension is correct.

good luck


Glenn Horrocks May 29, 2005 18:40

Re: Question regarding " Check isolated regions=f"
 
Hi,

Can you describe your model? Also, does the model run when you don't have the expert parameter set? Also also, what version of CFX are you using?

Regards, Glenn Horrocks

Robin May 30, 2005 10:21

Re: Question regarding " Check isolated regions=f"
 
You will get this error message if the sover detects that two or more fluid domains are not connected. As the error message indicates, you should only set this expert parameter if you intended to set it up this way.

Most likely reason is that you forgot to add an interface or made a mistake in doing so. Check your interfaces first. The solver also writes out a <casename>.res.err file with a variable field to display the separate regions. Have a look at this in Post to see where they are not connected properly.

Regards, Robin

UW May 30, 2005 10:53

Re: Question regarding " Check isolated regions=f"
 
Hi,Glenn Horrocks the model is a stirred tank with a Rushton turbine. MFR is used. The model did run but no calculation in tank domain when the expert parameter is not set. I am using CFX 5.6

Thanks

Neale June 5, 2005 19:32

Re: Question regarding " Check isolated regions=f"
 
I'll add that this error message can happen even if you have a single fluid domain with no domain interfaces.

It is printed, in serial run mode, when the flow solver detects that a three-dimensional region of the fluid domain mesh is completely disconnected from the rest of the fluid domain.

This is bad because there may be no information to set the pressure level in that region and will cause the flow solver to blow up.


All times are GMT -4. The time now is 03:33.