|
[Sponsors] |
Question regarding " Check isolated regions=f" |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 27, 2005, 16:55 |
Question regarding " Check isolated regions=f"
|
#1 |
Guest
Posts: n/a
|
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! |
|
May 27, 2005, 17:44 |
Re: Question regarding " Check isolated regions=f"
|
#2 |
Guest
Posts: n/a
|
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 |
|
May 29, 2005, 19:40 |
Re: Question regarding " Check isolated regions=f"
|
#3 |
Guest
Posts: n/a
|
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 |
|
May 30, 2005, 11:21 |
Re: Question regarding " Check isolated regions=f"
|
#4 |
Guest
Posts: n/a
|
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 |
|
May 30, 2005, 11:53 |
Re: Question regarding " Check isolated regions=f"
|
#5 |
Guest
Posts: n/a
|
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 |
|
June 5, 2005, 20:32 |
Re: Question regarding " Check isolated regions=f"
|
#6 |
Guest
Posts: n/a
|
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
question about uds | tanven | FLUENT | 2 | July 5, 2015 12:22 |
Unanswered question | niklas | OpenFOAM | 2 | July 31, 2013 17:03 |
connectivity check | Ted Crilly | Siemens | 2 | January 20, 2005 10:13 |
CHANNEL FLOW: a question and a request | Carlos | Main CFD Forum | 4 | August 23, 2002 06:55 |
question | K.L.Huang | Siemens | 1 | March 29, 2000 05:57 |