Error: Isolated fluid regions
 

I was trying to simulate a heat exchanger. The solver returned an error saying there were '4 isolated fluid regions'. While troubleshooting I came across this thread (http://www.cfd-online.com/Forums/cfx...tml#post327563) where CycLone suggested opening the res.err file in CFX-Post and plotting a variable (or creating an isovolume) to identify isolated regions.

Could somebody guide me on that? What variable to plot and how? Or how exactly to create an isovolume?

Thanks,
Rushabh

This is basic post processing and is covered in the tutorials.

I'm guessing it immediately failed when you went to solve?
If so you have to specify the pressure somewhere in each fluid domain (even just a reference pressure) for any enclosed fluid.

The root problem is there are unconnected sections of mesh - hence isolated fluid volumes. Either the mesh is wrong or th CFX-Pre setup is wrong. But the question is a basic one about post-processing.

Having said that, I don't think CFD-Post will help here anyway. Check your mesh in your mesh generation.

I am getting the same error msg. I just dont know what I am doing wrong. I have created a vid of my meshing. Its a little over 4 mins. Here's the link: http://youtu.be/J5nG-y1rM4w

I've been breaking my head over this for a week now. I would really appreciate any help.

Are the internal circles a pipe system for the heat exchanger or are they some form of heating/cooling element?

Ideally there should be no pipe (holes) in the Shell and initially I was not planning on putting holes (internal circles) in the Shell but going by the tutorial-geometry for the HeatingCoil example, I did. In that geometry they have drilled a hole in the Annulus and put a solid pipe in the hole (which can be simulated as a wire or pipe) and thats what I did for my Heat Exchanger. I made a hole in the Shell and fitted tubes inside.

Here's few images of the HeatingCoil geometry.

http://i40.tinypic.com/dc8x2t.png Heating Coil assembly

http://i41.tinypic.com/1076rfn.png Annulus hole

http://i41.tinypic.com/kdprf5.png Copper wire/pipe in hole

Sure, but you did not answer my question. What are the holes you have in the geometry?

Yup, so my point was that the holes mean nothing to me and I know they shouldn't be there at first place but I had to include them in the geometry to select a surface during the 'Domain Interface' selection. If I didn't have the holes in the shell I would have had no surface to select for interface like I do in the following image.




http://i40.tinypic.com/29290eu.png




In the pic the cold water zone is the Shell and the interface in shell region is the shell holes. The tubes carry hot water. Technically it is not a heating element but you could call it one therotically. So coming back to your question, the shell holes have no function as such and if I remove them and have one completely hollow shell I don't know what should I select for interface.

Thank you - that answered my question.

Do you want to model the flow in the tubes?

Yes sir but I would also like to see what's going on in the shell.

OK, now I understand the issue. You are always going to have isolated fluid volume in this model as the tube domains are not fluidically connected to the shell domain. You will have to use the expert parameter "check isolated regions = f" to turn off this check, as the error message says.

Why did you define fluid-fluid interface? Shouldn't it be fluid-solid interface? since fluid is connecting to the shell both through the tube and out side that.

You would use a f-f interface if you did not want to explicitly model the tubes. The thermal resistance of the tubes can be added as a factor in the interface model. Doing this simplifies the model considerably compared to directly modellign the intermediate metal tubes.