Heat transfer in condensing boiler
 

Dear users,

i'm simulating a heat transfer between two fluid domains through an aluminium solid (solid PIN heat exchanger). I've meshed three separate bodies (with face-face contact). Two fluids are basically Flue gas with inlet boundary condition (temp. and mass flow (outlet is defined with static pressure 0 Pa)); the other is water with same type of boundary conditions.

Since solid part is not thin wall domain, there is a good 20mm + PINs of aluminium between fluids. Is there any way to create two fluid and one solid domain and then interfaces linked to them?? As for present there aren't any examples of similar cases on forum (or i can't find them).

The inlet boundary for Flue gas has no reaction coupling; mixture is constant mass fraction mixture consisting of H2O, CO2, N2 and some Hydrocarbons..

Any help would be greatly appreciated,

Marko

This simulation is straight forward. Setup 3 domains, being 2 fluid and 1 solid domains. Then connect the solid domain to the fluid domains with two interfaces, one on each side.

This is just a simple extension of the CFX conjugate heat transfer examples.

The only bit you might not have guessed is that you will now have two fluid domains which are not linked. This will probably give a warning message but can be ignored in this case. You also probably have different fluids in the fluid domains - I guess air in one and flue gas in the other. This can be done with a multicomponent mixture, or you can use expert parameters to allow you to set different fluids in different domains yet still have a single phase and component model.

Thank you.. I'll give it a try and post summary..

Marko

you can define two fluid subdomain in a single fluid(parent) domain

To use two separate and different fluids, I do in CFX Pre:
EDIT > OPTIONS > GENERAL > ENABLE BETA FEATURES > Then uncheck "CONSTANT DOMAIN PHYSICS"

Thank you all for your answers. I've done all suggested, but it seems there is a problem in interface/s. I have picked (prior to meshing) the outer faces of both fluids (flue gas and water) and named them as "Flue Wall" and "Water Wall"; since both fluids are sorounded by solid material (aluminium). With solid domain this is no easy task, since the Heat Exchanger surface (water and Flue side) is very complex.. I've let the computer do this automatically; of course it didn't work (known solver error info).

My question is; between solid and fluid domain if there are in example 10 faces in solid domain and 8 faces in fluid domain which are in contact; i have to pick all surfaces (domain depended of course) to make a correct interface. How is possible to define or pick faces on very complex geometry?' I have ca. 250 faces just for solid part with contact with water??

Thank you in advance..


Marko

Individually selecting faces on a big geometry can be very tedious. That is why you should define it as a named selection (if WB) or a part (if ICEM) so it is easily referenced. But if you must individually select all the surfaces in CFX-Pre then use the hide/unhide commands and box select to make the task easier and less error prone.

Thank you. So back to the drawing board.. I'll post when there is some progress.

Marko

Well, it seems i'm stuck.. On simplified geometry setup works fine, so i suppose a full geometry Sim would do the job. I'm having a hard time defining named selections in meshing for faces that will be interface connected in CFX-Pre. As for the water body (later domain) and the flue gas body, there isn't any problem defining faces (all are enclosed by solid aluminium - heat exchanger) - both water and flue bodies are basically negative from full solid part. The completely other story is how to pick faces on heat exchanger. There are supposed to be two contact face groups. One with Flue gas side (negative from flue gas body) and other water contact group. Well hand pick is literally sisyphean work.. Is there any option to form face group from other body (ie water or flue gas)?? Sorry for off topic..

Marko

You just need some practise in the picking tools. There is individual selection and box select. Also note box select can box-unselect. Also there are adjacent surface and tangent surface tools.

So you might do a single select with the tangential surface option (which selects all the surfaces with continuous tangents), then a box select to add a few it missed then unselect manually a few surfaces it got which are not part of it. Also don't forget to hide parts which are not relevant so they do not confuse things.

Have a close look at the selection tools. From your model a box select then manually deselecting a few surfaces should just about get it.