[Shomaz ul Haq]

Dear all,

Hi. Hope everyone is well. I am modeling a heat transfer in double pipe heat exchanger. The inner fluid is hot water which is flowing inside a copper pipe. The outer fluid is cold water flowing in counter direction. The default domain interface name is "Domain Interface 1". In "Additional Interface Models", I checked "Heat Transfer", "Conservative Interface Flux" in "Option", "Thin Material" in "Option", "Copper" in "Material", and "0.05 [m]" in "Thickness". In "Basic Settings" tab, "Interface Type" is "Fluid Solid", in "Interface Side 1" "Domain (Filter)" is "Cold water", "Region list" is "cold_water_zone", in "Interface Side 2" "Domain (Filter)" is "Inner pipe", "Region List is "inner_pipe_outer_surface". I get the results for mass and momentum transfer and turbulence but not for heat transfer in CFX Solver, even though there is no error in CFX-Pre or CFX Solver. Would be grateful for help. I am attaching file for reference. Thanks

[Shomaz ul Haq]

Dear all,

Please help me. Dear Glenn Horrocks kindly help me. God bless you all. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

Dear all,

Please help me. Dear Glenn Horrocks kindly help me. God bless you all. Thanks.

I think that you didn't activate heat transfer model in domain options.

[Shomaz ul Haq]

Thanks Antanas, for the reply. Yes I included heat transfer in all domains. Please check thedocs I have attached too. Please help. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

Thanks Antanas, for the reply. Yes I included heat transfer in all domains. Please check thedocs I have attached too. Please help. Thanks.

Ok. I see. What do you mean by "don't get results for heat transfer"?

[Shomaz ul Haq]

I mean graphs of "Accumulated Time Step" versus "Variable Value" of "Heat Transfer - 1" and "Heat Transfer - 2" in CFX-Solver Manager are empty unlike graphs in Momentum and Mass - 1", "Momentum and Mass - 2", "Turbulence (KE) - 1", and "Turbulence (KE) - 2". This is what I meant.

[Opaque]

Create a new plot monitor, select residuals, and select H-Energy/T-Energy..

It may be the automated plots are not working as expected, but if you can see diagnostics for H-Energy in the output file, the data should be available.

One thing though that puzzles me is that you are getting Heat Transfer-1 and -2, and not a single Heat Transfer w/o numbering. The fact they are numbered separately is a sign you have not coupled the domain interfaces correctly, and the software created to independent heat transfer problems, i.e. the inner pipe is not exchanging any energy with the outer pipe.

[Shomaz ul Haq]

Hi Opaque. Thanks. How can I get the automated plots to work? Also I should mention that when I connected CFX-Pre to Mesh in Workbench and opened CFX-Pre there was only one Default Domain that comprised all three domains (inner fluid, pipe and outer fluid (I didn't make outer pipe in geometry)) and one Default Fluid Fluid Interface. Then I inserted the domain for the inner fluid (Hot Water) and then for the outer fluid (Cold Water) and then I changed the name of the Default Domain to Inner Pipe and made it solid as it now contained only the domain Inner Pipe. But the strange thing is that the default Fluid Fluid Interface remained a "Fluid Fluid" Interface even when I tried to change the Interface Type to Fluid Solid and clicked OK it changed back to a Fluid Fluid Interface. Then I had to insert a new Domain Interface 1 with Fluid Solid Interface Type and the Default Fluid Fluid Interface changed to one that I had inserted and there were no errors in CFX-Pre. Why did that happen? Would be grateful for an explanation for this. Also I would be grateful if somebody can tell me if one has a solid domain (Inner Pipe) between two domains (Hot Water and Cold Water) are there to be two Domain Interface (one between inner fluid and pipe and one between pipe and outer fluid) or just one. Do I need to add another Fluid Solid Interface Type Domain Interface. Thanks.

[Shomaz ul Haq]

Somebody please help. Would be extremely grateful. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

Hi Opaque. Thanks. How can I get the automated plots to work? Also I should mention that when I connected CFX-Pre to Mesh in Workbench and opened CFX-Pre there was only one Default Domain that comprised all three domains (inner fluid, pipe and outer fluid (I didn't make outer pipe in geometry)) and one Default Fluid Fluid Interface. Then I inserted the domain for the inner fluid (Hot Water) and then for the outer fluid (Cold Water) and then I changed the name of the Default Domain to Inner Pipe and made it solid as it now contained only the domain Inner Pipe. But the strange thing is that the default Fluid Fluid Interface remained a "Fluid Fluid" Interface even when I tried to change the Interface Type to Fluid Solid and clicked OK it changed back to a Fluid Fluid Interface. Then I had to insert a new Domain Interface 1 with Fluid Solid Interface Type and the Default Fluid Fluid Interface changed to one that I had inserted and there were no errors in CFX-Pre. Why did that happen? Would be grateful for an explanation for this. Also I would be grateful if somebody can tell me if one has a solid domain (Inner Pipe) between two domains (Hot Water and Cold Water) are there to be two Domain Interface (one between inner fluid and pipe and one between pipe and outer fluid) or just one. Do I need to add another Fluid Solid Interface Type Domain Interface. Thanks.

So you have domain for pipe, then why do you use thin material model in interface options? IMO if you meshed pipe then you should have two fluid and one solid domain with two conservative Fluid-Solid interfaces between them. Or you should just create two fluid domains touching each other, create Fluid-Fluid interface between them with thin material model activated. And each side of interface should be set as wall.

[Shomaz ul Haq]

Thanks Antanas for the feedback. I have already made a model with just two fluid domains and CFX-Pre just makes a Default Fluid Fluid Interface which is fine, but I want to include a copper pipe as well. As far as I know the thin material option is only activated with heat transfer which only shows for a "Fluid Solid Interface". By the way is there a way to add thin material in a Fluid Fluid Interface? Would be extremely grateful. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

As far as I know the thin material option is only activated with heat transfer which only shows for a "Fluid Solid Interface".

No.

Originally Posted by Shomaz ul Haq

By the way is there a way to add thin material in a Fluid Fluid Interface?

Interface Options -> Additional Interface Models -> Mass and Momentum -> Option = one of walls. And Heat Transfer checkbox will appear.

[Shomaz ul Haq]

Hi. Thanks Antanas. You are absolutely right. One question though. Do I select "No Slip Wall", "Free Slip Wall" or ''Side Dependent" in Option in Mass and Momentum in Additional Interface Models in Domain Interface (Default Fluid Fluid Interface)? Would be grateful. Thanks

[Antanas]

Originally Posted by Shomaz ul Haq

Hi. Thanks Antanas. You are absolutely right. One question though. Do I select "No Slip Wall", "Free Slip Wall" or ''Side Dependent" in Option in Mass and Momentum in Additional Interface Models in Domain Interface (Default Fluid Fluid Interface)? Would be grateful. Thanks

IMO no slip wall, but I think you know your problem better, so make your decision.

[Shomaz ul Haq]

Hi Antana. Thanks. I will use a non slip wall. In the meanwhile I have made two domain interfaces in CFX-Pre now and run CFX Solver but why do I get three graphs (two for H-energy and one for T-energy) in heat transfer when I use three domains (cold water, hot water, and inner pipe) whereas I get only one heat transfer graph when I use just two fluid domains with a Fluid Fluid Interface between them? Would be grateful. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

Hi Antana. Thanks. I will use a non slip wall. In the meanwhile I have made two domain interfaces in CFX-Pre now and run CFX Solver but why do I get three graphs (two for H-energy and one for T-energy) in heat transfer when I use three domains (cold water, hot water, and inner pipe) whereas I get only one heat transfer graph when I use just two fluid domains with a Fluid Fluid Interface between them? Would be grateful. Thanks.

Because you have two fluid domains separated by solid domain, so two H-energy plots for two fluid domains, one T-energy plot for solid domain.

[Shomaz ul Haq]

Thanks Antana. But shouldn't I get two heat transfer graphs for fluid fluid interface, one for one fluid domain and one for the other fluid domain? Would be grateful for an explanation. Thanks.

[Antanas]

Originally Posted by Shomaz ul Haq

Thanks Antana. But shouldn't I get two heat transfer graphs for fluid fluid interface, one for one fluid domain and one for the other fluid domain? Would be grateful for an explanation. Thanks.

I think you shouldn't. In the case of three domains both fluid domains are coupled with solid domain and not directly with each other, but via solid domain. When you have two fluid domains, they are directly coupled with each other. And we have the same energy equation for fluid domains. For solid domain we have different energy equation.

In other words, if all your domains are of same type and they all connected with each other via fluid-fluid or solid-solid (and so on) interfaces you'll have one H-energy or T-energy plot. For every unconnected domain you'll have its own plot as well as for every fluid-solid connection.

I hope you understand what I mean.