Counter-flow simulation
 

Hi all,

I am trying to simulate a counter flow problem of a double pipe heat exchanger (a coaxial pipe with a hot internal flow and an external cool flow).

I have run several transient solutions with two velocity inlets and pressure outlets with specified inlet temperature and an interface boundary between the two flows of 5mm. The pipe is of 1 metre length.

I am trying to estimate the efficiency of the heat pipe by obtaining a temperature gradient along the length of the pipe. Ideally the temperature should be reducing along the length of the pipe for the hot flow and increasing for the cold flow along its length. However my model does not seem to have any change in temperature along the length suggesting that no heat is being transfered between the two flows! What could be going wrong?

Any help would be very much appreciated. I can give more details if the above is too ambiguous.

I suggest you start out with a steady-state simulation.
From the little information you gave, I can only guess that the physical time of your transient simulation is orders of magnitude smaller than the characteristic time scale of the heat transfer process you are trying to capture.

I have tried a steady state simulation but with the same resuts: no heat transfer between the fluid.

The flow is supposed to be 1.5m/s however I have changed this to 0.1m/s to allow heat transfer but to no avail. The transient simulation was for 5 seconds of flow.

I have not set a heat exchanger model as I did not think was required. Could this be the reason for no heat transfer?

Hi feedq,

I've been trying the same kind of simulation for a parallel flow exchanger - I think reviewing your boundary conditions should help. What conditions have you imposed on your pipe walls? It's necessary to use a coupled condition to ensure heat transfer at the interfaces, whereas a constant heat flux with shell conduction should be imposed on the shadow regions - See if this works.

Also, I agree with flotus1 - a steady state would be better off to start with and once you've established effective heat transfer, you try a transient run.

I made a boo boo trying to view the contours with "global" ticked once, so make sure it's off if your variations are too small :p

Hope this helped!

Thank you this sounds promising!
I have a coupled interface between the flows but have only set the heat flow properties for the resultant "wall-19" created by the interface. I set the wall thickness and heat flux for this wall at 0.005m and 1000 respectively.

I shall try your suggestion on my model and let you know.

I have tried as you suggested, kartrmswy. I am getting the same results as before :( I did infact have global range ticked for my contours before. Unticking this seems to have not made a difference however.

Could the problem lie with my model selection? I have only ticked the energy equation and laminar viscous flow for simplicity. Should heat exchanger be used?

Thank you again for your help

You dont need a heat exchanger model since you are explicitly modeling the heat exchanger.

A few more questions:
How exactly did you define the interface between the two regions? My method would be to set the two adjacent boundaries to "interface" and define an interface with the option "coupled wall" from these two faces.
Does your solution converge (especially the energy equation?)
Is your flow regime really laminar? Otherwise use a turbulence model.

This is what my quick&dirty counter-flow heat exchanger simulation looks like:
Attachment 23164

Settings were:

• inner radius: 0.02m
• outer radius: 0.03m
• length: 1m
• inlet velocities: both 1m/s
• inlet temperature cold: 300 K
• inlet temperature hot: 500 K
• viscosity (both fluids) : 1 kg/(m s)
• c_p (both fluids): 1000 J/(kg K)
• thermal conductivity: 1 W/(m K)

Maybe by trying similar values you can figure out where the error in xour simulation is

Thank you for the reply flotus1.

In meshing I specified the two contact areas of the two fluids as "interface-cold" and "interface-hot". Then in the Solution window I used "mesh interfaces" to join these two interfaces and selected "coupled wall". This then created four different walls in the boundary conditions:
wall-19
wall-18
wall-6
wall-6-shadow
I changed the properties of wall-19. But had, until now, ignored the other three generated walls.

I understand now from kartrmswy's post that it is possible to use one defined interface which should give an interface and interface shadow in the boundary conditions. From this I would be able to created the coupled wall and shell conduction wall. I have tried to do this but I do not seem to get a interface-shadow.

In your setup, wall 6 should be the interface. Could you check if it has the option "coupled" in the thermal tab? I didnt change any of the properties of the wall boundaries after creating the interface. Very strange.

I forgot to mention that I created the geometry for the flows and not the wall between them as I was going to specify the wall properties between the fluids. So the interface would be for a fluid-fluid boundary rather than a fluid-solid

wall 6 has the coupled option. Should I change the settings of wall 6 shadow to a shell conduction and heat flux as suggested by kartrmswy? When wall 6 thermal settings are changed the wall 6 shadow's settings are also changed at the same time it appears

That seems plausible. I would leave the option coupled wall for now. Lets keep it simple;)
Is the wall thickness of wall 6 set to 0?

Would you mind posting a similar contour plot like mine for velocities and temperatures?

Attached is what I am currently getting. The solution converges and you are right the flow is not actually laminar but turbulent. I have more reading to do on this so I decided to leave this as laminar for now.

The wall thickness is 0.005m (5mm).

And here is the velocity plot. The flow should be 1.5m/s for both fluids however I changed this to 0.5m/s to encourage heat transfer

What about the velocities?

I highly doubt that your solution converges if you are not using any kind of turbulence model for the turbulent flow.
Laminar is not the "easy" option if in doubt what kind of turbulence modeling to use since it will result in completely useless results if the flow is turbulent. Use at least the standard k-epsilon model.

Here are a few more screenshots from my setup:
int1 and int2 are the two boundaries of each fluid zone which form the interface
Attachment 23167
this is how I created the interface
Attachment 23169
This is one of the walls that appear after creating the interface
Attachment 23168

running out of ideas...

Just one more thing: Increase the thermal conductivity of your fluids to about 1 for testing purposes.

Fantastic! There is a temperature drop along the heated flow :)

However I don't know where this has come from.. the cooled flow has not heated up.

Forgot to mention: I used the k-epsilon model but left all settings after this as default (i.e. the new properties in the velocity-inlets were left as they were)

OK, so the outer wall of your heat exchanger exchanges heat with the surrounding medium... To prevent further confusion, we should set this boundary to be adiabatic (zero heat flux) and turn off the heat generation.
Maybe this will allow the outer fluid to heat up significantly.

Changed the outer wall properties to adiabatic (I forgot about that!).

And now there is heat rise in the outer flow and heat drop in the internal flow
Attachment 23174


Danke schön. You are a scholar and a gent Flotus :)

Awesome!

Here's one more thing you can try, just to be sure: insert a line along the radial direction somewhere in the middle and check the XY temperature plot - that should bring clarity :)

I had a similar problem trying to identify if my wall was perfectly conducting or if the resistivity of steel was taken into account - the temperature plot cleared that up!

Good stuff, flotus1 :D