Simple Convective Heat Transfer in Pipe

[Anonymous]

Hello,

I am looking to use CFD to help me with some modeling work of a more complex heat exchanger.  I wanted to start off with some basic conduction and convection analyses before I moved to the complex work.  I am having a few problems with my convection analysis.  I am new to this, so it could be a very simple fix that I have overlooked, but I have searched through the forums and have checked my work and have found no solution.

I imported a .step file of a cylinder with a diameter of 2 in and a length of 40 in.  I assigned to this a material property of water.  For the inlet surface, I have a boundary condition of 15 lbm/h mass flow rate and a temperature of 60 F.  For the outlet surface I have the pressure as 0 psi.  I have assigned a boundary condition to the two surfaces of the cylinder of 100 F.  I have set the flow to laminar, adusted the mesh a few times, turned on ADV 5, flag "resid_bdry_force_calc", and I am running in steady state till convergence. 

My first question is why the "Avg. Temperature" on the outlet surface given by the wall calculator does not equal the "Outlet Bulk Temperature" given by the Sum file?

My second question is why the "Reynolds Number" given by the sum file does not change significantly from the inlet to the outlet despite the fact that the temperature increases from 15.556 C to 32.6809 C (with negligible velocity change)?  With a temperature change like that, there should be a change in the viscosity, thus a more significant change in the Re than from 42.74 to 43.07 right?

My third question is why the Sum file has the "MdotIn * Cp * (Tout-Tin)" not equal to the "Heat Transfer from Wall to Fluid"?  The difference is around 6 W.  The only heat transfer here should be the heat that is from the wall to the fluid, so shouldn't these two values be equal?

My fourth question is related to the overall results.  I have built two models based off heat transfer correlations for laminar pipe flow, and both calculators are showing a final temperature around 98.8 F and the CFD is showing a result of around showing according to the wall calculator a final temperature of around 95 F, and according to the Sum file a final temperature around 91 F.  I work with a few gentlemen who have doctorates in heat transfer and they verified the correlations that I was using.  Now, I could be wrong of course, but I was wondering if you guys have any comments on this?

Thanks for your time and help, I do appreciate it!  

Regards, 

William

[Jon.Wilde]

Take a look at this article, 'simple' pipe flow can be hugely complicated 😄

You also have two temperatures Boundary Conditions touching - this is not OK. What should CFD assign where they meet?

You are going to need a far better mesh too.

This will go some way to answering your questions I think.

[Anonymous]

Jon,

Thanks for the feedback, guess you are right about the simple stuff haha!  I have added a copper tube to the outside surface of the pipe, and I have applied the temperature BC on that tubes outer surface.  Further, I added some extra water "pipe" at the inlet.  I have also ran with a finer mesh.  I think that takes care of my third question, the heat flux values there are lining up well.  

I feel like my other questions are still valid.  What mesh settings would you recommend for this?  Do you have any other recommendations, or see any other modeling or setup errors here?

Thanks,

William

[Jon.Wilde]

No problem 🙂

OK, your other questions:

1. For the outlet temperature, use the bulk calculator, although this is calculated in a slightly different way to the summary file - it might be more mesh sensitive
2. I would think that your Re at the inlet might need to be measured a little further into the pipe, once the flow is stable, what is the % difference then?
3. Same here, what is the % difference? The mesh will always have an effect here. Ideally two elements through any solid thickness, then you might need to run a mesh sensitivity study through the fluid also

Thanks,

Jon

[Anonymous]

Jon,

Thanks again for the feedback, I appreciate it!  So I did a bit of a mesh study, and put my results in the posted excel data sheet.  As far as the Re number goes, I am not to worried about that and it isn't a major deal in my study, so please disregard from here on.  For the tests, I ran a few runs at different mesh sizes, and it looks like the results are lining up well.  All test runs were ran to convergence.  I plan to maybe try a smaller mesh size run overnight.  The main data points I was looking at were outlet temperature on the inner tube surface, then the total heat flux from the inner tube volume (fluid) and the outer tube volume (copper tube).  

The temperature difference still exists between the sum file and the wall calculator.  If I go with the wall calculator temperature, this lines up very well with my hand calculations.  But the total heat flux does not, it lines up with the temperatures recorded in the sum file.  I guess I am just curious about the disconnect here.  I feel like the wall calculator total heat flux should line up with the wall calculator temperature difference, instead of the sum file temperature difference.  Any comments or feedback on this would be much appreciated!  And again, if you see anything incorrect with modeling approach, please let me know!

Regards,

William 

[Jon.Wilde]

Are you certain that your models are totally converged? I would turn off (or tighten) the convergence assessment (Solve -> Solution Control -> Advanced).

If your models are converging with fewer time steps with less elements, this is the opposite of what we would expect. I guess that CFD is stopping too early.

Usually with more elements, the change from iteration to iteration is smaller and CFD can stop too soon.

Once you have done this, what is your actual % difference between hand calc and CFD?

Also between sum file and CFD?

I also think that there was an issue with the .sum file back in 2015 - pretty sure you would see a closer match in CFD 2017 🙂

[Anonymous]

Jon,

I originally turned the auto convergence assessment for a mesh of 1, but around 1500 iterations I turned it back on and put the settings slider all the way to the tight side.  Didn't see much difference in this data compared to the previous runs.  My biggest concern is the temperatures given by the wall calculator do not make thermodynamic sense.  For example, in the first run the wall temperature boundary condition at the inlet was set at 60(F), and the wall calculator stated that the outlet surface temperature is around 99.5(F), but the wall calculator stated that the heat flux was around 355(Btu/h), which this cannot be.  In mass balances based off specific heat and enthalpy with those temperatures, the heat flux is around 394(Btu/h).  How is the wall calculator heat flux calculated?  

As far as % difference specifics go, the CFD average to the calculated average is around 10% or so for heat flux.  For temperature the CFD results are spot on with my hand calculator program.  I didn't look at the sum file since you said there were some problems with it :).  Please see the attached data sheet for reference.  Not sure if you have any other recommendations.  I could turn the auto convergence assessment off, not sure if it would stop running haha. The temperature lines up pretty well with my hand calculator, so I can continue my research with that and just ignore the heat flux.  But if you do have any other tips, that would be much appreciated!  Thanks for all your help so far.  Don't mean to keep bothering you with all these questions!

Regards,

William

[Anonymous]

Any thoughts on this?

[KubliJ]

Hi William,

The wall calculator uses nodal results.  And it can have problems with nodes on shared edges.  It can't determine what value of that nodal result is for the surface selected or the other surface.  This can throw off the values of the wall calculator.

You can try resid_bdry_force_calc to improve the wall calculator results.

Thanks,
James