CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Simulation of heat transfer (http://www.cfd-online.com/Forums/cfx/115199-simulation-heat-transfer.html)

Clay March 26, 2013 01:01

Simulation of heat transfer
 
I am trying to simulate heat transfer for a plate heat exchanger. However, I am new at CFX. My result turn out to have no heat transfer. The parameters for the simulation must be wrong. Any help from you guys is much appreciated.

ghorrocks March 26, 2013 05:14

This sounds like a simply conjugate heat transfer simulation. Have you done the tutorials?

And if you get no heat transfer either:
* Your interfaces are not connected
* You have not run the simulation long enough for the heat flow to start up.

jthiakz March 26, 2013 06:22

CHT case setup details are required ...

Clay March 26, 2013 10:12

ERROR #004100008 has occurred in subroutine FINDL.
Message:
Insufficient space for array LNOD.

is this because the poor performance of PC?

There are heat transferred when i set the boundary condition of the interface with temperature.
But what i want to do is to let the heat transfer from the fluid domain.
By tutorial, do you mean the one with heating coil?

ghorrocks March 26, 2013 17:47

This is an unusual error and almost certainly caused by a problem in the way you set it up. But if you want any help you will need to post an image of what you are modelling and the CCL.

All tutorials are useful, but the ones with solid heat transfer especially so in this case.

Clay March 27, 2013 05:30

I have tried running it with my lab's PC. This is a simple version i tried to run before using the real model. The simple version only consists of two fluid region and a plate between them. There are heat transfer. There are temperature difference at the both outlets. But the temperature contour inside the plate seems to be constant. Is this correct? I was following a tutorial where they use air ideal gas as the fluid. In my case, I'm using water. Should i include the buoyancy?
Here are the results.
https://www.dropbox.com/s/j45yrjaw5e4108t/hotfluid.jpg
https://www.dropbox.com/s/k3jp7yuflww41tx/inout.jpg
https://www.dropbox.com/s/7oee9w44bhrczpq/platetemp.jpg

ghorrocks March 27, 2013 07:10

Based on the small amount of information you have provided I have no idea whether what you are seeing is real or not. If the thermal conductivity of the plate is high relative to the fluid then you would expect to see only small temperature gradients across the plate - in this case the effect could be real.

Alternately, if you have not set the interfaces up correctly then no heat transfer will occur.

Please post your output file and/or the CCL as attachments.

jthiakz March 27, 2013 07:17

# Check the Pr number for water and oil based on that fix near the wall mesh (heating surface) wher you'll have more temp gradient.
# check the material details, K
# check the turbulence model, it is better to you SST- KW
# Is interface area between fluid to solid are same, Pls show the interface area comparison
# Pls show the mesh cut section..

Clay March 28, 2013 01:02

Quote:

Originally Posted by hoahongtim0907 (Post 416722)
lĂȘn nĂ*o.............................................. .................................................. .....................

I do not understand you...

Clay March 28, 2013 01:21

Quote:

Originally Posted by ghorrocks (Post 416693)
Based on the small amount of information you have provided I have no idea whether what you are seeing is real or not. If the thermal conductivity of the plate is high relative to the fluid then you would expect to see only small temperature gradients across the plate - in this case the effect could be real.

Alternately, if you have not set the interfaces up correctly then no heat transfer will occur.

Please post your output file and/or the CCL as attachments.

I am not sure which one is the output file. Here is the CCL. What information should i provide? Because I'm still kind of new in CFX. Thank you for your patience.
https://www.dropbox.com/s/nxbs3jk0xtv5014/simplePHE.ccl

Clay March 28, 2013 01:28

Quote:

Originally Posted by jthiakz (Post 416695)
# Check the Pr number for water and oil based on that fix near the wall mesh (heating surface) wher you'll have more temp gradient.
# check the material details, K
# check the turbulence model, it is better to you SST- KW
# Is interface area between fluid to solid are same, Pls show the interface area comparison
# Pls show the mesh cut section..

how do i check the Pr number, material details and turbulence model?

Here is the meshing cut section.
https://www.dropbox.com/s/nm0oef9x6onpqsd/meshing.jpg

Clay March 28, 2013 01:44

I changed the fluid from air ideal gas to water. Should buoyancy be included, if so what is the buoyancy reference temperature for water?
The result of using water is different with the air ideal gas. No temperature change in the fluid. I used the same setting.

jthiakz March 28, 2013 03:43

#solid domain mesh is ok
# Pr number check this link, http://en.wikipedia.org/wiki/Prandtl_number, I mean to say that Pr less ,thermal diffusion is dominant than momentum. so Thermal BL is thicker than Momentum Boundary Layer.so you need prism mesh there. Now you are not having prism mesh, so the sharp temp grad near wall cannot be captured.
Create 10 layer prism mesh on fluid side interface walls (for both fluids), first cell height =0.001mm , growth ratio =1.3
# For buoyancy ref density in single phase flow. you can give far field density (unaffected density). In your case, check the density at inlet and same value use it for ref.density.
# But before doing all of this, pls make sure that the interface area (contact area) of fluid & solid are equal and update us value of it.
# Fluid time step =0.01s, solid domain =0.1s, update the convergence plot

Clay March 28, 2013 04:11

Quote:

Originally Posted by jthiakz (Post 416899)
#solid domain mesh is ok
# Pr number check this link, http://en.wikipedia.org/wiki/Prandtl_number, I mean to say that Pr less ,thermal diffusion is dominant than momentum. so Thermal BL is thicker than Momentum Boundary Layer.so you need prism mesh there. Now you are not having prism mesh, so the sharp temp grad near wall cannot be captured.
Create 10 layer prism mesh on fluid side interface walls (for both fluids), first cell height =0.001mm , growth ratio =1.3
# For buoyancy ref density in single phase flow. you can give far field density (unaffected density). In your case, check the density at inlet and same value use it for ref.density.
# But before doing all of this, pls make sure that the interface area (contact area) of fluid & solid are equal and update us value of it.
# Fluid time step =0.01s, solid domain =0.1s, update the convergence plot

Should i continue with this simple version of PHE or just go for the real model? The real model consists of much more plates with corrugations on it. The auto fluid-solid interface domain is not working, it seems impossible to select one by one out of so many surfaces.
And for water, there are only option to fill in buoyancy reference temperature and not density.

jthiakz March 28, 2013 04:20

Quote:

Originally Posted by Clay (Post 416904)
.
And for water, there are only option to fill in buoyancy reference temperature and not density.

yes , because for water (liquid), boussinesq model is used, so you can specify inlet liquid temp as ref temp.

Clay March 28, 2013 04:38

Quote:

Originally Posted by jthiakz (Post 416908)
yes , because for water (liquid), boussinesq model is used, so you can specify inlet liquid temp as ref temp.

Thanks, I am trying to run it again. Added inflation for the prism layer. Does the number of iteration affect much? And for mesh connection, i used GGI.

jthiakz March 28, 2013 04:44

# when you make the case setup, include temp monitor points in all the 3 domains
# run the case and first check the mass, mom,energy convergence levels and then check the monitor plots.
# Ideally Last 100 iteration(min) residual, monitor plot values should not change much
# pls show the residual plot

oj.bulmer March 28, 2013 08:34

Quote:

yes , because for water (liquid), boussinesq model is used, so you can specify inlet liquid temp as ref temp.
Typically, the reference temperature for Boussinesq approaximation should be volume averaged temperature, not region specific, to make it relevant to all parts of the domain.


Quote:

yes , because for water (liquid), boussinesq model is used, so you can specify inlet liquid temp as ref temp.
Boussinesq approximation is a faster way to achieve convergence in natural convection, using steady state physics, since the density is constant in all governing equations, except the buoyant term in momentum equations - where it is an empirical function of temperature difference and thermal expansion. But this only applies when temperature differences in the domain are smaller. The plots in attached snap show a wide range of temperatures.

I wonder, is it even appropriate to use Boussinesq approximation here?

OJ

Clay March 31, 2013 02:37

Quote:

Originally Posted by jthiakz (Post 416913)
# when you make the case setup, include temp monitor points in all the 3 domains
# run the case and first check the mass, mom,energy convergence levels and then check the monitor plots.
# Ideally Last 100 iteration(min) residual, monitor plot values should not change much
# pls show the residual plot

here are the results.
anything else need to be included?
https://www.dropbox.com/s/pyighpurgozndw9/coldfluid.jpg
https://www.dropbox.com/s/jmov3e3r0f7b7lj/hotfluid.jpg
https://www.dropbox.com/s/93mlt8zdkykvo5l/platetemp.jpg
https://www.dropbox.com/s/ezlhjkc5kwaxva7/meshing.jpg
https://www.dropbox.com/s/trw9njxsvy...attransfer.jpg
https://www.dropbox.com/s/pjsk59t4334km9x/momentum1.jpg
https://www.dropbox.com/s/ikx3sefp8dwkoew/momentum2.jpg
https://www.dropbox.com/s/uib8qv8pw2...ransfermax.jpg
https://www.dropbox.com/s/nk6c5rnqs5...mentum1max.jpg
https://www.dropbox.com/s/94rrxf1l00...mentum2max.jpg

Clay April 4, 2013 00:36

help? anyone...


All times are GMT -4. The time now is 08:34.