CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Cross Flow Heat Exchager (http://www.cfd-online.com/Forums/star-ccm/100482-cross-flow-heat-exchager.html)

iDeew April 25, 2012 16:25

Cross Flow Heat Exchager
 
1 Attachment(s)
I'm new to Star CCM+ and want to simulate a cross flow heat exchanger.
Please look at the attached picture.
The steel tube carrying a turbulent flow of water and hot air flows upwards across this steel tube. I want to see how the water heats up. I can create the volume mesh of the three regions. But when I try to simulate Star CCM+ giving me errors.
Any help will be appreciated.
Thank you

LuckyTran April 25, 2012 23:43

Hi, first, is there any reason why you cannot just look up a correlation for Nusselt number of this configuration and then calculate the water temperature without using CFD?

iDeew April 26, 2012 10:28

Hi LuckyTran,

Thank you for your reply.
The outlet mustn't contain any steam. So the maximum water temperature shouldn't exceed 100C. IMO 90C would be a good value for the outlet water temperature.

Thank you

LuckyTran April 26, 2012 10:32

Quote:

Originally Posted by iDeew (Post 357214)
Hi LuckyTran,

Thank you for your reply.
The outlet mustn't contain any steam. So the maximum water temperature shouldn't exceed 100C. IMO 90C would be a good value for the outlet water temperature.

Thank you

So do you want to do the Star-CCM simulation or no? Personally I don't see any point to doing CFD on this problem, it is straightforward. Use the smooth pipe correlations for the inside of the pipe and flow over the cylinder outside to get htcs. Then you just apply an energy balances and you can get water and pipe temperature everywhere. Doing this would also let you change operating conditions easily, whereas in CFD it is costly, expensive, and does not provide any new data.

iDeew April 26, 2012 12:03

1 Attachment(s)
Hi LuckyTran,

This is a part of a big simulation. I think if I understand how to set up this problem in Star CCM+ it will resolve lot of thing in the full version.

Full version includes a 10'X10'X10' compact heat ex-changer and 320 propane burners underneath it. and every thing is covered by a insulated jacket and the a steel jacket with a chimney on top.

Thank You

LuckyTran April 26, 2012 12:40

Quote:

Originally Posted by iDeew (Post 357243)
Hi LuckyTran,

This is a part of a big simulation. I think if I understand how to set up this problem in Star CCM+ it will resolve lot of thing in the full version.

Full version includes a 10'X10'X10' compact heat ex-changer and 320 propane burners underneath it. and every thing is covered by a insulated jacket and the a steel jacket with a chimney on top.

Thank You

There are also correlations for tube bundles. Again, there is very little in your setup that does not already have an existing (well known, and well tried) correlation for the htc. There are even full-blown correlations for entire heat exchanger units like you have with an accuracy as good as 10%. You can find these correlations in undergraduate texts in introductory heat transfer, for more complicated correlations there are many many many heat transfer handbooks available for heat exchangers. I do not think you will learn much by doing a Star-CCM simulation and you most likely will not come up with any new physics that isn't already known. I just don't want you to mistakenly believe that you are doing something that has never been doing before. On the other hand, since the configuration is fairly common, you have a lot of literature to check your simulation against.

If you are still interested in doing the Star-CCM run, for the sake of learning to use Star-CCM or whatever then it is still a good learning opportunity. Can you give some details about what is having trouble converging? Is it diverging or just not converging well?

iDeew April 26, 2012 13:35

1 Attachment(s)
Hi,

I'm a engineering student just binning to learn CFD with Star CCM+.
I want to know if I created regions/interfaces correctly.

Thank you

rwryne April 26, 2012 13:54

Quote:

Originally Posted by iDeew (Post 357265)
Hi,

I'm a engineering student just binning to learn CFD with Star CCM+.
I want to know if I created regions/interfaces correctly.

Thank you

Hard to tell from just a screenshot, but I did ntoice your "steel tube" is set as a fluid region

iDeew April 26, 2012 16:51

2 Attachment(s)
Hi,
Thanks...Fixed it
Simulation ran without an error. :)
But output is not quiet what I expected. There is no temperature gradient in he water column!
And why can I see whats happening inside the metal tube.

Thank you

abdul099 April 28, 2012 07:38

Did you try any tutorial? There is a heated fin tutorial in the user guide. That should give you an idea how to set up a CHT case.

Run it for a larger number of iterations. I'm not sure due to the low screen resolution on my laptop, but I think it run for less than 100 iterations, right? Therefore you will most likely not have a converged flow and energy field and therefore you should not yet give a shit about the solution.

One reason why you can't see any temperature gradient is because it might be too low. Water has a quite big heat capacity, therefore putting the min and max temperature in the scalar displayer to the min and max values in your simulation usually means, the low temperature differences in the water will not be resolved with different colours. Put a narrower range to the scalar displayer, maybe you can see something in the water.

When you can't see anything in the steel tube, it's not covered by the plane section or the plane section is not included in the displayer (when there is a plane section for every region).

iDeew May 1, 2012 14:12

This is the sim file ,

https://docs.google.com/open?id=0B43...l93M1RXMHdpMUE

Thank you for your valuable time

abdul099 May 1, 2012 16:45

I will have a look on the sim-file in the next days. Today is too late to take care of your issue...

abdul099 May 7, 2012 17:46

Okay, now I had the chance to have a look on your model. Generally it looks fine, with just a few minor points and a bigger one.

The first point is: There coupled energy model wasn't activated in all physics continua. Was there any specific reason why you didn't choose it for all continua? That's necessary to solve the energy equation in all regions, or you will not have any heat exchange from the air to the solid and from the solid to the water.
Anyway, I activated that and then it worked fine.


There are unnecessary interfaces. You can delete the In-place 1 and In-place 2. Both are referencing a boundary which is already used for an interface.

Interfaces work the following way: You pick two boundaries, usually from different regions, and create an interface with them. Then the solver nows, some quantities (in this case, energy) can be transferred from one region to the other one by passing it through the interface.
When you run the simulation, the interfaces will be initializes. That means, the solver checks on one side for faces in contact with faces on the other side of the interface. Then faces from both sides will be matched and form a single contiguous mesh for all quantities able to pass the interface. For this step, all faces having a partner on the other side, will be moved to from the wall boundary the interface boundary. So when you've got a conformal match, the wall boundary will be empty (all faces are moved to the interface boundary) and the second interface created by you (with exactly the same boundaries) will be empty as well - there are just no faces in the wall boundary left to match for the second interface. Therefore you can delete the mentioned interfaces, it doesn't hurt.


One of the minor points also regards the coupled flow model. Is there a specific reason why you chose the coupled flow model instead of segregated flow? It's not wrong, but I think the segregated solver might be faster. The coupled solver needs too long until the flow field is established.
By the way, a better initialization would help a lot, and it's not to hard to get an idea for some of the values. For example, the average velocity of the water inside the tubes can easily be calculated from the inlet boundary condition, therefore it might be worth to enter that in the physics continuum.


Anyway, the rest of the simulation looks fine. The only reason why you couldn't see anything happening in the water is due to the big heat capacity of water. The water doesn't heat up much, so you need to specify a narrower range for the scenes. And you also need to solve a little more than this 54 iterations one can see in one of your pictures. It takes some time until you've got a nice, converged solution.
Maybe you can use a smaller mesh. The mesh itself is fine, but it takes long to solve. You can learn the principles on a smaller mesh and have some quick results to see how it works.


I also recommend to create some reports / plots monitoring the mass flow averaged outlet temperature of water and air. That will give you an idea about convergence. As long as the temperatures haven't stabilized, you should keep on solving. That should be done in nearly every simulation since you can't really rely on residuals only.

iDeew May 7, 2012 18:46

Thank you so much for your reply and your precious time spending on me.
I'm still learning Star CCM+. Your reply is so informative & better than any of the heat exchange tutorials comes with Star CCM.
I'll do all the modifications you mentioned and let you know the progress.

Thank you again.
:):):):):):):):):)

iDeew May 9, 2012 15:48

3 Attachment(s)
It worked. I can see temperatures in all regions now.
I have another problem. When I draw streamlines, water doesn't seem to go through the tube (Direction of the blue arrow). Any ides??

Thank you

rwryne May 10, 2012 08:33

Quote:

Originally Posted by iDeew (Post 360167)
It worked. I can see temperatures in all regions now.
I have another problem. When I draw streamlines, water doesn't seem to go through the tube (Direction of the blue arrow). Any ides??

Thank you


Did you check your outlet boundary? Maybe something is wrong with it.

abdul099 May 10, 2012 17:24

How long did you run it? It takes some time (especially when using the coupled solver) until the flow field has established.
The model you put the link here looks fine when you run it long enough (and of course, activate energy solvers for all continua etc, like mentioned before).

But I just realized, the flow rate is very low. The water will need several minutes to pass the pipe, therefore it will heat up very much. Most probably boiling would occur in the pipe with this boundary condition. Are you sure, all values are right?

iDeew May 17, 2012 14:15

1 Attachment(s)
I let it run 1000 iterations. Outlet conditions are good.

I'm experiencing another problem. See the below error massage.,
This happens when I apply Coupled Energy to Steel tube.Do I need to add Coupled energy Physics to Water side too?

Thank you

abdul099 May 20, 2012 18:41

Yes. For a CHT case like yours, you want to solve the energy equation in all regions. Therefore you need to switch on coupled energy in ALL physics continua.

OR stick to the segregated solver, but then you need to switch to the segregated solver including segregated energy in all physics continua.

iDeew May 21, 2012 13:42

4 Attachment(s)
I changed all physics continua to Segregated solver. But Star CCM still gives me an incompatible error ?

I have attached the three continua & the error massage..

Thank you


All times are GMT -4. The time now is 11:08.