Well, that's an easy one. You just need to read my last post more carefully. :D

It is a CHT case. That means, you try to take the energy exchange between the regions into account. This is because you want energy to be transferred from the air to the solid and from the solid to the water. Therefore you need to solve the energy equation in ALL regions. So far, so good.
But all regions means in the air region, the solid region AND also in the water region. In your setup, there is no energy solver switched on for the water region, so there will no energy equation be solved in the water.

No matter if you're using the segregated or coupled solver (both is fine, although I usually prefer the segregated one due to hardware requirements). But you NEED to switch on an energy solver in EVERY physics continuum!

The error message points to that. It says, the issue can be found on the contact interface between the water and the solid. It says, the solid energy model is incompatible with the model on the other side. So it needs to be in the model choice dialog. Either a wrong model, or a missing model. In your case, it's a missing one.

Yeah
 

Ok now I can see the steel and water, Great..
below is all the 3 physics models I'm using now...

But I still don't see any change in temperature in steel or water!
Air inlet, velocity=1m/s & temperature =1000 C

Another question...Check picture 1.JPG....
there are gaps in between regions!! , which is only visible when you zoom the model...are they causing any problems?

Thank you

Again I have to say "that has already been answered" :D

You have set the scalar displayer showing the temperature to a range from 300K to 1000K. :eek: That is too much to show the small temperature rise in the water region.

You've got I think 32 colours in your colour bar by default. So every colour stands for a range of nearly 22K. When your water doesn't heat up for more than this 22K, you will not be able to see anything, just due to the resolution of your colour bar.
Now consider, water has a very high heat capacity. Your gas cools down by just a few 100K, so the water doesn't heat up very much, and you just don't see the water heating up, although in fact it does heat up.
You can adjust the range to something like 300K to 350K, and you should be able to see the water heating up. You can also clip all above the max temperature, so you don't see all the gas in red. You can even add a second scalar displayer with a different colour scheme (e.g. black-white). One is showing a plane section in the water, the other one a plane section in the solid and gas regions. Then you can set an appropriate range to both displayers independently, showing the results with the best resolution for all regions.

By the way, when you want to set the inlet condition to 1000 degrees centigrade, what I assume from your last post, you should correct the inlet temperature. It is set to 1000 Kelvin.

Regarding the gaps: Check the output for the interface matching. When it's a conformal match, don't worry about the gaps, it might be a display issue. If not, you will get a percentage. Then you should check it more carefully what's going on and give a little more information.
I don't have your model open right now. Maybe I will have a look on your model again later this weekend. I will let you know what's going on.

In the third figure from left, there is no energy model added. please add an energy model from the list, such as segregated fluid temperature, then it should give no error.
good luck

abdul099,
What did you mean by "Check the output for the interface matching"?

Thanks

Right click on your interface tree and hit re-initialize. Then watch the output window, you want it to say "conformal match" for all interfaces. A bad result would be "98% conformal" or something similar.

I don't see a re-initialize on the right click menu...!
Below is the output when I click Reset-All & Initialize

I think rwryne meant Reset & Initialize. That's what one might shortcut with re-initialize.

I just had a look on your sim-file. You're using a trimmed mesh, so you will not get a conformal match. But don't worry, you've got a 100% match and there are no faces left in the wall boundary. So you have a nearly perfect interface.
The "gaps" are just a matter of mesh resolution and face orientation. You can clearly see that when you display the mesh. That doesn't affect the solution since you have a 100% matching, so it's just a display issue.

Yup.....I usually check these thigns to get the wording right, but the .sim I have open doesnt have interfaces so I took a guess.

shows what happens when you assume!

ok...this is what the simulation looks like now
Any ideas about the strange behavior happening in the middle of the tube

How long did you run it? Are you sure, it is already converged?

1000 iterations

Thank you

Don't rely only on residuals to judge convergence. You should also look on some other plots, e.g. average outlet temperature, boundary heat transfer etc.
Also have a look on the scene while iterating. When it still changes, keep on iterating. But don't abort it too quick when it "does not change". Maybe the change from one iteration to the next is just too small to see it.

I would try to run it for some more iterations, for me it looks like the flow field hasn't reached it's steady state. Don't worry when it takes several 1000 iterations until the solution is converged, sometimes it takes very long.

After 5000 iterations it still looks unsteady..!

Thanks

But the picture has changed. It is not yet converged! When you "extrapolate" the change, it should sometime look nice.
And as I said in my last post: "Don't worry when it takes several 1000 iterations until the solution is converged, sometimes it takes very long."
I had some cases, a simple pipe (noncircular cross section), and it took 20 000 iterations until a steady behaviour had established.

But what just flashed across my mind: Do you still run with the segregated solver or have you switched back to the coupled solver?

ok I'll let it run....

I'm using segregated flow.

Thank you

Hm, weird. Did you reduce under relaxation factors?
Let it run for some iterations and keep us informed about the result.

Below picture shows 30k iterations.

I did not change relaxation factor

Thanks

Is it still the same model you had at the beginning of the thread? I run the model I got from you for 1000 iterations ish, and it looks fine. Did you change anything in the meantime?

problem in defining the region and boundary condition defination
 

hi,

i am working on the problem on heat transfer through the wavy pipe in star ccm+ i have attached the geometry of it. I am confused in defining the region. if i import my geometry as surface mesh and split my surfaces into three part then inlet outlet and wall.then i have also specified the constant wall temperature on the wall and applied the inlet temperature and velocity through the fluid which is less then that of the wall i.e the heat transfer takes place from wall to the flowing fluid. but when i see the outlet condition the solver has automatically specified the the outlet temp as 300 k:confused: which i don't require since the i want to know the outlet temperature only if i prespecify this then my physics of the problem is wrong.:confused::confused:Attachment 16529