[sieginc.]

I have a simple model of an air duct with a heat generating cube being cooled by convection. I've posted quite a bit about this project since I'm still learning star-ccm. One problem I'm having now is that I'm trying to simulate the heat transfer between the cube and the duct wall.

The first few iterations of the simulation appear normal:



However, after a while something strange starts to happen and I end up with something like this:



Things just seem to go haywire. There is no heat being generated at those points, which it doesn't make sense to me why there are those "hot spots" with blown up temperature values. I even turned off the heat generation, and ran the sim and these hot regions still appeared out of nowhere. The energy residual does not converge. My energy source comes from the interfaces on the inside of my cube:



It is a relatively low heat flux too. I have interface contacts between the cube base and the duct, as well as everywhere where there is a fluid/solid contact between the air region and duct wall + cube walls.

The models I am using are as follows:

Air - Constanty density, gas, high y+ wall treatment, k-epsilon turbulence, reynolds averaged navier stokes, segregated flow, segregated fluid temp, steady, three dimensional, turbulent

Cube - Constant density, segregated solid energy, solid, steady, three dimensional

Duct - Same as cube

What could be the cause of this phenomena? Here is a link to the sim file to play around with. It's all set up, but a volume mesh has to be generated and then the sim can be run.

http://www.sendspace.com/file/4hjbjg

[flotus1]

What type of cells does your mesh contain? Hex, Tet or Poly?

And which interpolation method do you use for the computation of the convective fluxes? Upwind? Central differences?

[sieginc.]

Mesh is filled with polyhedral cells. As for the interpolation method, where do I view this? I tried switching between segregated to coupled but that had no affect, same problem.

If the outermost surface of my model is a solid, and heat is beating dissipated out of it, do I need to enclose my duct within a larger fluid region representing the "room" the duct is in?

[flotus1]

Originally Posted by sieginc.

Mesh is filled with polyhedral cells

Since your geometry contains only rectangular elements, you should try to use the "trimmer" meshing method provided by ccm+. This will result in a hex-mesh which is superior in quality and computational cost to any polyhedral mesh. Do not forget to resolve the boundary layer, since this is essential for heat transfer calculations.
Maybe you could upload a screenshot of your mesh.

As for the interpolation method, where do I view this?

I am sorry, but right now i dont have access to ccm+. But the default setting should not cause the instabilities you observe.
Edit: there it is: pyhsics - segregated flow - convection
Choose 1st order ONLY if you cannot get convergence with one of the higher order schemes. Try achieving your final simulation with one of the higher order schemes.

I tried switching between segregated to coupled but that had no affect, same problem.

Keep it segregated, no need for a coupled approach here.

If the outermost surface of my model is a solid, and heat is beating dissipated out of it, do I need to enclose my duct within a larger fluid region representing the "room" the duct is in?

No. in fact, I would not even model the solid wall explicitly. Just model it as a thin surface. Again i cant tell exactly where to find this in ccm+, but it should be somewhere in the boundary conditions.
Same thing with the cube. Just put a temperature or heat flux boundary condition instead of modeling the solid.

In general, you could start your simulation without heat transfer to obtain the approximate flow field. Initialize the final simulation from this computation.

[sieginc.]

Originally Posted by flotus1

Since your geometry contains only rectangular elements, you should try to use the "trimmer" meshing method provided by ccm+. This will result in a hex-mesh which is superior in quality and computational cost to any polyhedral mesh. Do not forget to resolve the boundary layer, since this is essential for heat transfer calculations.
Maybe you could upload a screenshot of your mesh.

I am sorry, but right now i dont have access to ccm+. But the default setting should not cause the instabilities you observe.
Edit: there it is: pyhsics - segregated flow - convection
Choose 1st order ONLY if you cannot get convergence with one of the higher order schemes. Try achieving your final simulation with one of the higher order schemes.

Keep it segregated, no need for a coupled approach here.

No. in fact, I would not even model the solid wall explicitly. Just model it as a thin surface. Again i cant tell exactly where to find this in ccm+, but it should be somewhere in the boundary conditions.
Same thing with the cube. Just put a temperature or heat flux boundary condition instead of modeling the solid.

In general, you could start your simulation without heat transfer to obtain the approximate flow field. Initialize the final simulation from this computation.

I've tried using the trimmer before and it gives me an error stating the trimmer cannot mesh multiple regions.

The outer solid duct wall is very thin, approximately 0.063". I will upload the mesh when I get a chance, but doesn't this seem more like a physics error than a meshing one? I attempted to use the thin mesher on the outer walls but received an error, I'll describe it once I get a chance to run the sim again. I appreciate your help.

[flotus1]

OK, so no multiple regions for the trimmer mesh. Sorry I forgot about that.
But this would be one more reason to cancel the conjugate heat transfer simulation and use "normal" boundary conditions (walls) for the fluid instead.
Or use another software for grid generation, ICEM for example could get the job done in 15 minutes.

I cannot really tell if it is a meshing or a setup error without seeing either of it. But I already ran simulations in ccm+ with poor mesh qualities which resulted in flow variables getting out of the physical range as they do in your simulation.
Of course there could still be some mistakes in the setup.

[sieginc.]

Originally Posted by flotus1

OK, so no multiple regions for the trimmer mesh. Sorry I forgot about that.
But this would be one more reason to cancel the conjugate heat transfer simulation and use "normal" boundary conditions (walls) for the fluid instead.
Or use another software for grid generation, ICEM for example could get the job done in 15 minutes.

I cannot really tell if it is a meshing or a setup error without seeing either of it. But I already ran simulations in ccm+ with poor mesh qualities which resulted in flow variables getting out of the physical range as they do in your simulation.
Of course there could still be some mistakes in the setup.

If you have access to ccm+, I included a download link to my sim file at the end of the first post. I don't know if you have the time or not to take a look at it but it's there. All that needs to be done is generate a volume mesh, and then run it. You will see the errors I'm talking about very quickly.

[flotus1]

Sorry but I don't have access to CCM+ anymore.

[sieginc.]

Anyone else have any ideas? Thanks in advance.

[abdul099]

Originally Posted by sieginc.

I've tried using the trimmer before and it gives me an error stating the trimmer cannot mesh multiple regions.

That's partially right. The trimmer can't mesh multiple regions AT THE SAME TIME. It would work when you tick "per-region meshing" in the mesh continuum. However, for a CHT case I would stick to the polyhedral mesher since it can give you a conformal matching while the trimmer can't. But when you follow flotus1's hints, you might not have a CHT case and therefore the trimmer would be the first choice.
And as flotus1 said, as long as you don't explicitly need the duct solid, don't mesh and solve it! It causes a lot of trouble or a lot of cells (causing a lot of trouble) to mesh a thin geometry!

Originally Posted by sieginc.

If the outermost surface of my model is a solid, and heat is beating dissipated out of it, do I need to enclose my duct within a larger fluid region representing the "room" the duct is in?

Well, let's think a little more about this: Don't you need to model the walls enclosing the "room" the duct is in? And the air surrounding the room the walls surrounding the "room" the duct is in? And the rest of the atmosphere? And what about the rest of our solar system? The milky way? The local group? etc...
You only need to model what you're interested in and what affects your solution. Of course, a butterflies wing stroke in China might affect the temperature of your block in America or Europe or Africa or on the moon - but you will not be able to measure it, so I assume, you would ignore it. Also the air outside the room and the walls of the room will not cause a significant difference in your case since you're only interested in the heat dissipating to the air inside the duct. Therefore the walls of the duct can be modeled as a convection or temperature boundary, and I'm pretty sure, the difference will not be significant as long as you chose reasonable boundary conditions.

Originally Posted by sieginc.

... but doesn't this seem more like a physics error than a meshing one?

Maybe, but that's not proven. There are three options. Either:
- You've put right physics settings on a crap mesh
- or you've put crap physics settings on a good mesh
- or you've put crap physics settings on a crap mesh.
All other combinations should end up with a good solution.

I've donwloaded your sim-file and meshed it. The I tried to solve it, and the first message was "Warning: 1 cell in region Assembly 1.SolidDuct has zero or negative volume.". That means: Your mesh is crap. Not just crap but really crap. And guess what's causing the trouble? Right, it's the thin duct geometry!
When I create a section with a normal in Z-direction and look at the mesh in this section, I nearly get eye cancer immediately! It's not the worst mesh I've ever seen, but I'm sorry I have to say that, it is far away from being a suitable mesh.

When you need to mesh a thin geometry, you need to make sure, cells can get small enough to fit into the volume. In your case, the duct region is approx. 1.5mm thick. The cells are very flat, just to fit into the volume, since the minimum surface size is more than 6mm. And there are even two prism layers on ever side of the solid. No way, the mesher will not manage to create a suitable mesh with this settings.
Just imagine, you've got nearly sphere shaped objects to be put into a box. Let's say, some soccer balls. A sphere shaped ball has a perfect shape, just like a perfect (more or less sphere shaped) polyhedral. No think about a very flat box, just 5cm high. Will you be able to squeeze a soccer ball inside? And if so, will it still have a perfect, nearly spherical shape? No. So what can you do? Make the soccer balls smaller. Put baseballs inside. Or table tennis balls. Or throw the box away and go out for a drink and tell your friend "I don't need the box anymore since I can model the behaviour of my living room without taking a box of soccer balls into account".

Keep in mind: The "thickness to cell size" ratio might be one of the things causing your initial issue: Your mesh quality is too bad, causing the solver to diverge. The other thing could the the innermost air block. A totally enclosed air volume when running an incompressible flow is something the solver can't handle. There can be some mass imbalance due to round off errors, so the continuity equation is not satisfied. When the solver tries to correct this, it's getting worse with every iteration. So get rid of this air volume or run a compressible case.
You wouldn't have temperatures of -146C and 4700C in the same simulation when the mesh and the setup would be good. I still think, it's the cell quality, but you should look for both hints. And even when I'm wrong, it's NEVER wrong to have a good cell quality.

Further, your mesh is very small. There's no rule of thumb how big a good mesh needs to be, that depends very much on the geometry and the complexity of the whole case. But a mesh with only 200 000 cells for a complex geometry is always suspicious since it's very small. Like a car with 10 horse powers. Although there is no rule of thumb how many horse powers a car needs to have, everybody would investigate further when somebody tells, there's a car with 10 horse powers - just because the number is too low.
In your case the low cell count is related to the "too big" mesh values.

So let's make a long story short: My conclusion is to get rid of the solid duct geometry as long as it is not essential. Maybe it's possible to assume a constant temperature for the duct. Or you can assume some convection boundary condition. Think what's happening on the outer duct surface and how it will affect what's happening at your block.
When it's not possible to get rid of your duct, mesh it with better mesh values. In this case, better means "smaller mesh values". That will increase your cell count and therefore increase the solution time. It will take more time to mesh and solve and postprocess. But don't worry, that's how CFD works. You usually need to wait some time for results. Real cases use to be big and uncomfortable to handle, that's why some companies make good money with selling clusters (and others make good money with selling electricity for the clusters).

Now there are only two things left to write:
First, I'm sorry for using the word "crap" so often. But it was necessary since what I've wrote it is fact.
Second, I wish you good luck with your case. And of course, you will get further assistance when needed.

And by the way, I don't have version 6.04 on my machine and I will not install it. But when you have version 7.02 available, I might be able to send you the sim-file with some better settings.

[sieginc.]

The duct walls need to stay since the sim is being compared to a physical test set up. Insulating the cube in the set up would be too much of a pain so I'd rather take into account the heat losses in the sim. If I don't, the temps near the cube base will be higher in the sim since the base in the setup acts as a fin. I don't think the inner air pocket is the cause because I had it there in a previous sim where I only had the fluid region but not the solid outer walls and it worked just fine. I guess that means it's the mesh. I actually just got access to 7.02 so if you want to send me that file I would appreciate it.

Update: Well after switching to the trimmer, it seems to be working better now. The energy residual converges and I don't get crazy temperature values. However, the temperatures are about
20 C lower than what has been measured in the physical test set up. When I had the floor adiabatic, I just lowered the heat flux equivalent to what was being lost in the real test, and the values were almost spot on (save for the temps around the cube base which is why I wanted to include the heat transfer between the cube and the floor). All the physics are exactly the same, 50 W total power, 20 CFM flow rate, same geometric specifications on everything... I thought the culprit might be the contact resistance between the solid/solid interface between the cube and floor, but after toying with it it didn't seem to affect anything. Is there any way I can define a clearance between the cube and duct? I think in the test set up there is not a perfect contact. Also, is it normal for a CHT simulation to take REALLY long to converge? Before it was under 1k iterations, now it's over 4k and the temps still quite haven't flattened out.

[abdul099]

I'm sorry I didn't find the time yet to send you the sim-file. I'll do it Sunday evening...