[Phili]

Hello everyone,

for a research at university I need to simulate heat transfer / heat loss in an exhaust manifold using CFX / Ansys Mechanical (I'm interested in how much heat is lost in the exhaust manifold for efficiency calculations for a turbocharger).

I've read many tutorials about simulating heat transfer and most stated, that heat transfer can be simulated by using a multi domain interface (fluid domain and solid domain, linked by a fluid-solid-interface).
My problem is, that I have an existing mesh of the geometry, that only uses the fluid domain.
Is it possible to simulate heat transfer, by doing a CFD analysis of the fluid domain and importing the temperature loads at the wall to Ansys Mechanical?
I hope you get what I mean.

Since I'm quite new to CFX, any help is appreciated!

Greetings
Phili

[ghorrocks]

Let's cover some basics: What is a boundary condition? It is a boundary of your simulation domain where you can describe mathematically what is going on. So do you know mathematically what is going on at the wall boundary of the fluid (inner wall of the pipe)? If not then let's step one step out - do you know mathematically what is going on at the outer wall of the pipe? If you still cannot describe it then you need to go further out - out to the air surrounding it where I presume you can say the air is at ambient temperature.

[Phili]

Yeah, since I want to validate my simulation with experimental results from a test bench, I know the temperature of the surrounding air.

[ghorrocks]

In that case you need to model the exhaust gas in the pipe, the pipe, and the surrounding air to as far out as you need to go to define a realistic boundary condition.

You will find this sort of simulation is, for most people, unmanagable. So let's be a little smarter about this.

Do you have measurements of the outside temperature of the pipe? If so then you can use this as a fixed temperature boundary of the exhaust pipe outer wall - and then you have no need to model the surrounding air.

Alternately, you could apply the measured exhaust temperature to the wall of the exhaust gas (so the inner wall of the pipe). Then you have no need to model the exhaust pipe metal.

[Phili]

I do have measurements of the outside temperature of the pipe for a few operating points but I'm not allowed to use them for my simulation. They're just intented to be a validation for my simulation.
What I want to do in the end is simulating a whole engine map (or at least various operating points) in order to have an overview of the various losses of heat/energy.
That's why I can't use the temperatures as a boundary condition.

Furthermore I can't simply apply the exhaust gas temperatures to the inner wall of the pipe, because the wall temperature varies with the location.

[stumpy]

You can model just the fluid region in CFX and guess at the wall temperature. Export the HTC (Convection Coeff) to a text file then import this into Mechanical via External Data. Solve the Mechanical model, export wall temperature and update your fluid wall boundary condition. Repeat until you have converged the HTC and wall temperature. It would be MUCH easier to just solve the solid region in CFX and get a solution in a single step.

[Phili]

Yeah I share your opinion that it would be much easier to simulate the fluid and solid domain in CFX. Unfortunately we've to use the existing meshes which only contain the inlet, outlet and wall.

[ghorrocks]

The complexity of this simulation will be in the different time scales acting. The exhaust gas flows in big pulses and has wide temperature variations over the engine cycle. So to resolve this you are going to need time steps small enough to resolve the engine cycle. But the time scales of the pipe metal and surrounding air flow will be far slower. This is why I say this is an unmanagable simulation for most people.

Decoupling the fast time scale to long time scale components will greatly assist you. Stumpy's suggestion is one way to do this.

[Phili]

Originally Posted by stumpy

You can model just the fluid region in CFX and guess at the wall temperature. Export the HTC (Convection Coeff) to a text file then import this into Mechanical via External Data. Solve the Mechanical model, export wall temperature and update your fluid wall boundary condition. Repeat until you have converged the HTC and wall temperature. It would be MUCH easier to just solve the solid region in CFX and get a solution in a single step.

After discussing some possibilities, I gonna have to try your approach.

Just to be sure I understood it correctly:

Let's say my exhaust gas has a temperature of X.
I simulate the fluid region in CFX, with the wall boundary condition set to a strict wall temperature of Y.
Then I import the simulated HTC into my mechanical model in order to solve it and get wall temperatures as a result (what about other BC's such as radiation from the metal to the surrounding air?).
Then I use these new wall temperatures for my "strict temperature" wall boundary condition.
I repeat until I've converged the HTC and then do a final simulation with that HTC?

Thanks in advance!

[ghorrocks]

But Stumpy's final sentence is relevant - "It would be MUCH easier to just solve the solid region in CFX and get a solution in a single step." So why not just model the pipe as a solid region in a CHT model in CFX. Then you get it in go, rather than having to iterate between two simulations.

And yes, radiation is important. If you do not include it you will be miles off. But your decision is whether a simple radiative heat transfer boundary (done using a CEL expression with the Boltzmann constant and T^4 and all the rest) is adequate or whether a full radiation model is required. As long as nothing too hot or too reflective is in the surrounding regions then the simple approach should be OK.

So I would put a combined radiation and convection boundary on the outside wall of the pipe. You can do this by using a heat flux boundary, and defining the heat flux as a CEL expression, with the sum of the convective and radiative heat transfer components. I have done this with similar hot pipe simulations and it works well.

[Phili]

As I said, I would like to do it like that, but since I'm doing the simulation as part of a university project, I'm not allowed to... -.-

As for the radiation, the simple approach should be fine I guess, since I'm simulating a "test bed kindish" environment.

I guess I'll try that and keep you guys updated!

[ghorrocks]

Not allowed to do what? There is nothing in the model I just described where you assume the measurements. Let me explain it again.

The exhaust gas is in its fluid domain. There is a solid/fluid interface to link to the exhaust pipe wall which is modelled as a solid. There are no assumptions on this interface, just let the solver find the conditions present. On the outside of the exhaust pipe wall use a combined convection/radiation boundary. You will need to generate your own CEL to do this (it is not a built in boundary condition) so use a heat flux boundary, with the heat flux set to the sum of the convective component (h(T-Ta) where h is a reasonable convection coefficient, T is the temperature solver variable and Ta is your ambient temperature, maybe 25C) and the radiative component (s*e(T^4-Ta^4) where s is the Stefan-Boltzmann coeff, e is emissivity, and T and Ta are as before).

See? The measured values are not used anywhere. The only tuneable inputs are the ambient temperature and the exhaust pipe emissivity. If this is for a university assignment I hope I get some marks for that.

[Phili]

I get your point. My problem is that I have to use the existing mesh, that I've gotten as part of the assignment.
In the mesh, only the fluid domain is modeled (basically like e.g. in the InjectMixer tutorial).
So in order to do the simulation the way you suggested, I would have to apply changes to the existing mesh (or am I missing something)?
And that's exactly what I'm not allowed to - don't ask me why...

[ghorrocks]

OK, it you cannot add mesh for a solid for the pipe then ignore it. It probably did not do much anyway, just reaches a equilibrium.

The apply the combined convection/radiation condition to the outside of the fluid domain as a heat flux.

[Phili]

Btw, what are your experiences on theoretically calculating HTCs, using Gnielinski correlation, Dittus-Boelter equation etc?

[ghorrocks]

I have never used any of those methods and cannot comment on their effectiveness. I have a table of standard HTCs for typical conditions and I use that (from Incropera and DeWitt, Fundamentals of Heat and Mass Transfer).

[stumpy]

Yes, the approach you outlined (on March 28th) is exactly what I meant. You asked about radiation boundary condition. On the CFX side you can include radiation in the domain. A simple model such as P1 should be OK since the exhaust gases will be optically thick I assume. To account for radiation to the surrounding you can apply a radiation boundary condition on the structural side.
A couple of other points:
- Use at least version 14.5
- Exporting the HTC from CFD-Post should be easy enough. Use the AXDT (External Data File) option
- In Mechanical create an FSI interface for the region that touches the flow and enable the check box that says something like "Export Results" on the FSI interface. In the solver directory for the Mechanical solution you will then get some axdt files containing the temperature and heat flow, which you can re-format and use as a profile boundary condition in CFX. Alternatively, read the Mechanical rst file into CFD-Post and export a Profile Boundary for temperature (CFD-Post will only read corner node and not mid-side nodes from an rst file, so you might loose some resolution here).

Lastly, is it really the intention of your project to model the surroundings and solid? You could just solve only the flow field in CFX and apply an External Heat Transfer Coefficient as a boundary condition. Obviously it's an approximation, but perhaps that was the intention of the project.

[Phili]

After taking a break from the project due to exams, I'm focusing on my simulation again.

I have one more question regarding your approach, Stumpy:
Do I guess at the inner wall temperatures and apply the HTC to the inner walls of my Mechanical model or do I guess at the outer wall temperatures and apply the HTC to the outer walls?

Really appreciate your help by the way!

[ghorrocks]

You should be able to answer that question with some simple analysis. Do a 1D thermal resistance analysis of the exhaust air, pipe to ambient air thermal path. That will tell you whether significant temperature changes happen across the pipe - so you can make an informed decision as to where to put the boundary condition.

[Phili]

Well of course I have got a temperature gradient through the pipe wall.