[Ben Mc]

Hi guys.

I'm a 4th year Mech Eng student using Ansys CFX for my final year project and I'm having some issues accurately representing the situation I want to model in CFX. My project involves comparing underfloor heating to conventional heating types (air con, bar heater etc). What I want to model is a single room with a surface temperature on the inside surfaces of the room, which is due to the radiation from underfloor heating (which I am not modelling). I then have found some heat transfer coefficients for the walls of the room, and I want to simulate how the room temperature changes from an initially set temperature over the course of a transient simulation. My assumption is that from the set surface temperature, heat will be transferred into the air and around the room through natural convection.

Initially I modelled this as a simple box, setting the floor with a fixed temperature and having a heat transfer coefficient on the walls and ceiling of my box. 10cm mesh size (5x5x2.5m room) with transient timestep of 1 sec. This ran through, although not giving the results I wanted, it appeared that not enough heat was being provided from the one surface to heat the room, over the simulation the temperature dropped.

Because of this I decided I wanted to try and model a surface temperature on each of the inside walls (including ceiling and floor) instead of just one surface, but I also need to have a heat transfer coefficient on each of the walls so that heat can escape to outside. These two options are conflicting, and I can't put them both on a single wall.

My next idea was to put an extra layer of mesh elements around the outside of the original, and set this as a solid. I broke down the heat transfer coefficient I worked out to the convection coefficient, which I put on both (inner and outer) surfaces of the solid, and the conduction coefficient which I put as a property of the material. I then fixed a temperature on the outer surface of the inner fluid region. After trying a few things I could not get the simulation to run, it kept on crashing due to divergence / overflow.

I'm wondering if anyone has an idea of a better way to model my desired situation, or if there are any glaring errors I've made in the way I have done it thus far.

[Ben Mc]

Have changed my approach to this problem, and have a new issue. I've gone back to my old, simple approach. I just have a rectangular prism, modelling my room. The 4 walls and the ceiling have a heat transfer coefficient (2.28, 0.62 W/m^2K respectively), and on the floor I'm putting in a heat flux of 50 W/m^2. According to my manual calculations, having twice that heat flux should stabilise at approximately 24.5 C. I'm confused why then that my simulation is looking like this so far. http://puu.sh/4XdXl.png

Obviously not enough heat is getting out, am I misunderstanding how the heat transfer coefficient boundary condition works? I assumed it was to represent the overall heat transfer coefficient of a wall, including two convection processes and the conduction process, is that incorrect?

[ghorrocks]

The convective boundary requires both a heat transfer coeff and a reference temperature. What reference temperature did you use?

Also - this simulation will be highly non-linear. Have you looked at the temperature field it is predicting? I bet you will find you have a hot cloud of air at the top and a complex plume of air going from the floor to the ground. You simple calculation does not take into account this stratification or plume.

[Ben Mc]

I set the outside temperature on the heat transfer coefficient boundary condition as 5C and initial inside temp as 15C. You are right, my simple calculation was just an energy balance and didn't take into account any of the more complex effects, but I still expected it to be somewhat relevant. Temperature field its predicting (simulation finished overnight) is this - http://puu.sh/4XM0E.png

Hottest region being at the bottom. I'm unsure why its automatically selecting the legend scale so high, the top half of it doesn't appear to have any of those temperatures anywhere in the model.

Based on your response, is it possible I'm misunderstanding the heat transfer coefficient boundary condition and how it works? I was under the assumption that I would set that boundary condition on a surface, it would calculate convection onto that surface from the adjacent fluid, conduction through it, then convection to the outside of that surface, which is at the "outside temperature" specified in the BC.

[ghorrocks]

Your image suggests either the flow has only just started or you have not activated buoyancy. Have you activated buoyancy? It also suggests your mesh is quiet coarse - this is OK as you develop your model, but once you have the model working you will need a finer mesh to get accuracy.

The convective BC is simply q=h(t-tr), so you need to define h and tr (reference temperature) to define the heat transfer. You can apply this on the outside of a fluid domain or on a solid domain. You do not define this between domains (you use interfaces for that) or inside domains.

[Ben Mc]

Thanks for your responses thus far.

The transient was run for one hour of simulation time, 3600 * 1 second steps, so its possible that the flow has not fully developed. Buoyancy is activated, using a density of 1.225. http://puu.sh/4Y1KR.png.

Mesh is indeed coarse, 100mm hex mesh. I'm hoping to get results that make sense with my expectations before I look for higher quality results or doing any mesh sensitivity testing.

So with the convection BC, you're saying the surface will receive its temperature from the fluid through Ansys' calculations (I'm assuming it must calculate its own heat transfer coefficient based on the local fluid conditions), then we just provide the reference temp and the h value for it to work out heat transfer from that surface to outside?

I've obtained my heat transfer coefficients from an air conditioning manual which provides a table of overall heat transfer coefficients (U values) for a variety of wall, ceiling and floor types. Have I incorrectly used this U value as the h value?

[ghorrocks]

I do not know what the U is you refer to. It is something specific to AC work and I am not familiar with it.

CFX applies the convective thermal boundary conditions as a heat flux, where the heat flux is a function of h, the fluid temperature at the wall and the reference temperature. That's all, nothing too complex.

[Ben Mc]

Maybe this image will help me explain what I'm trying to clear up. http://www.argentumsolutions.com/ima...atExchange.gif

To transfer heat from one side of a wall to the other, it first heats the wall up by convection, then conducts through to the other side, where it heats up the other fluid by convection. Instead of heat transfer coefficients you can use thermal resistance which is the inverse, and then heat transfer behaves very similarly to electrical resistance calculations. In the case of that picture, summing 1/ha + L/k + 1/hb would give R, which is 1/U, where U is the overall heat transfer coefficient.

My question is whether the heat transfer coefficient boundary condition captures this, and is accurately portraying heat flowing from one fluid through the wall to an external fluid. Sorry for this same question bouncing back to you over and over, it's just that the phrasing you and the program use make it seem like its only calculating one of the convection transfers. And I'm searching for anywhere I could have made errors in setting up the sim. I'm running a steady state simulation currently with 50mm mesh size and the same conditions as the transient to see how it might end up.

Edit - Just found this information http://puu.sh/4Y9bG.png
So it looks like this BC just models the heat going from the fluid into the wall. Does this mean that the Tref I supply in the BC is enforced to be the temperature of the fluid near the wall? Is this BC even providing a way for heat to escape my system?

[ghorrocks]

The last link you posted describes the convective BC. The Twall is (funnily enough) the temperature of the wall. If you do not know the temperature of the wall then you cannot use this boundary condition. The whole idea of boundary conditions is that you know what is happening at them - if you do not know what is happening you have to move the boundary to somewhere you do know what is going on.

[Ben Mc]

So the "outside temperature" field is actually defining the temperature the wall is at?
All this notation is confusing me, all I want is the heat transfer equivalent of the "Outlet" BC for fluids. I have heat coming in the floor and want it leaving through the walls. Shouldn't the program have knowledge of the temperatures from the equations and initial conditions (at least of the adjacent fluid)

[ghorrocks]

I suspect you are not looking at this in the right way. The whole point of boundary conditions is that you can describe mathematically enough of the flow conditions at that point (momentum, heat, anything else - everything) that it is mathematically defined. Then inside your domain all sorts of weird flows can happen, but as you are directly modelling that it is fine.

So definition of boundary conditions is like cutting a block out and saying I am only going to model this block - and replacing the cuts you made to extract the block with boundary conditions on the block. You have several choices of boundary condition, but you have to choose one.

If you do not know the condition at a boundary face then you cannot use that face as a boundary condition. The normal practise is to then make the modelled domain bigger and move the boundary condition further out - either to somewhere where you know the conditions so you can define boundary conditions or that the boundary is far enough out that specifying the wrong boundary condition has a small enough effect on the flow of interest that it does not matter.

[Ben Mc]

Yeah, I can understand that. I think I should have enough information to use the current location as a boundary condition, or at least I'm under the illusion I do because of still not understanding how it works properly.

If fluid B is inside my room and fluid A is outside from this image, what temperature am I defining when I enter a value into "Outside temperature" for this BC? Assuming TwB and TwA are the surface temperatures of the wall on each side.

[ghorrocks]

From the image you appear to have 3 choices of BC location.

The inner wall face - then you just model the fluid domain and use a convective BC (probably) on the outer face. The Twall would probably be your best guess at the wall temperature.

The outer wall face - then you model the fluid and solid domain, and have a convective BC on the outer wall face. The Tref then should be the temperature of the atmosphere outside. Note that this approach does not include radiative heating, you would need to add that separately if you wish.

In the atmosphere - you could put the BC in the atmosphere away from the wall, so you model the inner fluid domain, the wall and some of the atmosphere outside. This is going to be the most accurate but also the most complex.

All three of these approaches can work, it is a matter of what you know about the situation and the accuracy/simulation size trade-off you can accept.

[Ben Mc]

Yes, those are the three BC cases I imagine too. I think the third one would be too computationally intense, as I need to run transient sims in order to find out how the temperature of the room behaves over time. The second case, I tried doing something similar as I was saying in my original post but I came undone, and I think playing around with multiple domains and interfaces might be too complicated for me at this point.

One clarification, for the first case you say I would define the temperature of the wall (Twall), but for the second you say I would define the outside temperature (Tref). So does the definition field "Outside temperature" for the BC change which term it defines in the convection equation q=h(Twall-Tref) dependent on the context?

Also I tried fiddling with some steady state simulations last night trying to get some further understanding. I did a quick model using the first BC case you mentioned, which should mean that the temperature I enter in the BC as "Outside temperature" should define the Twall. However, looking at the results file, I can plot a temperature contour on the wall which shows temperature variation, should this not be possible if I am fixing the wall temp at Twall?

Thanks once again for all your responses, I hope I'm not getting on your nerves, I'm really just trying to wrap my head around this.

[ghorrocks]

No, your questions are interesting. The questions which get on my nerves are where the answer is in the documentation. That's just laziness.

You are correct that the equation is not really q=h(Twall-Tref). If you look in the documentation it states q=h(Tb-Tnw), where Tb is the specified boundary temperature and Tnw is the temperature at the internal near wall boundary element centre node. Tnw is a modelled value and will vary, and Tb is specified in the BC. But for a convective BC on a fluid domain Tb represents the wall temperature, and for a convective BC on a solid domain Tb represents the fluid temperature.

Hopefully that clarifies things a bit.

[Ben Mc]

It does, thanks. So in my case, since I don't know what the temperature of the walls will be, only the ambient outside temperature, I will have to use the second of your earlier proposed BC cases? What set of BC's would I use going from the inside to out? Obviously the external one will be the convection BC as just discussed, with specified temp being my ambient air temperature. What about the inside of the solid domain and the outside of the fluid domain?

[ghorrocks]

If I was you I would start with the boundary on the inside and just assume the wall temperature to be the outside ambient temperature. Once you have got that running reliably and you trust the answers you can try adding the wall and putting the BC on the outside of the wall. This way means you have do the development with a simpler model and you get to see what difference adding the wall makes.

[Ben Mc]

In that case, I've come full circle since that is the simulation I have been running, with poor results. Since the BC we've established should be OK, I need to look somewhere else for poor results. Residuals for the simulations for the momentum variables are usually around the order of 10^-2, which is poor, but they do not decay further, so obviously sim is set up poorly, need better mesh, some other improvement. Also, I've been dubious about whether the buoyancy is performing correctly, it seems as if it takes a very long time for the heat to spread from the floor, as the top of the room is usually close to initial conditions (15C) while the base might be 100C hotter.

[ghorrocks]

Before you add complexity to your simulation to get better accuracy you should do a mesh, timestep and convergence tolerance sensitivity study. You have already stated your mesh is coarse so the results are going to be rubbish. When you add the external wall they will still be rubbish.

Buoyant flows like this usually start doing their thing very quickly. It sounds like you do not have buoyancy set correctly in your model.

[Ben Mc]

I understand what you mean by mesh and timestep sensitivity (I think), which is seeing how the results vary when I fiddle with those settings. What is meant be convergence sensitivity?