Exactly the same thing. Change your convergence tolerance from 1e-3 to 1e-4 and 1e-5 (If you can get there) and see if it makes any difference. Likewise for the time step size if you run a transient simulation - adaptive timesteps with 3-5 coeff loops per iteration is good here because it couples convergence tolerance to time step size, and means you have one less variable to do a sensitivity analysis on.

How does the adaptive timestep work? Does it just vary the timestep in order to find lower residuals or something? I've put it on in my recent simulation and it dropped the time step from 1sec down to 0.5 (which I put as my lower limit because I want the simulation to finish some time soon), and its satisfying the RMS of 10^-4 and convergence of 1% within 10 coefficient loops which is much better than previously.

The best way to run adaptive time steps is to get it to home in on 3-5 coeff loops per iteration. Then it automatically adjusts the time step size over a series of timesteps to achieve it (if it is possible to achieve).

This is when the solver is running at its most efficient for most simulations and with good time accuracy.

10 coeff loops is too many for most transient simulations in CFX. CFX runs better with smaller number of coeff loops and smaller time steps.

Yeah I think most timesteps are converging in 5 loops currently, it was higher at the beginning of the simulation.

That means you are pretty close to a good time step size - assuming your convergence tolerance is OK. But still you might as well use adaptive time stepping so the time step size can grow and shrink with the complexity of the simulation as it progresses.

I just left convergence tolerance at 1%, that was the suggested tolerance in the workshop simulations I did. Besides, probably not worth pushing too hard for results with a coarse mesh. I'm figuring the results at this point are going to more qualitative than quantitative. Although hopefully not too far off the mark.

Yes, on a coarse mesh a reasonable guess at the parameters is OK. When you are confident things are working properly then check those assumptions and refine the mesh to an accurate solution.

Another question Glenn, when I analyse the simulation in Post, and plot a temperature contour along the wall, is it actually plotting Tnw (temp of the fluid directly adjacent to the wall) or the temperature of the wall? If the latter, will the convective BC continue to use Tb to calculate the heat flux throughout the simulation?

On a similar note, I think I remember reading somewhere (maybe on these forums) that the heat transfer coefficient you supply in the BC is only used as an initial value, and this gets recalculated during the simulation depending on the flow conditions at the boundary. Is that at all the case?

Have a look in the documentation about hybrid and conservative values. That will answer your wall temperature question.

No, this is not correct. If the boundary is internal (eg a fluid/solid interface) then the h is calculated by the solver at all times - you do not need to define an initial value. If the boundary is external and you define it as a convective boundary then the value of h you define is used for all time steps.

So since post by default displays the hybrid values, shouldn't the wall be coming up as the defined Tb in post?

By default it should show the hybrid temperature value at walls, so if you have defined a wall temperature it should be that temperature.

http://puu.sh/52J2K.png Any idea why this is happening? Should be at 278.15 (5C) I thought.
Also do you know how I can work out where those min/max temps are in the model, its a bit alarming that there is a 250+C spot in my room.

Use an isosurface to find the hot spot. It can be caused by all sorts of problems from numerical problems to not setting the simulation up correctly.

How can this be occurring?
Image 1 Isovolume of anything above 318K
Image 2 Isosurface of 350K

How can what occur?

What boundary condition have you put on the bottom? Are you sure it is converged?

Boundary condition is a wall, with heat flux specified. I mean, how can there such a small isovolume, which is defined by any temp 318K or over, and a much larger isosurface of anything at 350K?

That is the hybrid and conservative values. Your wall is quite hot, but the heat has not penetrated far into the domain. So you get a hot isosurface right next to the wall. Isovolume looks at the conservative values - and they are much cooler as they are further away from the wall.

For the convergence study (and the like) log on to the ANSYS Customer Portal and view the CFX Introductory Training Material, this is covered in the Best Practices presentation under Iterative Error (lots of pictures).

That sounds like a very useful resource. I had a quick look and could not find it. Can you post a link to it?

Uploaded is a print screen from the ANSYS Customer Portal showing where it can be found under the Tutorials & Training Materials section, all the presentations are in File 1. There is even short videos covering the material - worth a look.