I am modelling a 6" diam tube at ambient temp with a 30W heat source in it. Surface temps reach typically 450 to 500 degK. I have a pressure outlet at exit but at inlet I am not sure what to put. I have been using velocity inlet and specifying 0.01 m/s just to get things moving but am concerned that I may be throttling the flow which may in turn explain why I am finding it hard to converge continuity as there is a mass flow imbalance. Would a presure inlet BC be ok and if so what values should be put for pressures at boundary given the likely flow of not much! Not much is my guess.

Would appreciate a voice of experience and perhaps some references to read.

Chief

Is the tube vertical, horizontal or angular?

sorry, you get too familiar with your own problem.

The tube is vertical acting as a chimney to take the heat away. It is therefore open at each end. I am experimenting with different exit chimney diameters to maximise the air flow to cool the body as efficiently as possible. I would like the boundary conditions to be sympathetic to the induced flow rather than having to prompt it with guesses as to the inlet velocity.

Chief

Sorry, having the same problem... :P Different scale, same problem.

It seems to work fine (with no pressure or speed specified) as long as the angle isn't 90 degrees or 0 degrees. At least the Fluent User Interface program I am working with Airpak.

I moved on to other aspects of my project, and in the meantime thought of two possible solutions:

1) perhaps tilting it to 89 degrees...

2) changing the gravity vector to include a slight x or z direction.

3) a third possible way may be to jut out the heat source a bit, like if it is a small light bulb or heating coil. (I cannot, since this is not the case)

I am guessing it is due to the way natural convection is calculated as directly opposing gravity, and from what I have read, natural convection off a vertical plane is a bit more complicated.

Also, I don't have a phd in anything... so take my advice for what it's worth... maybe my ignorance will require a more intelligent retort... In which case I will be quite happy.

no worries- a PhD doesn't mean squat unless you can apply what you know. Experience by messing around with something generally as you are doing can give a good appreciation for characteristics that a text book or journal cannot.

You have raised some interesting points but you do not say what you mean by not working at 90 or 0 degrees. I am not familier with Airpak but in Fluent you can see plots of scaled residuals ( the calculation errors ) for the different quantities you are solving e.g. vel x and y, energy and continuity plus perhaps turbulent parameters. In my modelling the residual of continuity does not reduce below about 1e-1 which I guess is not much good. You can also see how mamy iterations it is taking to converge and again mine takes a long time (roughly 20 thousand, yes twenty thousand) iterations. On a simple desktop this takes several hours. Perhaps this is normal for unstable natural convection problems. How do nat conv problems solve in Airpak? I assume it uses similar routines to solve or is specifically designed for cooling problems?

Chief- without a PhD

I believe Airpak uses a method which coarsens and smooths the gaussian convergence... or something like that, (I don't remember the name) to help speed up convergence. A simple model as yours should take no more than 1000 its.

At 90 or 0 degrees, it is like airpak gets confused.

For example, at 0 degrees, continuity goes crazy. It starts spewing air out of both sides of the pipe, with no way for air to get in. Convergence is not possible AFAIK without more detailing of the model.

At 90 degrees, the air starts to circulate inside the tube or pipe, as it has been shown to do in physical experiments in two-pane closed window experiments.

I assume this is because Airpak uses a simplified calculation for convectio, or it may be that I am missing something. AFAIK, natural convection on a vertical plane requires pressure moving against static pressure.

http://www.cfd-online.com/Forum/fluent.cgi?read=21563

this is wheer I specified my problem. Someone said I should turn off radiation, but my project has switched focus for now, so I have not checked up on it.

I should have included radiation in my problem too but have not had the patience to fill in all the material properties. As I am only interested in the nature of the flow relatively speaking so I have just created more heat sources of the different solids nearby to simulate the rise in temp due to absorbed radiation. i know this doesn't take account of rise in air temp due to radiation absorption but this I expect to be quite small in a pipe 6" in diam.

How do you get a figure for the typical number of iterations a problem needs? I assume it is a function of mesh precision and domain size as well as required convergence??

Chief

A good explanation what pressures have to be set can be found in the fluent 4 user's guide p. 14.65 ff and 14.88.

Due to Fluent's redifinition of the pressure, the hydrostatic head shall not be included into the b.c. pressure value, hence for a vertical pipe 0 Pa at inlet and outlet is correct.

Further on the velocity profile of a heated pipe is very different from a forced convective laminar or turbulent flow.

There are velocity extrema near the wall (similar to the letter M). And the flow might become unsteady depending on the Ra-number!

Volker

thanks Volker. I should explain a little better as the heat source is a point source in the centre of the flow through the pipe. The pipe is essentially acting as a cooling duct. I am modelling the most efficient exit geometry given the bouyancy induced flow e.t.c hence the query regarding sensitive BC's. Thanks for the advice.

Chief

Hi, I think for your problem the heat generation in the body is not sufficient. You can take both as pressure outlet conditions. But according to physics, the fluid density will reduce and it will go to top, and high dense fluid will come down, and also it will take fresh fluid from the bottom, so you have to take pressure-outlet at the bottom. And also you can do one thing, increase the heat generation in the chip, and increase the fluid thermal conductivity, and see how the flow patterns are coming. For your problem, i think, the heat generations is not sufficient, so it will take lot of time to induce flow inside the tube, so there is nothing to worry if the solution is not converging after 20000 iterations, but slowly those 20000 iterations will reduce from time step to time step. And also you can try by reducing the realaxation factores.

I hope these things will help you

VenuGopal

VenuGopal

thanks for your insight. I was hoping someone would have some experience to share and you seem to have played in this area before. I will experiment with the power input and see if convergeance is any better. thanks for the hints on the BC's too.

Chief