Natural convection in an open domain
 

Hallo,

I've been working for a couple of weeks on this problem, but I really struggle to find a solution. I'm wondering if Star CCM+ can really solve this kind of problems.

What I'm trying to simulate is the classical case of natural convection on a heated plate, situated in an open environment.
I'm trying to replicate the results obtained in this article (https://www.google.it/url?sa=t&rct=j...0ovVhBdaj3YWcw) where CFX-5 was used.
I built a domain with the same geometric dimensions and tried to obtain a similar mesh.

The boundary conditions I used for the wall were 'Adiabatic' for the bottom part and 'Constant temperature' for the top part.
For the atmospheric contours, the top part was defined as 'Pressure Outlet' with constant ambient temperature, while for the long front part and the bottom one I tried different combinations of 'Pressure Outlet', 'Stagnation Inlet' and 'Wall', always keeping the temperature as constant and at ambient value.
The combination which gave the best results seemed to be 'Pressure Outlet' for the frontal boundary and 'Stagnation Inlet' for the bottom curved boundary. Anyway there were some weird flows and the convergence was terrible, above 10^(-3).

I tried to enlarge the domain, either by placing another adiabatic plate on top of the heated one, either by widening the air gap between the plate and the frontal boundary, with no avail.

I suspect that somehow Star has troubles with solving or modelling this kind of problems because of the way the BC are defined, since there isn't any 'Opening' option.
Spending quite some time searching in the literature, I didn't find any reference to a similar study performed by using this software.

The flow is laminar and I didn't use the Boussinesq approximation, but rather the 'Ideal gas' model. The conditions were steady.

I'm attaching the results obtained with a 'Pressure outlet' front and 'Stagnation Inlet' bottom.

I hope that I gave all the information necessary to make the problem clear and receive some help.

Thanks in advance.

There's nothing about this model that star can't solve if the setup is correct.

'Opening' is not a boundary condition in any code. I suspect it's some kind of CFX jargon for something. Generally open natural convection cases will use pressure conditions at the boundaries, but you have to specify a pressure gradient that fits the system if your boundary is in the direction of gravity.

Make sure you have also set the reference density correctly.

By specifying 'a pressure gradient that fits the system if your boundary is in the direction of gravity', do you mean a zero gradient pressure condition on the vertical atmospheric wall? I tried this but still the results aren't good at all.
I wouldn't know how to set them differently.

No, in fact the pressure gradient on the external boundary is nonzero. The physics of natural convection depend on it. You have to specify the gradient due to gravity.

So the gradient boundary condition for pressure at the front wall should be defined as dp/dx = density * gravity_acceleration?

If I'm wrong, could you please tell me how to set it?

Thank you very much.

Sorry, should have been more explicit earlier. You don't want to specify the gradient at each cell, you want to specify the pressure value. That should change in height, so there should be a gradient across the entire domain.

So this gradient that I should specify, is dependent on the height of the boundary that I'm defining? Is this due to the variation of pressure in the column of air because of gravity?
In this case I don't think that this applies or really matters in the situation I'm studying, given the really small geometry of the problem.

If instead I didn't interpret your words correctly, than I still wouldn't know how to define this boundary condition rightly.

No, that's what I meant. The physics of NC depend on it existing, but if your domain is big enough, you can probably get away with a constant pressure condition.

See if you can find the details on what the 'opening' boundary condition is.

I don't really understand what this domain is trying to model. Just a vertical plate? Why does it have such a strange shape?

Yes, I indeed saw how enabling the 'Gravity' option changes the pressures at boundaries and the flow fields even with all other conditions being equal and using a small domain.

I'll definitely check what the 'Opening' condition exactly means.

The reason why I gave the domain that odd shape is simply because I tried to replicate as closely as possible the conditions used in the aforementioned paper. I think it was originally used in order to follow better the development and shape of the NC flux, but I'm just guessing.
Anyway I tried also with a rectangular shaped domain and results don't improve.

What I'm going to try now is to define a pressure boundary condition defined as p (y) = g * density * height. I think this is what you meant in the previous answers, right? It makes sense to me.

I went further with my simulations, trying to vary the domain and the boundary conditions, but the results still look weird.

As suggested in the previous posts, I tried to implement a field function on the pressure outlets that took into account the variation in pressure caused by the weight of the air column.
I defined this as -9.81*density*Yposition.
I tried it in combination with both the ideal gas model and Boussinesq.
Still, the results that I obtain seem to be strongly conditioned by the pressure gradients that are present on the boundaries, while the natural convection is much less influent.

I also tried to define the pressure on the pressure outlets as Field Function 'pressure'.
In this case the movements caused by pressure differentials at boundaries disappear, and the natural convection is evident.
However, the flow reaches the top of the domain (this one also a Pressure Outlet with 'Pressure' Field Function) and then bounces/get redirected to side, where at some point finds a way out. There is of course something wrong.

I really don't understand why both the above boundary conditions for pressure fail to give realistic results, and I don't know what could I tried to do differently.

I'm posting here four pictures of the vector fields. They are all obtained using the Boussinesq approximation.
The first one is with a 'constant' pressure, the second one with the -9.81*density*Yposition field function, the third one with the 'pressure' field function. The last one is a detail of the third.
I enlarged my domain in order to be sure that the heated plate (on the left side) doesn't influence the 'atmospheric opening' on the right side.

I hope to find some help and thank in advance for your replies.

What does your mesh look like? Is this steady?

In the images is my mesh. The prism layer is 22 mm thick (the adiabatic plate is 76 mm tall, the heated plate 381 mm, and the domain 1 m wide), with 29 layers and a near wall thickness of 0.1 mm. Minimum and target surface size are 2 mm.
Worst quality is 0.59

I tried also some finer and coarser meshes but the results don't seem to change much.

Yes, I used a steady model as I was trying to replicate the procedure and results of the article.