[hebeldebel]

Hi,

I have a physical testbox with a heat source inside it. The box has 3 holes and is placed inside a chamber with regulated temperature.

To simulate my testbox, I created the walls of the box and gave them a specific temperature and created 3 boundaries as pressure outlet for the 3 holes and the surrounding environment.

With static pressure the simulation starts to diverge after 160 iterations and with environmental I do not see any convergence after 7000 iterations (and the net mass flow inside or outside the box varies between +40 and -20 kg/m^2-s)

Is there a way to do this without simulating the chamber as well?

[me3840]

This sounds like a natural convection problem, which are very difficult to solve steady-state, which is sounds like you're trying to do. Natural convection is not a very steady phenomenon.

What solvers and physics are you using?

[hebeldebel]

Hi,

thank you for your time, here are some more informations:

initial conditions of the air: 303K
boundary temperature of the outer walls: 303K
temperature of the pressure outlets: 303K
heat source turned off
enabled models for air:
gravity, segregated fluid temperature, ideal gas, cell quality remediation, two-layer all y+ wall treatment, realizable k-epsilon two-layer, k-epsilon turbulence, reynolds-averaged navier-stokes, turbulent, segregated flow, gas, steady, gradients, three dimensional
number of cells: 3802271
I have one source of forced convection inside the setup simulating a radial fan.

I tried to check, if the output makes sense and plotted the sum of the mass flows through the 3 outlet. It never reaches 0.

[me3840]

You didn't mention there was a fan before, so that should be better for the steady-state approximation. What are you using for your fan source? How have you implemented it geometrically? Is the fan curve correct?

Since you have cell quality remediation enabled, there should be a field function available called bad cell indicator that will show you where poor quality cells exist, I would take a gander at that.

Furthermore, I would not use cell quality remediation. CQR is basically admitting your mesh sucks and you're willing to get a less accurate answer. The obvious solution is to improve the grid, not to diffuse the answer. Can you post some images of the geometry and grid?

You need to find out where your mass is going. How big is this box? Why are you measuring mass flux rate, though? Normally folks just measure mass flow over all of the BCs and sum it.

[hebeldebel]

Originally Posted by me3840

You didn't mention there was a fan before, so that should be better for the steady-state approximation. What are you using for your fan source? How have you implemented it geometrically? Is the fan curve correct?

I forgot to mention it, but this is important, of course. It is a radial fan represented by a region of air. This region has a motion specification via reference Frame (rotation rate 6300 rpm).

Originally Posted by me3840

Since you have cell quality remediation enabled, there should be a field function available called bad cell indicator that will show you where poor quality cells exist, I would take a gander at that.

I saw some Bad Cells (value of two) at the pressure outlets and locally increased the amount of cells, which solved the problem except for one or two cells.

Originally Posted by me3840

Furthermore, I would not use cell quality remediation. CQR is basically admitting your mesh sucks and you're willing to get a less accurate answer. The obvious solution is to improve the grid, not to diffuse the answer. Can you post some images of the geometry and grid?

This will be difficult, because I don't really know how much I am allowed to show, but I attached two basic pictures showing the pressure outlets.

Originally Posted by me3840

You need to find out where your mass is going. How big is this box? Why are you measuring mass flux rate, though? Normally folks just measure mass flow over all of the BCs and sum it.

My bad, I thought it would not matter much, because the areas are constant. I will do another run measuring the mass flow.

[hebeldebel]

I did another run with more cells at the pressure outlets and I disabled CQR.

The mass flow seems to oscillate around 0 g/s and the residuals probably wont change much more. What can I do to get closer to 0 g/s? More cells? Change the under relaxation factor?

[hebeldebel]

sorry for the triple post but it seems you cannot add picture with the edit function.

Here are some picture with streamlines starting at the fan outlet.

[me3840]

How big is this thing? Mass fluctuations in the e-4 kg/s range are pretty good for industrial problems.

The velocity field coming from the fan looks really strange. Why do the streamlines branch off?

[hebeldebel]

Originally Posted by me3840

How big is this thing? Mass fluctuations in the e-4 kg/s range are pretty good for industrial problems.

I added a picture for the size. As it is rather small, I thought even e-4 kg/s fluctuations have an big impact.

Originally Posted by me3840

The velocity field coming from the fan looks really strange. Why do the streamlines branch off?

There is a heatsink right after the fan, its fins split the flow up.

[me3840]

Er, didn't see the scale on your plot, the mass convergence is in e-6 kg/s range, which is good.

So there's a heatsink and a fan in this box...is there anything else hiding?

The residuals fluctuate in a very transient fashion, I wonder if some transient flow structure is limiting the steady simulation. The heatsink and fan seem rather small compared to the size of the box, which really isn't that big. I wouldn't be surprised if the largest eddy in the box has some transient nature.

Have you taken a look at any other engineering values? Perhaps we can nail down what's causing the fluctuations from that. It may also be worth looking at where your residuals are high.

[hebeldebel]

Originally Posted by me3840

Er, didn't see the scale on your plot, the mass convergence is in e-6 kg/s range, which is good.

So there's a heatsink and a fan in this box...is there anything else hiding?

There are two obstacles on top of the heatsink and three pillars connect the heatsink to the bottom boundary wall. The pillar diameter is about 4 mm. The fan is directly attached to the rear of the heatsink and there is a distance of approx. 80 mm between the front of the heatsink and the boundary wall in the front. No other parts are present inside the box.

Originally Posted by me3840

The residuals fluctuate in a very transient fashion, I wonder if some transient flow structure is limiting the steady simulation. The heatsink and fan seem rather small compared to the size of the box, which really isn't that big. I wouldn't be surprised if the largest eddy in the box has some transient nature.

Should I try to find out, where this eddy is located? If so, I would look for high vorticity values, right?

Originally Posted by me3840

Have you taken a look at any other engineering values? Perhaps we can nail down what's causing the fluctuations from that. It may also be worth looking at where your residuals are high.

I will look at the residuals right away, what do you mean with engineering values?

[me3840]

Vorticity may do well, yes.

Engineering values, as in things you're interested in seeing. Temperatures, velocity probes, integrals of shear stress, something.

[hebeldebel]

I am sorry it took me this long to answer, but there was the weekend and simulation took another day.

I am interested in one engineering value, which is the temperature of a specific point on the heatsink. I therefore monitored it and ran the simulation. I added the results below.

Mass flow still fluctuates, but I would say I can neglect it, as I am primarily interested in the temperature. The temperature seems to converge, although it is not the same value as seen in real life.

My preliminary estimation would be: I can use this setup, but I need to tweak fan speed (adjusting voltage not rpm in real life) and continua of the solids to get to the right temperature.

Am I correct about that, or do I need to check something else as well?

[me3840]

There are plenty of other things I would check. Put some probes in the flow and measure the velocities, see if they are periodic.

Perhaps run with temporary storage and see where the residuals are high.