Boundary Conditions Setting for Natural Ventilation Model

[annisanurul]

Dear All, 

I would like to ask for your suggestion regarding natural ventilation model. 

I want to simulate a natural ventilation model which combine the internal and external flow, like the one in this page https://knowledge.autodesk.com/support/cfd/learn-explore/caas/CloudHelp/cloudhelp/2014/ENU/SimCFD/fi...

I attached the png file of my model after simulating it. So basically, the model is already covered with an external void which represents the external air around the building. I set up the model as follows:

1. Material environment changed to variable and set to the actual air temperature (30 C)

2. All wall, floor, and roof set as concrete

3. There is a human model as well to analyze the thermal comfort

4. Set one surface in the external void box as inlet, and the opposite surface as outlet

5. Set the top surface of the external void box as slip/symmetry

6. Set the velocity on the other sides of the external void box (next to the top surface) to have the same direction and velocity as the inlet boundary condition (I did the set up like this because I followed this post: http://simhub.autodesk.com/discussions/threads/330/post/5547674)

And My questions are:

1. As can be seen from the attached figure, Does the external void box is still too small in this case? because the velocities in both sides of the building (colored green) are higher as if there are constrictions around that part. Does that mean the both sides of the external void box are not represent free external air?

2. And, also from the figure, it can be seen that the iteration process shows a very jagged line. Does it indicate something is wrong in my current setting? 

3. I also read in this post (http://simhub.autodesk.com/discussions/threads/330/post/5547674) that I cannot apply internal boundary conditions. So, does it mean that I cannot set boundary conditions in the internal geometry, such as wall or floor or ceiling of my model? What if I need to assign temperature boundary condition in the internal wall to obtain a more accurate result, what is the best approach that I could do?

Looking forward to hearing your suggestions

Thank you 

[Jon.Wilde]

Hey!

I think I can help here with a few short comments:

1. Yes - I would probably double it in all directions, maybe a little more on the outlet side. As a check also - is the air box created in CAD? You do need to do this to avoid an air gap underneath the building
2. It is likely that you need a finer mesh or you have recirculation at your outlet (I presume you have a flow rate at inlet and a P=0 at outlet? This is ideal)
3. You could apply a volumetric heat load to a volume OR suppress a part from the mesh and then you can apply a temperature BC to a surface of it (essentially making the temp condition sort of external as it is adjacent to a void)

Hope that helps,

Jon

[Amal.C]

Hi @annisanurul,

I would like to check if we were able to respond to your questions. Please let us know if you still need help 🙂

Thanks,

Amal

[annisanurul]

Hi @Jon.Wilde

Thanks for your reply and sorry that I didn't give respond immediately

1. Yes, I used the geometry tools in Autodesk CFD to create the air box. But now, I am creating the air box in CAD to ensure that there is no air gap underneath the building. But, I still have a question regarding this issue. Is there any recommendation for the ideal size of the air box?

I read in this web (https://knowledge.autodesk.com/support/cfd/learn-explore/caas/CloudHelp/cloudhelp/2014/ENU/SimCFD/fi...) about calculating the domain size which states "Generally, the exterior or “far-field” boundary must be at least 5 to 10 chords upstream and 10 to 20 chords downstream of the body. Higher Reynolds number flows will require far-field distances in the upper portion of this range."
Do you think it's okay if I don't follow that rule? because my model will be too big and I won't get the fine result for my focus area (the inner part of the building)

2. Yes, that's true, I assigned a flow rate and a temperature at the inlet and a P=0 at the outlet. But, actually, like I said above, my focus area is in the inner part of the building geometry (Need to know the thermal comfort in the building). I just built the air box to model the actual condition where there are other buildings around the building that I want to analyze and see the impact of the building to the inner air flow.

So, should I set a finer mesh to all area in the model or do you have any other suggestions? Because it will increase the number of mesh and increase the simulation time as well.

3. Thanks for this suggestion, I think it works. I already tried to suppress the part and assigned temperature BC in a more simple model and it works. I will try in my current model as well.

Thanks in advance
Nurul

[Jon.Wilde]

Hey, no worries.

To respond:

1. This is likely OK, could you share an image of what you have now? We can give a rough yes or no 🙂
2. I would look at a couple of regions:
   1. Be sure you have more than 1-2 elements from the top to the bottom of your domain near the inlet and outlet. CFD can leave these too coarse with large elements where you need something a little smaller
   2. Make a test - run it without refinement inside/around, then refine a region including the building by 30% or so and see if this changes your results
3. *high five*

Thanks,

Jon

[annisanurul]

Hi, @Jon.Wilde,

1. Here I attach the .cfz file of my model. Please let me know whether it's already OK or I still need to expand the air box.

2. I also attach the .jpg file that shows the element near the inlet (This done by choosing the Autosize button). The element number seems still less than your suggestion. So, I think I still need to set a finer mesh on the inlet and outlet BC. 

Regards,
Nurul

[annisanurul]

Hi @Jon.Wilde

I already run the simulation for the model above and after 100 iterations, I got an unrealistic result (Can be seen in the attachment below). 

The velocity result around the outlet BC doesn't make sense, it reaches 9 m/s whereas I only set the velocity at inlet around 1.11 m/s. 

I also already made a finer mesh for both the inlet and outlet BC (the element number between the top and the bottom part is more than 2 element for those surfaces).

Do you have any suggestions how to fix it? Should I increase the iteration number? Or should I make a longer distance to the outlet surface?

Thanks

[Jon.Wilde]

Hi,

Great, the model is now on the ground, this is loads better.

Yes, I would say the mesh is too coarse - CFD somehow needs to form a flow profile right? This is very tricky with only one element 🙂

My starting point with a coarse mesh might be something like a 0.6 refinement to the model, all volumes (applying this to the model as is, gives me 5m elements).

How much RAM do you have on your machine? CFD tends to need something like 1-2.5GB of RAM for every 1m elements. Usually on the lower end if the mesh quality is good - equilateral elements.

I would make this something like 10x as high - you need to avoid artificially accelerating the air above the building as well as around the sides.

It probably doesn't need to be as wide but let's go with it for now.

Then make the outlet side something like 2x as long - so the flow is nice and smooth before it exits.

[annisanurul]

Hi @Jon.Wilde

My PC has 8 GB RAM, so I guess I can increase the element up to 5-8m.

I tried to create higher air box, but only 5x the building height and for the outlet side, I made it around 2x longer and the total of the element is 3.5m. So, I did not change the refinement due to the limitation of my machine. 

However, I found another problem. I tried to simulate the model with slip/symmetry BC in the top side of the air box and left the other side (left and right) of the air box without BC (scenario 1). I ran the simulation for 100 iterations and it works. But, it means that the simulation doesn't represent the real condition where the left and right side of the box should represent free air. So, I created another scenario (scenario 2) and added velocity BC to both sides which have the same direction with the inlet velocity BC. With this current setting, the simulation stopped with an error message "Solver has stopped unexpectedly due to divergence". I attach my updated model below. The file size is quite big, but please take a look.  

My question is:

Do you think all my current setting in the updated model already correct?  Or do you have any other suggestions how to model the BC for the left and right side of the air box? Or that is not the problem in this case?

Thanks

[annisanurul]

Hi @Jon.Wilde

Just wanted to update the information from my previous post

So, I started the simulation again for the scenario 1 and set the iteration number to 200. Unfortunately, it showed the same error with the scenario 1. In the 130th iteration, the simulation stopped due to divergence as well. I think this problem is not because of the BC setting for the other sides of the box air. 

I read some pages on Autodesk forum that mention that to make a more stable simulation, I need to switch to Adv5 for the advection scheme. Is it true? 
Do you have any other suggestions?

Thank you