Scalar Mixing problem - Gases do not mix

[Anonymous]

Good morning everyone (and happy New Year),

As the title suggests, I have a scalar mixing problem within a large room. Air is coming in through nozzles set around the room on high level and the second gas is coming off the floor. Lower inlets represent air infiltration through closed doors.

There are 2 scenarios in the design study.The first simulates for airflow only and the second is for mixing gases.

I have followed the guidelines and any helpful advice I could find in the forum however the gases do not seem to get mixed well (see picture attached), not to mention the crazy amount of time it takes the simulation to run (120 iterations approx. 3 days...).

The setup I have tried so far was the following:

- Material: Air (Variable), Scalar 0 for air, 1 for second gas. Density/Viscosity/Conductivity/Specific Heat were defined using "piecewise linear" method for increased accuracy.

- I tried both "Pressure=0" and "Unknown" for air infiltration and I have tried to assign scalar 0 (air) as well.

- Mesh was around 3mil elements. (PC limitations)

- Both options for ISC.

- Advection Scheme 1 and 2

- I have tried both options of flow compressibility.

- Heat Transfer enabled to assign gravity.

- Turb/Lam ratio increased to 2000 due to the small size of the nozzles.

Notes:

The design of the airduct inside the room that extracts the air, may seem a bit unconventional, however it was the only way to define the extract flow rate within the domain (in reality they use dampers to adjust it). I understand I should make the outlets longer, but I was constrained by the duct size and I am pretty sure this does not affect the mixing.

The version I use is 2013.

The support file and screenshot showing the results when the scalar is enabled are attached for your convenience.

Any suggestions at this point would be much appreciated as I have spent significant time on this, trying different options with no luck.

Thank you in advance for any help you can provide.

Edit: It does not allow me to upload the .cfz file saying "The contents of the attachment doesn't match its file type". The filesize is 7.55MB and I do not have Dropbox.

[Jon.Wilde]

Hi AndyManc,

I think that somehow sharing the CFZ might really help here, there are a few unanswered questions which the CFZ would highlight. Are you able to install Dropbox if I share a folder with you?

My initial points from your comments:

1. What are your inlet conditions and is this all that drives the flow?
2. What are you outlet conditions?
3. What is heating/cooling the air?
4. Better to run with ISC on unless you are running transiently
5. Are you seeing flow speeds high enough to warrant running with compressibility on? If not, leave it off
6. What does your mesh look like? It would need to be quite fine

Kind regards,

Jon

[Anonymous]

Hello Jon,

Thank you for the quick reply. I am afraid I cannot install Dropbox where I am. Can I upload it on a multihost server (i.e. multiupload) and post the link? Otherwise it will have to wait until I get home.

In the meantime please find attached screenshots in the pdf file, where I show all the key features of my model and a screenshot of the boundary conditions.

1) As you can see from the screenshot, the first inlet flow rate (0.1215m³/s) applies on each nozzle and has been assigned as air (scalar 0). Pressure 0 is on the lower openings (I have tried unknown AND removing the scalar value as well without any result) and the third flow rate (0.27m³/s) has been assigned at the outlets (this answers your 2nd question). The very small flow rate (1e-05m³/s)  is the second gas (scalar 1) and it is applied on the floor.

3) There is no heat in the model. I have only enabled this option to turn on gravity.

4) I only run it in steady state and I have tried both options for ISC.

5) The velocity of the air coming off the nozzles is fairly high compared to the flow velocity within the room, however I have tried both options without fixing the gas mixture problem.

6) Please see pdf file attached. I understand it is not as fine as it should be, however I am limited by the PC specs. (12MB RAM)

[Jon.Wilde]

Hi AndyManc,

Sure, feel free to use any method that works 🙂

Thanks for the images too, very useful.

Regarding the model - you have done the right thing recessing those outlets in the duct (I'm impressed, so many users do not do this and it all helps). The only thing I think might be an issue is that you will need to suppress the duct from the mesh - to avoid having internal surface BC's which are not permitted.

Gravity will only have an effect on the air if you have have the density changing with reference to the scalar. Otherwise I would just run forved convection only. What are your flow speeds, is the gravity component significant? 

Avoid unknown BC's, these are only really used downstream in compressible models, not usually needed here.

The mesh does not look too bad, although it does need to be of good quality for scalar models. Let's cross that bridge once we have checked over the model.

It might be worth considering a manual mesh here also..

[Anonymous]

Hello Jon,

Thank you for the feedback. Please find the link to download the support file HERE. I hope this one will work.

As you will find from the support file, the extract duct was modelled within the room and then "removed", resulting in an empty volume. It was the only way I could think, so I could define the flow rate at the outlets. Suppressing the "duct", will result in suppressing the entire room!

The density of the second gas is considerably higher (1.20 for air, 9.73 for second gas), hence the gravity is on.

[Jon.Wilde]

Hi AndyManc,

Thanks for sharing, I have it here and I have more questions/comments! Sorry that there is so much to read here.

How you have the outlet duct set up is fine, the BC's are essentially on a boundary, no problem at all with that.

You defintitely want to leave ISC on.

Use ADV5 rather than 2.

Try with flow only first - forget the density change initially. We can then turn on gravity later.

Is the heavier gas really meant to enter through the floor? This Boundary Condition may not work too well, can you model the floor space and have a real inlet at the side somwhere? It depends what the floor is made from really, is it tiled?

I could easily see the scalar 1 trying to exit where you have a P=0 and Scalar =0, which cannot be correct. Consider a flow rate here? (although you will need a P=0 somewhere)

The mesh is one of the large issues here. You likely need a mesh that is outside of the scope of your PC. Manual meshing should help I think, most of the coridoors are of similar size.

The other issue is the scalar - there is a large change from one density to the other, this is not easy.

Check out the mesh below, this shows 1 or 2 elements across gaps in some places, we should have more. Maybe 4-5 is a starting point although I fear that may still be too coarse.

[Anonymous]

Hello Jon,

Thank you for the comments.

The heavier gas in an ideal model, would come off the surface of the suppressed parts (aka all over the place simultaneously), so it would not be "realistic" if I was modelling the gas coming in through a single nozzle (unless the steady state gives me the "final picture", showing a well mixed gas, regardless the source?).

Therefore, and for simplicity I assigned it on the floor (which is concrete by the way) and I suppressed the rest.

Since I am in the learning curve, I would like to ask how does this interfere with the mixing. Is it the large area that it comes from and the size of the adjacent elements? Would it be better if it was coming from several smaller ones (i.e. the surface of the suppressed objects)?

We extract more air than we supply in the system, therefore we will experience inflitration (see attached) when I solved for airflow only. For this reason I set the scalar to air on these openings since we are bringing fresh air from outside (although I have tried without setting any scalar either, showing no difference). I attach another screenshot showing velocity magnitude when scalar is enabled. It does not look anything close to the previous analysis, like it has not worked properly, hence I would not pay much attention to any vectors pointing out (reverse flow).

From what I understand the choices I made in the setup were correct, since I had tried your recommendations already (except the conservative Advection Scheme 5) and the main issue is the mesh that does not let the simulation to run properly and possibly the large difference between densities we deal with. Is this correct?

Best regards

AndyManc

[Jon.Wilde]

Hi AndyManc,

Regrding your final comment, yes. This is likely the issue we are facing here.

Our other concern is with the large inlet on the floor. Are there no inlets but a gas given off by the materals, which are suppressed here? I see the challenge for sure.

If that large inlet works (it might, although it is not traditional) I am also concerned that it is really close to the P=0 and Scalar=0 inlets. You are right to have Scalar=0 here if flow can enter, but it might cause solver issues if flow exits. Is there another way to set these up or are they just 100% open to air with no forced convection at all?

Kind regards,

Jon

[Anonymous]

Hello Jon,

Thank you for the response and your valuable assistance.

I am afraid I have already made enough assumptions / simplifications in the existing model and further changes could possibly compromise the accuracy of the results and what we are trying to see.

Kind regards

AndyManc