Help with simple simulation (#1)

[Anonymous]

Is there anyone available that can help guide me through a simple simulation? The case is about exaust air to see how will it move in an open area with wind flow. 

Best regards.

[Anonymous]

something like this. 

[marwan_azzam · Accepted solution]

Hello,

I imagine you only need to model the air domain.

• One inlet for the wind with a set inlet velocity and Scalar=0, and Temperature boundary condition (BC).
• One inlet for the exhaust gas with a flow rate (or velocity), Temperature, and Scalar=1 BCs
• One outlet with a Pressure=0 BC.
• Set the properties of Air to Variable.  This way they are a function of temperature.
• Turn on Scalar under Solve and set the coefficient of diffussivity.

Marwan

[Anonymous]

Hello Marwan. I am glad to see your reply. Very helpfull as allways. 

Here is a .cfz file and some further explanation of the case. I have some questions in order to help me validate the simulation. (i tried to drag and browse the file but i get a message with

"Correct the highlighted errors and try again.

• The attachment's exhaustandmethane.cfz content type (application/octet-stream) does not match its file extension and has been removed.") How can i share the .cfz file?

Case: A hydrocarbon storage tank with a pressure vacuum safety valve (PVSV) is close to a heater´s exhaust gas at 650°C. Analyze the danger of explosion if the hydrocarbon vapors meet the high temperature exhaust.

Approach: Since Autodesk CFD is not able to mix 3 fluids, I imagine 2 runs of simulation scenarios to analyze this danger.

Scenario #1: How close and at what temperature will the hot exhaust get to the PVSV with certain ambient air velocity.

Scenario #2: How close and at what concentration will the hydrocarbon vapor get to the heater´s exhaust with certain ambient air velocity.   

As shared in the file i imagine it has been done correctly. That being stated i do have some doubts/questions. 

Q#1: Should I use a created material for fluid scalar mixture of Air-CO2 or Methane?. I suppose yes because I want to input CO2 and hydrocarbons with air.

Q#2: Should I use compressible or incompressible flow on Solve window? I suppose incompressible because it is at ambient location (no enclosed vessel or area).

Q#3: Should I use transient or static? I suppose static is enough since I am worried about the worst-case scenario.

Q#4: Do I need to check gravity box and its direction? I suppose yes since i am interested in heat transfer.

Q#5: Is the fluid mixture correctly applied? I suppose yes following examples on “Scalar Mixing Analyses (Part 1&2)” dated 4 nov 2016 on YouTube Channel “Autodesk Simulation”.

Extra Q: When using Transient solve. What is the difference between assigning IC to all volume’s vs not all volumes? I think i have seen some examples without all volumes and also have been recomended to apply ICs to all volumes. 

Here are some screenshots

As allways, thank you very much and best regards!

[marwan_azzam]

Hello,

You are welcome.

In order to attach a cfz file you have to zip it first.  Attach the zip file.

Marwan

[Anonymous]

Hello Forum. I share my .cfz file. Case explained above. Welcome are any qustions and coments.

Q1: Does it look allright? (setup and results)

Q2: One big question: Why does scalar colour seep inside the steel tank? (see image)

Materials: created fluid Air-CO2 or Methane (depending on case "EXH" and HC") Density Scalar 0=Air 1=Other fluid. Set on variable. Rest of materials as steel. 

BC: shown

Mesh: refined Exhaust outlet (inlet to model) to 0.5 and CFD created volume Air to 0.5.

Solve: Automatic convergment assesment tight. First flow then Heat transfer (gravity applied). General scalar applied acording to case. 

image where i question the scalar result

 I also see on Iso volume that the methane is goin inside the vessel through the outlet, as if it were recirculating. 

Q3: Is there anything i can do to prevent this aparent seeping and recirculation?

Allways thankfull and best regards. 

[frederic.gaillard.7 · Accepted solution]

Hello @Anonymous , 

I saw two major flaw in your model, 

1. First and foremost you have internal boundary condition. Those must be removed or be modelized in another way.
   1. What you could do is supress the tank from the mesh and keep your BC as you did. 
   2. the other aspect that cause problem is that you have, on the same surface, a pressure and a volume flow rate BC. You can't have them both, i suggest you to keep the 27.1m3/min. 

The second major problem is your surface where you apply your P=0 BC. They are too large, recirculation will appears on those surfaces. Withdraw the pressure bc on the lateral face. Keep only the one who is opposed to your intlet (surface40)  You can add slip/symetrie on the side face to neglect the drag.

Hope it helps 

Fred

[Anonymous]

Hello Fred. I am sure your reply will help. 

Tho i am no sure i understand well your observations. On the internal BCs: Does this refer to my volumetic or masic flows as in they are internal to the Air volume? I took this video as a reference https://www.youtube.com/watch?v=nlr8CHQhigs If so, i see not much diference in aplying this BCs to the example in the video. Please, if you could elaborate a bit more on this observation for i am not sure how to apply the necesary changes you suggest. 

     1. I will try suppressing the tank. But will i see the flow bouncing off it? (I had in mind refining its mesh to prevent the apparent seeping)

     2. I had applied it that way, with only flow rate, but in the results i appeared as if it did not flow (with velocity it did look like it flowed but with volumetric it did not)  What is the issue with applying both flow and pressure?

In similar fashion on the same video i see a pressure outlet with a big perimeter. The reason i applied them this way is because in either surface40 or surface38 (depending on the scenario) i will have ambient air wind blowing and the rest of Pressure 0s are supposed to simulate open area. (2 vessels in a outside enviorment, one releasing methane and other releasing CO2 at high temp., and wind blowing in a certain direction) 

       I will research more on slip/simetry because i am not sure how it works. Would just aplying the inlet wind and the rest as s/s reflect my case? 

       As is, i did not visualise or identify recirculation on the Air. Where i seem to see it is in the methane outlet and the exhaust outlet. (i am considering to check the fully developed flow to prevent this aparent recirculation)

Hope to hear from you again. Best regards. 

[marwan_azzam · Accepted solution]

Hello,

Thank you for sending the model.

In addition to what Frederic said:

I ran it here and was not able to get the same plot you show in the image in your post.

To answer why the scalar seeps into the solid, it is just interpolating through one element between a zero and non-zero value.  I would not worry about it.

Having said that.  You have that small inlet where you have both pressure and flow rate defined.  If you know the flow rate delete the pressure.

Also, I don't see why you need any of the Steel parts.  I would suppress them all.  This is a flow analysis and they do not contribute to it.

Marwan

I would also refine the mesh around that small inlet to better capture the flow.

[frederic.gaillard.7 · Accepted solution]

Hello Ivan,

Internal BC

As the name suggest, boundary condition should be applied at the limit of your model, so when you apply BC on the interface of your chimney and the atmosphere, where they are surrounded by fluid, are an exemple of an internal BC. This probably explain your ''leaking problem'' inside the tank. Something, it might be hard to apply BC in the middle of a model, so usually, the work around is to suppress a part of the model and apply a BC on one of its surface. 

• I will try suppressing the tank. But will i see the flow bouncing off it? 
  • The flow will follow the BC applied
• I had applied it that way, with only flow rate, but in the results i appeared as if it did not flow (with velocity it did look like it flowed but with volumetric it did not)  What is the issue with applying both flow and pressure
  • In proceeding this way you over constraining your model. Check this video after 25min 
  • Correctly using Material and Boundary Conditions in Autodesk CFD 

Hope it helps 
Fred

[frederic.gaillard.7 · Accepted solution]

Hello Yvan, 

i would also pointed out another problem : the recirculation over your outlet. 

Right now you have a mass imbalance around 30'000g/s in your system. The good news is the imbalance is quite small compare to the masse flow rate who enter in your model (less than 1%) but it can alter your accuracy of your numerical prediction. 

To avoid this type of behavior you have to extend your air volume in the x coordinate.  By doing this way, you will allow the flow to stabilize and ultimately the turbulence generated by the tank will disappear. The flow will become unidirectional and the mass imbalance will tend to zero. 

Hope it helps 
Fred

[Anonymous]

I am very gratefull for both your helps, Marwan and Frederic. I have applied all of your suggestions and the model looks a million times better. I continue to make some minor modifications to the values only, the way the input is as you both suggested and informed me. Can i "accept as solution" more than one reply? 

Tomorrow i will add a next .cfz file showing the improvement in the simulation. 

Best regards!

[Anonymous]

I was unable to upload the .cfz file for future reference to forum users do to my trial version ending. (It did slip my mind when it still was possible and i apologize)

I extend my gratitude to any viewer of this post and most especially to Marwan and Frederic. 

Best regards. -ITF