[sasundar]

Hello there,

I'm new to this forum and I have a basic query in the simulation and I'm a starter in CFD.

Currently I'm trying to a simulate a burn pit flare (Jet fire simulation) with exit velocity of 148 m/s fuel is propane and release size is 12.75mm.

And I'm considering complete combustion even though in-reality it will only 90- 98% efficiency.

I have built a simple fluid domain, with Wind as inlet BC (boundary condition) with wind speed of 1m/s and rest is considered as Atmosphere with opening BC and the ground and burn pit surface as no slip wall BC.

And the fuel source is defined as inlet BC with subsonic flow regime. And flow input as velocity.

My issue is when i'm specifying the fuel release velocity as 148 m/s the RMS is not converging properly and ends in 1E-03 and results are not as expected.

But when i'm using 100 m/s as fuel inlet velocity (or less than 100 m/s) the RMS is converging good and ends in 1E-05 and results such as flame temp and incident radiation are pretty matching the expectation.

So please help me or advice what is issue if i'm increasing the velocity more than 100m/s the RMS not converging good and results are wrongs. Please correct me if i'm doing anythin wrong in the model setup.

I'm modelling in steady state analysis.

Much appreciated for your help and support.

Thanks

[ghorrocks]

If your simulation works well at 100m/s but not at 148m/s then it is almost certainly some physics causes that. You probably have a physics model you have defined which is not applicable, or the flow changes into a new regime (eg transient vorticies start forming). You can only tell by close analysis of your model's results, a knowledge of the physics of what is actually happening and a knowledge of what the models you have selected in your simulation are.

My recommendations are to:
* Check whether the models you are using (eg combustion model, turbulence model, steady state/transient etc) are applicable
* Have a look at the 148m/s results in the post processor. What do they look like? Is something weird? Do they look like they are going transient?
* Also look at the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[sasundar]

Thank you very much for your advice.

The Turbulence model is selected SST as typical taken from a literature paper on vertical jet fire simulation. The combustion model is selected Eddy Dissipation and the soot model is selected as Magnussen. These basic model are selected based on the literature paper as mentioned above.

Also please see attached post processed results of velocity and flame temp contour for two cases.

[sasundar]

Please see the attached CFX solver setup input. Once again thank you very much for your time and advice.

[ghorrocks]

My second and third points both refer to the possibility of requiring a transient simulation, but this simulation is steady state. Have you read my previous post?

You have a reference pressure of 1 [atm] and your initial condition has a relative pressure of 1 [atm], which means you are running this simulation at 2 [atm] absolute. Is this what you intend?

Your boundary "Atm" is an opening, but you specify the velocity. Normally you specify the pressure of openings as the flow direction is unknown. Is this what you intend?

You have not set the pressure level! There is no boundary which has a defined pressure. I am surprised you got anything to converge if you do this. You MUST set the pressure at a boundary somewhere.

You appear to have some very serious problems to fix