Learning Forum

[Agung Limowa]

hi, I'm modeling a duct and a tunnel where the duct is inside the tunnel (3 of them). the duct have fan to exhaust to suck all the existing air out. My problem is when i use mass flow outlet and mass flow inlet as a boundary condition, i got a floating point exception warning, but when i use velocity inlet and pressure outlet it give a good result. My problem is pressure outlet is not working at my case because the existing of the fan make the pressure is different and i have control the pressure, what should I do?  Theres any way i can control the flow just by pressure ?

[Rob]

Maybe restrain yourself to one thread? 

Mass in & mass out and velocity in & velocity out will have problems, which is why we always leave a flow boundary floating to let the solver balance volume/mass in the domain. You need to look at your entire model and carefully work out what values you know, what you don't know and what can be calculated. 

[Agung Limowa]

Hi, I'm really sorry but i can't find my old thread, i'm asking back about my problem, after i use the outley as pressure outlet it, always give me divergence after 200ish iteration and the floating point exceed, what sees the problem?

i have 4 velocity inlet boundary condition 3 pressure outlet and 2 masflow outlet, i dont know what might be the cause of this problem ?

[Rob]

Assuming the mesh is OK, and you're using all the default for everything else try dropping the Courant Number/Pseudo Timestep. 50 or 0.1 respectively may be a bit more stable. 

[Agung Limowa]

i will try it thankyou

 

[Agung Limowa]

Hi again, i have try another method but it seems like it is stationary state what might be the problem should i iterate more?

[Agung Limowa]

And also the report definition give a constant osilation what should i do ?

[Rob]

Given the level of convergence I'd look at lowering the time step and keep going. However, is the system transient? I mentioned the two underrelaxation terms for the Pressure Based Coupled Solver, not transient. 

[Agung Limowa]

 

yes it is transient analysis, i will try to keep going and thank your for your advice, i will reach out if something happen 

 

[Rob]

Why? Also, at the flow speeds you're using how long does it take flow to get from one end of the system to the other?

[Agung Limowa]

so the goal is to look the airflow and the affect to the temperature in certain amount of time, that's why i used transient analysis, is it something wring with it ?

my flow speed about 20m/s and the domain is about 1800m long 

[Rob]

Not necessarily, it's just with 20m/s you're resolving a time scale to converge 20m/s crossing a typical cell size; but also need to run to ensure the transient solution isn't still seeing the initial condition as a result (ie the solver has changed the flow to be correct rather than what ever you set at t=0). 

[Agung Limowa]

ok, i got it, after i do several more iterations, the continuity is have raised, what it is mean? is my solution cannot be converged, i still don't get it

[Agung Limowa]

as an information, i have tight cell resolution around 16 cell of 8m cells <0.1 orthogonal quality, Is it give huge difference, i deny it because i thought is just really small amount cells and it quite large model, I've tried to reduce it and that's the best number i can get 

[Rob]

Which may cause solver issues if they're in regions with high gradients. 

Also, check the time step against the cell size: how long does it take for flow at 20m/s to cross a cell? 

[Agung Limowa]

hi, the time to cross a cell is quite fast the whis is abaut 0.0001 s, and also as you suggest i have continue iterate and until 3000 iteration the solution (velocity) get converged but the residual is remain the same what should i do ?

[Agung Limowa]

hi again, i have try using the same model and when I raise the velocity in the inlet what happen is a floating point exception, so i conclude that my problem is not on my mesh right? but my boundary condition ? and also what can make this problem happened? 

[Rob]

It's a transient calculation so you need to resolve the flow with time, and converge all time steps. The iteration count is irrelevent, it's the number of time steps you need to consider. As you're not resolving the time scales in the domain I'd be very wary of the results. 

Changing the boundary condition means the flow sees a sudden jump in value, again, you need to consider time scale. 

 

[Agung Limowa]

hi, I have continued til the end of the timesteps, and it shows a straight line to the solution, so it means the solution is clear, right?

[Rob]

It means it's not changing (much) at the position you're monitoring. I can't tell you a solution is correct without a lot more information (which I'm not allowed to do) and also because I'm not permitted to tell you if a model is correct (I've got to be careful regarding experience & engineering knowledge to adhere to the Export Laws). 

What I do suggest is doing a lot more post processing and discuss both the model and results with the project supervisor. Explaining what you've done to someone sat with you will highlight any oddities in the results, but you'll also spot things as you explain. 

[Agung Limowa]

okay thanks for the advice, I am just really confused about the residual, is the residual the main parameter to say that one solution is converged? which one we prioritize to the solution the report definition result or a scaled residual, is the residual as my photo is acceptable ?

 

[Rob]

The monitor isn't a residual. It's a report from Fluent of a value at every iteration/time step. When it's level it's a good sign that the model isn't changing at that location. However, as you're monitoring an average you may be masking localised changes in value. 

Residuals are the solver reports and are a function of how much the overall solution is changing. 

Convergence is typically OK when monitors stop changing, residuals drop by the required number of orders of magnitude and fluxes balance. For a transient run the extra requirement is that previous time steps have converged otherwise you risk a model that's wrong but returning to "correct" over time, so at some point it will be OK. If you check the AIS courses (Learning on here) there will be something covering this in the Fluids/CFD modules.