[Vaaj]

I have reduced a 3D domain into a 2D (planar) domain. The inlet for 3D is a face(surface) at the circular pipe inlet. For the 2D it is an edge.

Is my mass flow inlet same in these cases? or only the mass flux remains the same?

How do I convert mass flow rate inlet initialization between 3D and 2D planar domains?

[FMDenaro]

Originally Posted by Vaaj

I have reduced a 3D domain into a 2D (planar) domain. The inlet for 3D is a face(surface) at the circular pipe inlet. For the 2D it is an edge.

Is my mass flow inlet same in these cases? or only the mass flux remains the same?

How do I convert mass flow rate inlet initialization between 3D and 2D planar domains?

physically the flow rate (rho*u_av*A) is never the same... in 2D you have a virtual area given by the line lenght of the inlet x 1 (unit lenght) but in the pipe the cross area is a circle.

[flotus1]

I guess this is a Fluent question...

First of all, 2D planar is the wrong approach for an originally axisymmetric geometry. If you use 2D axisymmetric, you can use the same value for the mass flow rate at the inlet as in the 3D case.

A mass flow rate in a 2D planar case can be calculated like this



where H is the height of the inlet in the 2D planar case, is Fluents reference width for 2D planar cases (1m by default) and is the surface area of the mass flow inlet in 3D. This should yield the same average flow velocity if 2D planar is a valid simplification for your physical setup.

[FMDenaro]

I agree... but this way you change the physics of the problem...the Re number will be different, insn't it?

[flotus1]

For cases where the 2D planar approach is valid, the Reynolds number should be the same in 2D and in 3D with this approach.

Imagine the inlet in 3D is a rectangular plane with dimensions 0.1m x 0.1m and the mass flow rate is 1kg/s with a density of 1kg/m³. This yields an average flow velocity of 100m/s.
Switching to 2D planar: the mass flow rate according to my formula is 10kg/s. If I am not mistaken, this should yield the same average flow velocity in Fluent and thus the same Reynolds number.

[FMDenaro]

Originally Posted by flotus1

For cases where the 2D planar approach is valid, the Reynolds number should be the same in 2D and in 3D with this approach.

Imagine the inlet in 3D is a rectangular plane with dimensions 0.1m x 0.1m and the mass flow rate is 1kg/s with a density of 1kg/m³. This yields an average flow velocity of 100m/s.
Switching to 2D planar: the mass flow rate according to my formula is 10kg/s. If I am not mistaken, this should yield the same average flow velocity in Fluent and thus the same Reynolds number.

Consider the Re= u_av*H/ni, (u_av*H) being the volumetric flow rate. Clearly, the Re number is the same in 2D and 3D provided that u_av*H is the same.

[flotus1]

So we agree since H has the same value in 2D and in 3D and my formula keeps u_av constant?

[FMDenaro]

Originally Posted by flotus1

I guess this is a Fluent question...

First of all, 2D planar is the wrong approach for an originally axisymmetric geometry. If you use 2D axisymmetric, you can use the same value for the mass flow rate at the inlet as in the 3D case.

A mass flow rate in a 2D planar case can be calculated like this



where H is the height of the inlet in the 2D planar case, is Fluents reference width for 2D planar cases (1m by default) and is the surface area of the mass flow inlet in 3D. This should yield the same average flow velocity if 2D planar is a valid simplification for your physical setup.

Yes, the same H and same averaged velocity give the same Re number.

The doubt was about the formula you wrote, consider the same in terms o the volumetric flow rate:

(u_av*H*1)2d_planar = (u_av*H*h)3d *(H*Lref/A3d)

right?

[flotus1]

I think you need to replace *1 on the left side of your formula with *L_ref and that´s it. Otherwise the units don´t match.

Anyway, I quickly checked the implementation in Fluent. My initial assumption was correct and so is the formula in my first post here.
The only caveat: when post-processing the volume flow rate at a mass flow inlet, fluent uses the depth from the reference values tab to calculate it. The flow velocity is indifferent to these settings. I don´t know if you can even change the value of L_ref to any other value than 1m.

[Vaaj]

Thanks a lot for giving so much of thoughts on this problem,

I did use the mass flow for 2d before, by taking the the inlet width * 1m reference as suggested by you.

The flow is a compressible flow and I have the pressure, mass and temperature (or density changes) variation with respect to each time step and I want this varying property to be initialized at the inlet through out the run time.

The original simulation is to capture how the air flows from a 0.6 L container at 21 bar(a),300K to 20L spherical container. Since, I am not able to close the valve at the end of 45 milli seconds and the simulation has to run for 60 ms and the feeding phase is shorter, I modeled the inputs of air and got the time varying functions assuming isentropic expansion.

I am not able to reach the desired end point where the air at the end of 60 ms is at 1 atm and 300 K inside the 20L sphere.

It is a compressible, transient flow. Later I will be adding particles to it.

Questions:

1) If I want to simulate the pressurized container, how to mimic the valve action ?
2) If I model the air flow inlet without the container, how do I initialize properly. Since i have all inlet data how to initialize everything with UDF or transient profile (I tried profile but not reaching the final solution).
3) How to let Fluent know that the final boundary conditions are 1 atm and 300 K iniside the entire zone of spherical chamber?

Pictorial representation of mesh and the simulation conditions are in this link. I m not able to post image here!

https://ibb.co/dEQCgQ



https://www.cfd-online.com/Forums/ma...tml#post647897

[FMDenaro]

Originally Posted by flotus1

I think you need to replace *1 on the left side of your formula with *L_ref and that´s it. Otherwise the units don´t match.

Anyway, I quickly checked the implementation in Fluent. My initial assumption was correct and so is the formula in my first post here.
The only caveat: when post-processing the volume flow rate at a mass flow inlet, fluent uses the depth from the reference values tab to calculate it. The flow velocity is indifferent to these settings. I don´t know if you can even change the value of L_ref to any other value than 1m.

I was thinking about such expression... Assuming that (u_av*H) is the same, doesn't reduce to 1 = h*(H/A3d) ??
And A3d is, of course, h*H ... I think that I'm not understanding correctly such correction implemented in Fluent...