Mass flow
 

Hi,

I´m facing a Problem with the flow rate results from my Simulation.
I have a gasfeed (both sides closed), square sectional area. The inlet is in the middle on the bottom and I have some holes in the top equidistant. When I calculate the flow rate in each hole with the funtion calculator I observe that it´s not symmetric.
The Operating Condition is 1 Pa; pressure outlet 0 Pa, velocity inlet = 0,08 m/s.
In attach you can find a sketch.
Could someone help me?


thanks

Roughly speaking by the look of your sketch & parameters, probably one of the only reasons for non-symmetrical results could be the mesh..however I am assuming that your mesh is structured and symmetrical as well..? Have you checked by using finer mesh? What flow model & sub-model are you using (Laminar/ Turbulent, k-E, etc.. ?

Hi,

I´m using unstructured mesh and laminar model.
I don´t know how to do a structured mesh in a 3D square section model. Could you help me?

But I have tried with 500.000 / 1.000.000 / 2.000.000 and 5.000.000 elements and in all of them are not symmetric and Keep changes the results.

In attach the mesh I used withh 4.000.000 elemnts.

Not sure about the order of asymmetry or the error magnitude but the mesh does seem pretty random... so can you mention a rough error %age you are encountering? I am assuming all outlets have different mass flows..?
For mesh optimization, try fixing the max. element size and opt for hex dominant mesh OR face meshing first on rectangular faces, then on circular faces of outlets and lastly on curved surfaces if outlets would probably do the trick.. I am not at all an expert in effective meshing so won't be able to recall exact details but i believe it wouldn't be too difficult considering your case spending some time on mesh method and element sizes .. time spent on meshing would be time well spent so a quick video search for a tutorial or for hex mesh in the meshing forum would prove pretty fruitful..

By the way when you say it keeps changing the results on every increment of mesh elements, it means you haven't at all reached the grid independence and problem lies in your mesh.. if further increase of no. of elements may penalize you significantly on computation power then you may consider simplifying the model accordingly..

Yes you are right... I´m having around 10% or 15% difference from one Simulation to another increasing the refinement of the mesh.
I will try to use face meshing as you mentioned. But when I use face meshing it doesn´t let me choose the mesh method (hex or tet). Am I doing something wrong?

Yes face meshing is different from applying hex or tetrahedral mesh method.. you're doing it right, just keep mapped meshing option on..

Do you think Inflation (10 layers) is also a good idea in the outlets?

Yes sure it would always enhance the near outlet result if you may need them to be.. but i guess the initial step would be to have a symmetric mesh and run to ascertain symmetrical results... inflation layers would ideally be a part of grid independence routine once symmetrical results are established..

I have done a new mesh with hex elements. (attach)
I got 4.000.000 elements.
What do you think?
How should I know if it is symmetric or not? Just visual? Or there is any tool I can use?

it seems much better now, would be fairly realistic to see more convergent & symmetrical results.. Not sure about any tool to check symmetry.. running it to evaluate the difference would be something to look at... I am not sure about the multizone feature details used here nevertheless shouldn't stop you from giving this a go...

It´s running now the Simulation...
Let´s see what will happen :)

As it will take a while to finish, tomorrow I post here the result and we can discuss if you have time ok?

thank you so much for you guidance

It works pretty well... Now it´s much more symmetric. :)
What would you suggest in order to study the grid Independence? This Simulation I have run with 1.000.000 elements.
Would you say to add Inflation at this time? How many layers?

Good to know.. you could further try and enhance this by face-meshing the outlet circular faces and curved surfaces separately..
Up to best of my knowledge, inflation layers are usually for the accuracy of results at mesh elements near the boundary of flow domain so that would not entirely reflect grid independence however adding 3-5 inflation layers on the outlet nozzles/ tubes normal faces (if of particular interest) would always generate much more precise/ detailed results.. the grid is pretty fine already roughly speaking.. but until unless you do not have a benchmark for your results or per your expectations, increasing and decreasing (yes decreasing! because you may have vitally crossed the grid independence point at a considerably coarser mesh) mesh elements with acceptable percentage error & tolerance would be essential for conclusion..

Thank you... I will do that...

Just one question regarding vector plot Animation (if you know). I tried to animate the vector plot in the YZ plane. Basically it starts with the gas getting into the pipe through the inlet and going out through the outlets. Than it seems to Close both inlet and outlets and the animations Keep going Forward. Then starts again. What should I catch from that? Why it seems to Close the outlets and inlets? I suppose there is any relation with the fact that it is steady Simulation. Do you have any hint about that?

In this meanwhile I´m running the new Simulation focusing on the grinding Independence.

thanks

Not sure about closing the inlet or outlet.. that is probably related to the flow parameters.. would probably need more details to comprehend that... However, yes all of this is because it's a steady state analysis and the streamlines/ flow is fully developed hence repeating the flow path..

Hi Fresty,

After the Simulation with 2 millions I got different results from flow rate. Is still nearly symmetric, but the flow rate in the middle is increasing in comparison with the sides. It´s feasible because the inlet is in the middle. But my concern is because now i shoulg refine even more the mesh and the Simulation will take to much time (I think almost two days) as the Simulation with 1 Million elements took almost 24hours.
What should I do? Am I going to the wrong direction? Because afterwards I would like to simulate with two inlets or even 3 inlets to see if I will have a better flow rate Distribution.

The simulation is ultimately what one intends to yield out of it so you would have to set goals & parameters to make sure you're heading in the right direction..
What is the percentage error this time? How far are the results from your benchmark/ validation data?

If you are planning to go ahead with grid independence and further optimization (assuming your percentage error is still too high to accept)..the ideal way would be to reduce (unnecessary) complexity of the model.. few quick changes would be to use symmetries in your model if the orifices are co-planar and model is somewhat repetitive.. from what i can see (looking at the first 2d and rest of the isometric views you have posted) you could straightaway cut the model in half at the plane intersecting the inlet and outlets..then further slice in half from the plane perpendicular to the cut section from the centre of the inlet & the middle outlet... this would give you 1/4th of the model (from the inlet POV) that you currently have and of course reduce the computation time massively.. once you plan on increasing inlets to compare, that model could also be simplified by symmetry or periodicity accordingly..

Hope this helps your cause as all of these are deductions from what i could comprehend about your simulation from the provided info..

Thank you so much for your answer.
But regarding Benchmark, I don´t have it. There are not so many studies in low pressure gas flow. That makes the development more difficult.
And as about your suggestions to cut in symmetry planes, I think ist a very good idea... I will try.

thanks