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

Just one more question, as the inlet will be divided by 4 ... I will use a quarter of my previous model... The inlet velocity (BC) I should also divide by 4, correct?

theoretically yes as volumetric flow is directly additive (per my humble understanding)... this is something you could always check i guess.. not sure how fluent defines symmetry bc option.. it may be possible that once symmetry planes are defined the velocity input is considered for the entire inlet area rather than the 1/4th.. however just go through the below for an insight..

https://www.sharcnet.ca/Software/Flu...ug/node258.htm

Hi,

I increased the number of holes and than my solution doesn´t converge anymore. There are reverse flow in practically all pressure outlets. Each hole I called as one outlet. I have a 500 mm pipe lenght and 19 holes (2mm Diameter). The pipe has a square sectional area (L=30mm).
Laminar flow , steady state.

As there is the presence of reversed flow, it means that the pressure inside the gasfeed is lower than the pressure out of the Domain? If it´s correct how can I identify that in the Simulation? How to see the pressure inside the pipe and out of the Domain?

One additional Information, if I increase the velocity inlet this Problem (reverse flow in the outlet) vanish out...
What´s the Explanation for that?

What are your outlet BCs? Have you specified the Outlet pressure & Operating Pressure? what are the wall conditions of the pipe?
The local pressure drop at a certain region could also result in reversed flow.. in your case the local pressure drop increase at the outlets due to increase in local velocity seems sufficient to have caused reversed flow by increase in dynamic pressure loss..which you probably should expect firstly because of low pressure flow and secondly as you mentioned earlier that the pressure difference to drive the flow is only 1 Pa (please correct me if i got it wrong).. by increasing the velocity you're helping the flow to have enough momentum to pass through even if the pressure drop is the same (in physical terms)..
You could use an expression to see the pressure at inlet as well as at outlet however you could always get an approximate idea from contours considering the issue is quite prominent already..

The Outlet BC is pressure outlet = 0 Pa. Operating pressure = 1Pa. You are right, the pressure difference to drive the flow is 1 Pa.
How can I use this expressions? Where are them?

Another addittional Information... This Problem of reversed flow doesn´t appears with just 7 holes in the same conditions. It´s the same Explanation? With 7 holes I have less dynamic loss?

I am not really well versed in Fluent UDFs or expressions, however, it shouldn't be hard to find them with a quick search in the forum.. they should be something like (not the right syntax for sure).. area-avg(pressure)@location ...

Yes that would be the reason.. the increase in velocity (momentum) is necessary to cover the increase in number of outlets..

Now I just made a test to see if it works accordingly. I reduced the outlet from 2mm to 1.5mm. Then I could observe that the mass flow rate was the same because the discharge area reduced but the velocity increased to Balance and also the pressure inlet increased.

So maybe to vanish with the reversed flow maybe a solution is to increase the Diameter of the holes, than the velocity will reduce and also the pressure drop. Am I right in my way of thinking?

Yes i believe that should be the case.. however, you could compare your test situation with another by increasing the outlet diameter and see the physical changes in the system. It would always be more or less a trade off situation and you would have to find the optimum design point between change in diameter/ no. of holes/ dynamic loss etc. (given that your pressure difference to drive the flow remains same).

One Thing that I could observe is that the mass flow rate (kg/s) is almost the same in all holles. This can be explained by the fact that is a steady Simulation, flow is fully developed and the pressure difference that drive the flow is small? Or do you have a different opinion?
Because I could not see any effect off back flow because of the fact that the sides are closed.

Also the viscosity effect is almost negligible, so there is not many loss in the pipe, right?

Please see the attachment:

The first one is with 7 holes and the second one with 19 holes. Both in the same conditions. From the pressour contour can be seen that both has negative gauge pressure in the outlet. But why just in the second one with 19 holes the reversed flow appeared? I cannot understand that...

Hi,

I increase the Diameter of the outlet to find the "borders" of my Problem. When I increased, started to happen "reversed flow". It means that for my purpous, this configuration didn´t work well with larger diameter. Therefore the convergence (1e-6) is not achieved anymore. This is what I would expect, since I´m reducing the internal pressure. My question is: How can I quantificate this amount of reversed flow? How can I evaluate the way it is affecting the gas flow?