Discussion Forum

Hi

Well I'm no CFD expert, but my advices are:

for your geoemtry, redraw your circle slightly smaller i.e 22.5 or 23 mm radius. Now you are going all to the edge of the rectangle, this makes silver points that are very tedious to mesh and gives you a very local and fine mesh, hence it takes ages to solve.

Then CFD is a complex physics, I would suggest to start with Laminar flow (even incompressible) with a lower in-flow velocity, or even to ramp the inflow with a smooth step function and a parameter. Then to switch to more advanced turbulent modes physics, and even use the laminar flow case as initial velocity and pressure for your turbulent study.

I would aslo suggest that you see with your system admin or your COMSOL rep to get hands on a more recent patched version. I wounder if the default sover sequence will not be more complete with wall effect presolvers then.

ANd as you do not have a pressure output, I would force a (or a few) p=0 point constraints, to give the solution a fixed point for stabiising the absolute pressure (it's also a dependent variable), you could take one of the 4 points in the far end of your channel.

Now with such a "small" inlet forsucha large outlet slit, I would asume that yourairflow will remain rather concentrated and exit somewhere in the middle of the slit, and rather locally

Finally, when you have complex models and solving cases, use the solver "plot while solving" and for each solver steps to be able to see better what is happening

--
Good luck
Ivar

Thank you very much Ivar!

I have also tried to limit my problem first to 2D, but there I still encounter some problems with initial values.

You have mentioned step function. How can I set it up on inlet value?

Hi

In V4 try the Definition Functions STEP then open the advanced tab to get access to the slope value, do not forget to plot to check its shape, you often need a time lag of up to half the slop to start fully at "0", this is however not always advisable, sometimes its better to start with a "small" value else the solution is too "flat" and the solver does not always manage to find any optimum

--
Good luck
Ivar

Should I then use as velocity at inlet expression like:

V*step(t)

trying to do so I still have problems with obtaining "coherent initial values".

Do you know any tutorials for fluid flow module, that I could study and learn from them ?

Best regards,

Mike

Hi

try to start with a laminar flow and V=1m/s to get the system converging, then increase the velocity and then switch to turbulent

--
Good luck
Ivar

Hi,

First you need to redefine your inlet circle a bit smaller. Then you can use subsequent steps to increase from a small velocity, abotu 0.9 m/s, to the final velocity you want, 5.9 m/s.
You can do that in several ways, going time-dependent can require a lot of computational effort. If you do not need to analyze transient solutions, you may want to divide the simulation into several stationary studies so that you can intervene at each study level if anything goes wrong.

To reduce computational cost, you may also splti your domain and enforce a symmetry condition.

I also strongly recommend to use direct solvers, possibily PARDISO, when doing CFD. Please find attached a sample about how you can solve your problem and a picture of velocity+streamlines.

Cheers

Thank you very much for the hints, now I can get clo0ser to my results.

There is just another issue I cannot resolve. In the real setup, the outlet is made of small long tubes, therefore enforcing only normal direction of the outflow. For 2d laminar flow model, there is such a option in boundary condition. How can I approach this problem here?

Hi,

I am not sure it would be a good idea to force the outlet to have an outflow normal to the cross-section. If you are looking for a realistic solution, while checking whether the normal component is the most important, you may simply impose a pressure or stress condition at the outlet.

However, if you really want, you may impose a velocity condition at the outlet, and choose normal outflow velocity or choose velocity field and specify the normal coordinate only.


Cheers

Thanks a lot - your guides are pushing it forward.

Nevertheless, when I utilize your model, whatever pressure I set at outlet, the flow profile doesn't change (it seems to only bias the whole solution).
Another problem I found is that in this model : there is always a "backflow" into the chamber next to the inlet, while measurements show no such a behaviour. I have an outlet flow velocity profile measured:

x 40 125 210 290 375 460
flow 0.55 1.12 0.83 1.11 1.22 1.52

I also know that there is 10mbar of the pressure at the inlet.

Because visualisation of any changes of 3d model takes long time, I thought about simplifying it to 2D model. But here I still encounter some problems with finding proper boundary condition.

As I understand it I should implement a boundary, which will act with force as "wall" for horizontal flow, and as viscous friction for vertical. Then I would manipulate the viscosity parameter, to obtain known pressure at the input.

Do you have any suggestions how to construct such boundary condition without implementing horizontal wall each 1mm ?

Hi,

I am sorry but it is quite unclear to me what you mean when you say that "I should implement a boundary, which will act with force as "wall" for horizontal flow, and as viscous friction for vertical. "; how are you supposed to distinguish between an horizontal and a vertical flow? Here, we are talking about fluid mechanics, that is continuum mechanics, how can you distinguish between one direction and the other?

Also, I don't think you can say there is a problem in the model if you have a "backflow", I think you may need to refine the mesh. Please remember what I showed to you is a way to get a solution, it is up to you to get a perfectly working model.

Finally, you may want to think a little bit about the meaning of a pressure outlet. If you increase the pressure at the outlet it is extremely unlikely you will see major changes in the flow pattern, it is rather likely that by increasing the pressure at the outlet you will simply get an equivalent increase of pressure throughout the domain (maybe that is what you meant when you wrote "it seems to only bias the whole solution").

Cheers

Hi

indeed the concept of "Gauge pressure" and "absolute pressure" is often misunderstood, and perhaps not enough enhanced in the doc.

Most CFD simulation are done with a "Gauge pressure" (and p=0 at outlet is handy) , while COMSOL adds an absolute pressure to get the total fluid pressure to extract the physical characteristics of the fluid in correct absolute values (check the absolute pressure and the equations in the main physics node)

--
Good luck
Ivar

I think you are right about the documentation. It took me a moment, but finally I have reached to the point, where I know what I am looking at.

As I mentioned above, I decided to use "Boundary stress" with "normal stress, normal flow" condition and :outlet: boundary type.

Now I am pretty sure, that my boundary resembles an array of fi 1x10mm holes. Nevertheless I still get solution which is way different from measurement data, as I described above.

Do you have any suggestions how could I get them more close to each other?

Best regards,

Mike

The output in the real model consists of number of fi 1mm holes in 10mm thick block - therefore it enforces only normal flow.
I know that I could try to draw them - but it will be tedious task and will complicate my meshing. In order to obtain filimar effect I wanted to implement a force on the boundary which will be in form of F_x=a*v_x F_y=b*v_y, where big enough value of a will imitate the vertical wall, and b will correspond to viscous friction in the channels.

Fortunately I dig into options and I tried to apply :Boundary stress: with "normal stress, normal flow" condition.

I have slowly increased f_0 parameter for normal stress in order to obtain pressure at the inlet, which I have measured in experimental set-up.

My solutions converge well, but unfortunately I get totally different flow profile, then I get from experiment. Model output is almost a step function with rather steady "high flow" region, while experiments show almost linear profile.

do you think that adjusting turbulence parameters can lead me to solution closer to the experimental results?

Best regards,
Mike

here is the model

Hi,

All right, now I think I can see some flaws in the reasoning. You built a model with a single outlet, if you have several small holes as outlet you may not design a single one and then pretend it to have normal flow only.

It is important to note that normal outflow is a consequence of the design of the domain; therefore it will be extremely difficult that you will manage to force a normal outflow if the design of the domain does not support it.

CFD is intertwined with geometry and even small changes in it may determine large differences between real results and computed ones.

You may re-design the domain to match the actual geometry of your device. Please note that you just said that "The output in the real model consists of number of fi 1mm holes in 10mm thick block", however you have designed a single rectangular outlet.

Cheers

Yes I did so, because the outlet is a matrix of those fi1mm holes in 10mm thick plate, which is placed where my outlet is.

But if you suggest detailed modelling of it, is there some easy way to select the chosen faces of domains created by "create matrix" command while building geometry?

I would like to create the array of holes, and then select only their sidewalls to become "inner walls". How to do it with few hundreds of faces?

regards,

Mike

Hi

I would say it's not only the holes but also the tube length that will have some effect (pressure drop ... ) and then the entry shape, with a cone no cone ...

For the geometry you ca draw a rectangle for the surrounding, and therein a circle for the first hole, then repeat that on an array definition with range() operators if the mesh is regular. Then if this is done on a workplane ou can extude that over 10 mm or whatever needed. But you will end up with a locally detailed mesh, hope you have enouh RAM.

For selection you have boxed selection and Definitions Selections nodes of different types, inclusive a geometrical coordinate definition one

--
Good luck
Ivar

I have an idea how to build the geometry, but I foresee big problems with selecting the faces which should become outlet, and which should become walls. Manual selection will take ages and will be very error prone.