Simulation of a simple duct inlet

[Anonymous]

Hi @David.Short. and @Jon.Wilde !

So now in a different thread..

My problem consists of running cfd for a duct inlet device (air-flow), and for this, I need to run different geometries. So basically, the idea is to set a constant flow speed in the duct-outlet, and measure the boundary layer thickness at some position of the duct and/or check whether there is any flow separation, in order to decide which inlet has the best performance.

So far, I was running only axi-symmetrical 2D only because it's way faster and this simple case allows it (duct flow), but we are doubting pretty much about the results we've got, therefore we decided to test a 3d model.

As an example, please see bellow my last try:

This is a half-model where this half-hemispher is the air environment and the inlet+duct is shown in the middle. I also attached the _support file so perhaps you may have a look.

Boundary conditions I set flow speed normal to the duct section, symmetry at this half-surface, and zero gauge/total pressure at the circular wall, and this back wall (suppose to be the 'room' or free-field condition).

This drawing comes from a 3d model which is composed by this half-hemispher and a inlet. This drawing I've done in Inventor and just imported to CFD autodesk. I set this hole half-hemispher as "air", or we could also call as a far-field condition. The inlet bell-mouth I set as solid/alluminium.

Here it goes some screen-shots of the progress. In the beggining it seems quite ok, flow field makes quite some sense, but after ~200 inter. it starts getting unstable and makes no sense anymore.

I think my mesh has about 1M points, solver is Low-Re k-epsilon. => Question: Is this the best option for this case? We expect to have laminar boundary layer in the begging and then it becomes turbulent somewhere in the curvature.

I mentioned I was running 2d-axisymmetrical, and for this I used sst k-omega, which consider the hole boundary layer turbulent, which therefore is not that precise.

Do you guys have any suggestions? It should be a simple simulation!

Thanks a lot!

84 inter.209 inter.246 inter.3100 inter.

[Jon.Wilde]

2D would be perfect here! Do you still have this model as it would be a much better starting point.

One issue that I can see (without digging into the setup tweaks just yet) is the spherical outlet. Here you just need a static P=0, not total by the way.

The main issue though is the shape, ideally we need to keep things simple and be sure that you never have recirculation over an outlet. If you do, you would see exactly what you are - weird results and overall instability.

So, what I would do is vent this into a long cuboid with a P=0 at the far end (or a larger room with a small cuboid outlet on one wall like most test facilities have).

Could you try it in this way?

How is this installed and tested in reality?

Thanks (and thanks for starting up a new topic too),

Jon

[Anonymous]

Hi @Jon.Wilde thanks for your reply!

yes I will try again over 2D, and soon I have it setup I share the _support file again!

In our application we have a ~10m long duct with a fan in the center speeding-up the flow. This is placed inside a quite big room. My task now is to design a better bell-mouth for the intake!

do you have any suggestion for the most suitable solver? As I said, we expect to have some laminar boundary layer at the inlet, and then a transition to turbulent.

Regarding this pressure boundary condition, we discussed this and static pressure (gage) zero means no flow at this point, in theory, right? It doesn't make much sense for me to set this condition.

Thanks again!

[Jon.Wilde]

Zero pressure (gauge) means ambient pressure. It is entirely applicable here 😉

I would worry about the solver settings later and get the geometry right first. Just run everything as default and check it works OK, then we can play with the settings 🙂

[Anonymous]

all right but static or total ( gauge ) pressure?

could please explain better your suggestion for the room design? or perhaps a rought sketch?
I'm trying some geometries here. Did you mean, the inlet and outlet should be in different rooms?

thanks!

[Anonymous]

Hi @Jon.Wilde

I think now it heads towards something reasonable.

I attached this screen-shot and the _support file again. Are these boundary conditions right?

Does this sketch make sense?

Thanks again!

[Jon.Wilde]

Just static pressure, total is used when you have closer to supersonic flow.

I would try to model something close to how you test it, but maybe a little smaller. 

I would think it ought to be like this (please forgive my very poor image) with the P=0 on the surface indicated. Be sure that that outlet is long enough that you do not have recirculation over the boundary condition.

[Jon.Wilde]

Go for simpler, just one P=0 and use an extension so you funnel the air and have no recirculation. Right now that would likely be quite unstable.

Looks a lot better though, nearly there!

[Anonymous]

Hi @Jon.Wilde !

I'm not quite sure if I understand correctly your drawing.

So, I actually run my old drawing, but now I set this right-hand part as hardwall (i.e., didn't set any boundary condition) and zero pressure at this circular surface.

For my understanding it looks quite ok.

Do you have suggestions to modify it?
My further main question now is about the solver.. for this application is "Low Re k-epsilon" the best choice? As differences among different inlets are not that expressive, we look for a good simulation of boundary layer condition in order to compare different performances of each inlet.

Many thanks!!

[Jon.Wilde]

We still need to get the basics, it is not OK that you have flow both entering and exiting over the P=0.

My drawing is basically a test room with the unit mounted on the ceiling. There is a P=0 at the end of the duct on the left.

I would start with the kw model and ADV5. With kw, you need to be sure your Y+ is close to 1 (enable Y+ as a result quantity within Solve-Result Quantities).

Firstly though, we need to get the room shape correct 😄

[Anonymous]

Hi @Jon.Wilde ! All right.

here is my last simulation

First I tried with a room connection between outlet/inlet but there were a lot of recirculation, and you mentioned to avoid it. Therefore, I remove the connection between inlet and outlet rooms. Does this room make sense for you?

Sorry but I definitely can't understand your drawing, I did my best!

Is this important to have a room for the outlet? I mean, maybe it does interfere in the duct flow profile.. I don't know! Because for my study itself, the outlet doesn't really matter.

Further, I enabled Y+ as a result quantity but seems to be all zero, i.e., all plot is dark blue.

Thanks!

[Jon.Wilde]

I must apologise, really sorry as I think I misunderstood this. I was looking at things backwards.

Your outlet is on the right?

If that is the case, what you had before was perfect.

The inlet side is what I think should be changed, so we remove that curved surface.

[Anonymous]

No problem.

Yes the inlet is at the left side and outlet at right side.

You mean, is not necessary to pay attention on what is going on with the outlet, correct?

So the drawing of message 9 is enough in terms of room design? Shall I keep that vertical side at the right-hand side w/o boundary conditions? i.e., hard wall?

what you mean with "so we remove that curved surface."?

thanks!

[Jon.Wilde]

Thanks 🙂

Message 9 - I would simply extend the outlet a little keeping the same cross section. Our general rule is that it ought to be 10x longer than the width of the tube. Otherwise, all is good.

For the inlet, can you see that you also have flow exiting here? This is not really ideal, which is why I was suggesting a larger room.

So it would be like what I shared before but with that opening as the inlet, same thing in reverse 🙂

Maybe try with what you have now and see, just keep a close eye on the convergence plot to be sure it is smooth. 

We would usually have a boundary condition further away from the test unit too (like the awful drawing I did).

OK, let's get to the solver also so you can get some results 😄

The Y+ you can see from the legend on the left hand side - you should be able to change the ISO surface view settings to identify where it is close to 1 and where not.

Try these as wall layer settings to begin with, these are usually pretty good with the SST kw model and a good guess at getting to a Y+ of 1:

[Anonymous]

Hallo @Jon.Wilde !

I increased the room size and prolonged the duct as you mentioned. I also set these boundary mesh enhancements as you mentioned.

here you can see results for both speed plot and Y+.

did I plot correct this Y+ results? I'm not quite sure..

I'm also still not quite confident about this boundary layer. With this turb. model 'sst k-omega' does it consider all boundary layer turbulent?

Thanks!

[Jon.Wilde]

I would add a few more wall layers to get the Y+ down to 1, although you could plot it with an ISO surface to understand where the 2.2 value is. 

All looks a lot better now, the inlet is only sucking in and if this stays the same, I would not change the geometry further.

Better to refer to the help guide for the technical stuff as it is already written out, no sense in me repeating and making mistakes 🙂

What you might need to do now is disable the auto convergence (or at least really tighten it) and run it a lot longer to see if the results change - I suspect the flow might stick to that wall a little better in reality.

[Anonymous]

right.

yes, i set to run fixed 3000 interactions and it looks better indeed.

I'm still not sure about the boundary layer modeling. Does sst k-omega consider it all turbulent?

would you recommend another Turb. model? perhaps this "Low Re k-epsilon"?

I had a look in the help menu, and seems plausible..

Thanks!

[David.Short. · Accepted solution]

Hi @Anonymous,

SST k-omega will resolve laminar regions just like Low Re k-e but has superior turbulence modelling capabilities within turbulent boundary layers therefore i recommend sticking with SST k-omega. Make sure you have y+ down near 1 such that laminar sub layers are captured accurately.

This thread may help explain further the near wall treatment of SST k-omega.

All the best,

David

[Anonymous]

Ok!

thank you very much @David.Short. and @Jon.Wilde.

If you say sst-k omega can deal with laminar regions as well, it is fine. We really thought it treats everything turbulent, which is definitely not good for us.

Thanks!

[Anonymous]

Hi again @David.Short. !

sorry for insisting in this point but we are still not sure exactly about what is really happening.

Within the Turbulence option, when sst k-w is selected, we see these two selection options for laminar or turbulent boundary layer. The thing that I wanted you to clarify is: if I select Turbulent (which is in fact what I did) will the solver consider a completely turbulent boundary layer over the whole wall?

In case this above sentece doesn't hold, i.e. it computes both laminar and turbulent depending whether there is a transition,  is there some 'hidden' model or feature that models the transition point from laminar to turbulent throughout the chord length?

Because again, in this case we expect to have some laminar boundary layer in the beginning and at some point the transition will occur. I would be happy to understand better what is really going on in this simulation.