[maverick90]

Hi everybody !

For a project, I need to study the impact of a pressure wave of a tornado on the blades of a fan. So, I modeled a ventilation duct with a fan inside.

At the entry-> pressure inlet. Output-> outlet pressure. I split the fluid volume of the duct into three parts: input, output and the surrounding pale.

I implemented interfaces. Two surfaces between the fluid inlet and the rotor, and two surfaces between the outlet and the rotor.

I decided to use MRF. In the Cell Zone Condition of Fluent, I selected my 8 blades, enabled "Frame motion", rotational velocity: 42 rad / s and direction rotation axis: X = 1 Y = 0 Z = 0

In Mesh Interface I connected the input rotor surfaces and the output rotor surfaces so that I have two interfaces separating the input and the output rotor.

For solution initialization, I enabled hybrid initialization. And finally, I calculated for 600 iterations. I get the following result for the pale. The result is wrong because the static pressure on the blades is constant. I made several attempts but nothing was good. It seems that Fluent don't rotate the blades even if I enabled MRF.

It would be great if you have a suggestion. Maybe a problem with modelisation? Interface? Fluent configuration? I'm really annoyed. Thank you in advance.

P.S: I know there are similar subjects but I found anything.

[maverick90]

I made some modifications and I get better results but it is still wrong.

*I deleted the interfaces. I let the fluid volume into three parts but I deleted the interface boundary conditions because it seems the interfaces are done automatically by fluent.

*In cell zone conditions: piece_5-fluide-rotor-> 42rad/s, motion absolute, rotation axis direction: 1

*Boundary condition:
- I specified moving wall, motion absolute, speed 0 rad / s for the walls of the duct (wall_inlet, wall_middle and wall_outlet) because they are stationary
-For the fan, all wall_fan.shadow: moving wall, motion relative, speed 0 rad / s for the walls of the duct, it wasn't possible for wall_fan alone because by edit, I can't change anything. Maybe it's the mistake? A problem with shadow? I do not know very well the notion of shadow.
A problem with the model, the geometry?

Here some pictures for a better understanding.

The pictures are for 42 rad/s but I get exactly the same result when I applied 0 rad/s :/

Any help would be great !

[Bionico]

Hello Maverick,
I suggest reading Fluent Tutorial about MRF and SMM: interfaces zones are required for this kind of simulation.
Have you tried Sliding Mesh Model? From my experience with fans (I'm not an expert but I simulated cross-flow fans in the past) this model is much more reliable. You have to set up a transient simulation in order to capture the turbulence between the blades.

Regards

[maverick90]

Thanks for your reply !

You're right for interfaces. I re-added these interfaces even if I still get the same results.
As you suggested, I tried SMM. But I didn't succeed to initialize in solution initialisation of Fluent, the message says I have to close Fluent, send the error and restart the software. I think there is a problem with periodic zones. I have read that SMM is more adapted for stator-rotor and I have only one rotor.

I think there is a problem with geometry but I don't know.

I split the volume into three fluid parts disconnected so that I can add two interfaces between the inlet and the rotor, the rotor and the outlet. In the volume of rotor, there is the 8 solid blades with the solid hub.

After meshing, I get in Fluent wall_fan-shadow...You can see on the previous pictures (pale=blade) It's strange. Have you any suggestion for geometry or any else?Or where could I find how simulate a fan?
Thank you very much

[ghost82]

Hi maverick,
if you're using MRF you don't need interfaces, and if I were you, I would not create them, since you can have slight discontinuities across them (even if this isn't your problem..).
So connect the 3 volumes (you have 3 connected volumes and the central one shares the 2 lateral faces with the left and the right volumes).
Check the attached picture to see if you set correctly zone and wall boundary conditions.

Instead, if you want to use sliding mesh you must create interfaces; the only difference is that you have to select mesh motion in zone panel, instead of frame motion.

Daniele

PS: if you want to share the cas file I can have a look at it.

PS2: why do you have wall fan and wall fan shadow?Shadow means that you have 2 overlapping surfaces, but for the fan you should have only one surface..

[jiangtao167]

Originally Posted by maverick90

I made some modifications and I get better results but it is still wrong.

*I deleted the interfaces. I let the fluid volume into three parts but I deleted the interface boundary conditions because it seems the interfaces are done automatically by fluent.

*In cell zone conditions: piece_5-fluide-rotor-> 42rad/s, motion absolute, rotation axis direction: 1

*Boundary condition:
- I specified moving wall, motion absolute, speed 0 rad / s for the walls of the duct (wall_inlet, wall_middle and wall_outlet) because they are stationary
-For the fan, all wall_fan.shadow: moving wall, motion relative, speed 0 rad / s for the walls of the duct, it wasn't possible for wall_fan alone because by edit, I can't change anything. Maybe it's the mistake? A problem with shadow? I do not know very well the notion of shadow.
A problem with the model, the geometry?

Here some pictures for a better understanding.

The pictures are for 42 rad/s but I get exactly the same result when I applied 0 rad/s :/

Any help would be great !

hi maverick
u can solve the problem in SRF scheme instead of MRF scheme,which u can specify the whole domain as one fluid zone and activate frame motion option then specify the parameters, SRF and MRF scheme are both steady solution approaches,if you want get a unsteady result mesh motion instead of frame motion should be used, and interface is not necessary either if that inflow is uniform in your case

[maverick90]

Thank you very much for your replies !

@ghost82: I have not my computer this week-end. I will check Monday so that I can follow your suggestions. I don't know why I have wall-fan-shadow. I don't know how avoiding these shadow objects. If there is no change, I will keep you in touch.

@jiangtao167: I will try what you suggest.

Thanks again

[ghost82]

Originally Posted by maverick90

I don't know why I have wall-fan-shadow.

Did you mesh also the fan volume (solid volume)?

Edit: from your screenshot showing cell zones I think you didn't subtract the solid from the fluid volume, so you meshed also the solid and this is the reason of the shadow walls; back to pre-processing to subtract the solid zone!

[ghost82]

Just for fun (fan ) I simulated the fan with frame motion; I made a quick and simple simulation without worry about mesh (full tetra with size functions); solution is converged with standard k-epsilon turbulence model.
You should obtain a static pressure profile similar to that in the attached picture.
If you have fluent 15 you can check my cas/dat/msh files to look at settings, you can download them here:

https://www.dropbox.com/sh/cafd5c2fow4xjbg/KSaCCNZzae

Daniele

PS: note that my rotation axis is z

[maverick90]

That's awesome what you have done. It really helps me.

I follow your suggestions I think. But I am not sure that my geometry is correct.

I join the capture of geometry:
Extrusion1: Solid_Blades
Extrusion2: Fluid_Rotor
Extrusion3: Fluid_Inlet
Extrusion4: Fluid_Outlet
Extrusion5: Solid_Hub
Booleen10: Fusion of Blades+Hub->Fan
Booleen12: Substract (Target: Fluid_Rotor Tool Body: Fan) This step is correct? Because if I do Target: Fan Tool Body: Fluid_Rotor, the fluid_rotor and fan disappear.

For Meshing, you can see the second picture. I don't see the Meshing of the fan in this step but maybe it's normal. It allows to not see the wall_shadow I guess, according to what you said.

So in Fluent configuration, I can follow what you have done. See picture to observ what pieces I have in fluent. (I don't know how you have done to separate stator and rotor). I follow exactly you have done with your file.
Just one thing, for my configuration, I have to put 0 Pa at pressure outlet and -2600 Pa (gauge initial pressure too) at inlet and operating condition: 0 Pa.

[maverick90]

Here some results. I would like to know if my geometry is correct so that I am sure I have done the right configuration. Otherwise, maybe could you upload your geometry? Just to be sure.

Thank you again for your time !

Edit: I added my geometry file. I hope you can see my geometry

[ghost82]

Hi maverick!
from the pressure profile I think you're on the right way.
Sorry but I cannot see your geometry file; I have only fluent and gambit; if you want you can upload the cas file and I will look at it.
From the cell zone panel the only difference is that you have one rotor zone and 2 stator zones; it's ok, you will have one zone with frame motion (the rotor) and 2 static zones instead of one; the most important thing is to keep attention to define velocity in the wall boundary condition panel.
Also make sure your solution is converged, let the residual go down till they are "flat": you have to see near similar pressure profiles on all your blades.
I uploaded in the dropbox link the geometry file (msh, I'm working with gambit as I said) but you can also open the cas file into fluent to look at the geometry.

Daniele

PS: "wall-piece-14fluid rotor" and "wall rotor" are the fan and the wall of the cylinder (rotor part) isn't it?

[maverick1990]

Yes, "wall-piece-14fluid rotor" is the fan and "wall rotor" is the wall of the cylinder (rotor part).

So, to be sure, it's normal I don't see the meshing on the fan (as you can see on the picture). On the picture of the meshing, you can see I don't have assigned a boundary condition for the fan but only the wall. Is it the right way?

I will look at your geometry more specifically. Thanks !

Juste one last question I think , "Also make sure your solution is converged, let the residual go down till they are "flat": you have to see near similar pressure profiles on all your blades." How can i do that in Fluent? Because I have followed what you have done in Fluent I think.

[ghost82]

Originally Posted by maverick1990

Yes, "wall-piece-14fluid rotor" is the fan and "wall rotor" is the wall of the cylinder (rotor part).

So, to be sure, it's normal I don't see the meshing on the fan (as you can see on the picture). On the picture of the meshing, you can see I don't have assigned a boundary condition for the fan but only the wall. Is it the right way?

I will look at your geometry more specifically. Thanks !

Juste one last question I think , "Also make sure your solution is converged, let the residual go down till they are "flat": you have to see near similar pressure profiles on all your blades." How can i do that in Fluent? Because I have followed what you have done in Fluent I think.

Well, if your simulation was running that means all your volumes/surfaces are meshed, so you have meshed also the fan walls; in fluent you can see the mesh on the fan surface in the general tab->display or in the contour tab->draw mesh (you have to select only the surface(s) on which you want to display the mesh).
The boundary condition of the fan wall ("wall-piece-14fluid rotor") is a relative rotational velocity of 0 rad/s.
About residuals: when you start a simulation you should see (if you didn't change settings) a chart like this:
http://aerojet.engr.ucdavis.edu/flue...tg/img1917.gif

Probably you left the default convergence criteria (solution converged when scaled residuals are <=10^-3); if the residual curves are not "flat" in fluent go to solution->monitors->residuals and delete the check on "check convergence".
So, set a high number of iterations and when the residuals will be "flat" you will manually stop the calculation.

Daniele

[maverick90]

Ok, thanks. I have no more question
I will improve the convergence and that should be better.

Thank you for being so patient (I am a beginer). I am really grateful.

[ghost82]

No problem, everyone was a beginner; the idea of the forum is to share something if you know how to do it, or if you think how to do it .

[maverick90]

Re-Hello,

I would like to know the torque of the fan so I go to Report->Force->Moment-axis-of-rotation and I get a moment but the value is wrong. Is there a specific configuration to do?

[DDD]

Hi, i have a problem very similar to this one. I have a rotating fan and i want to study the flux of air created by rotation of fan blades. I created a big parallelepide with the fan inside and i used these setting:
- cell zone condition for fluid with enabled "Frame motion", rotational velocity: 50 rad / s and direction rotation axis: X = 1 Y = 0 Z = 0
- Boundary condition:
for the lateral walls: moving wall, motion absolute, speed 0 rad / s because they are stationary

for the fan: moving wall, motion relative, speed 0 rad / s
for the wall

for the walls perpendicular to X, pressure-inlet and pressure-outlet, moving wall, motion absolute, speed 0 rad / s

- k-epsilon model

- hybrid initialization

Talking about velocity, if i put the fan in a "long parallelepiped" i see what i thounght infact there is a sort of vortex. X velocity is very small but it probably depends on fan shape.
What i can't explain is the fact that if i use a very big parallelepiped with the fan inside i have that flux close to lateral wall is very fast and flux close to fan blades is very slow. In my opinion it has to be the contrary because rotation of fan blades product the flux. Does someone know the reason why i see this thing? Have i committed some mistakes in the simulation?
Thank you for your attention.

(the imagine that i can't explain is the last one )

[ghost82]

You are simulating your case with one single reference frame; you should use instead multiple reference frame. Create a fluid volume close to your fan and make it rotate; the sorrounding bigger volume will be stationary.
Read some tutorials about multiple reference frame or read posts above nad see pictures.

Daniele

[DDD]

Ok thanks.
But making some attempts i discovered that this configuration gives me the results that i expected (i attacch two imagines):

- cell zone condition for fluid without enabled "Frame motion"
- Boundary condition:
for the lateral walls: stationary wall

for the fan: moving wall,rotation, motion absolute, speed 200 rad / s

for the walls perpendicular to X, pressure-inlet and pressure-outlet

- k-epsilon model

- hybrid initialization

In other words allthing is stationary except to fan that is defined as "moving wall". Is it wrong or not?

Besides i have another question. Using that configuration but without inlet and outlet but only stationary wall (in other words a paralleleiped of stationary wall with stationary fluid and moving fan) i don't see a convective flux as i expect, flux is always very slow... Can it depends on fan shape or did i committ any mistakes in simulation?