[amin.z]

Hi!
Can someone explain to me all of the difference between "mixing plane" and "mesh interfaces"?
Which solution is more accurate?

I'd be very grateful if someone help me!

[ghost82]

Hi Amin,
if I understand correctly the mixing plane is a model.
Mixing plane is also an interface, suitable for certain problems, where you can create a plane between 2 zones, a rotor and a stator.
Fluent guide describes this model to be able to average the results on the mixing plane in the circumferential or axial direction, by averaging these values (area-weight or mass or mixed-out) and by creating profiles of flow properties.
These results are passed from the downstream zone to the upstream zone, on the mixing plane.

On the other hand, an interface is a generic couple of surfaces, on which there is no specific calculation as inthe mixing plane, I think variables are only passed across these surfaces; usually they are used to connect 2 zones with different meshes or to simulate moving mesh problems.

I don't have experience with the mixing plane model, but it seems that the unsteady state moving mesh is the most accurate model.

Daniele

[amin.z]

Dear Daniele! Thanks for your reply!
You did mention the useful tips! But there are still some problems:

When should we use mixing plane model or mesh interfaces?
in the same problems which are more accurate?
and with sliding mesh which is more suitable?

My project is about the rotating air inside a rotating electric motor.
There is an interface face between two domains and I'm using periodic BC for two domains with 60 and 24 degrees! Angular velocity is 2000 rpm!
Which model do you recommend?

Thank you in advance for your help

[ghost82]

Please post a sketch of the 2 domain zones and where interfaces are.

Daniele

[amin.z]

2 photos attached
Forgive me if the photos are not clear enough!

[amin.z]

The rotary part is formed from a rotating fan with 15 blades and spinning rotor!
I'm modeled the fan with 1 blade(1:15 with 24 degrees) and rotor with 60 degrees!

[ghost82]

Ok Amin, it's clear your problem.
Consider that what you call interface 1 and interface 2 are not interfaces, but 2 (partially) overlapped surfaces: you will build one interface with that 2 surfaces in fluent, what you call interfaces 1 and 2.
Mixing plane is suitable for your problem, because you can create the plane between the 2 zones.

However, I have not experience with this model, I only used mrf/sliding mesh (without mixing plane) so I don't know if the model will be accurate enough.

I think you can try simple mrf, mrf+mixing plane (steady solver, they should not take too much time to get solved), and if you are not satisfied with your results switch to sliding mesh (unsteady).

Daniele

[amin.z]

Dear friend!
But I think this two faces are interface! I think that could choose the faces as interfaces because I'm using periodic BC!
And I used mrf with interfaces mesh and it's almost converged! But I'm looking for a method with less numerical errors!

[ghost82]

No Amin, I think that the vertical lateral faces are periodic bc, not interfaces.
You should set these faces as periodic.
As I written try to switch to the mixing plane model+mrf, then to sliding meshes, so to see if there are macro errors in calculaion.
I'm not at home now, tomorrow I will sketch what I want to say.

Daniele

[amin.z]

Oh! Amazing point!
I'm waiting for your sketch!

Tnx for your help dear!

[ghost82]

In my opinion, here is my setup, assuming 2 rotor zones and a stator (if I don't understand correctly your problem please clarify better).
All faces "parallel" to the flow should be set as periodic rotational (not interfaces!).
All couples of faces connecting stator-rotor zones (normal to x axis in my sketch) should be set as interfaces periodic repeats.

N.B.: if you use sliding mesh, your mesh is moving, so interfaces (periodic repeats) are a must: this ensures that when surfaces of the interfaces don't overlap, they are treated as periodic repeats.

If you use mrf or mrf+mixing plane, "interface" is a must, but you can avoid creating the "interface 2", because in this interface the 2 surfaces completely overlap and your mesh doesn't move during calculation.

If you plan to switch to sliding mesh consider to create all interfaces, also for mrf calculations, so to not have to modify your geometry when you switch to sliding mesh.

Daniele

[amin.z]

Dear daniele!
Tnx! Your suggestion is same my model!
I used mrf and the problem is converged!

But I have an important question:
If we assume that angle of right side rotor is 24 degrees ( 1/15 slice) and angle of left side rotor and stator is 60 degrees (1/6 slice), is the value of mass flow valid?
Is this value for 1/15 slice or 1/6 slice?

In my case the mass flow is 32 gr/sec and it's too low for whole model and 1/6 slice!
I think maybe solver could not recognize slices of periodic correctly!

Thank your in advance!

[ghost82]

Where did you compute the mass flow rate?
To not have doubts, compute the mass flow rate not at the interfaces, but in another plane parallel to interface.
Remember that you have to multiply the mass flow rate you read by the number of periodic repeats.

Daniele

[amin.z]

Originally Posted by ghost82

Where did you compute the mass flow rate?
To not have doubts, compute the mass flow rate not at the interfaces, but in another plane parallel to interface.
Remember that you have to multiply the mass flow rate you read by the number of periodic repeats.

Daniele

I read mass flow at main inlet at left side of model (left side of left rotor) and main outlet at right side of model ( right side of right rotor)
I think the mass flow rate for various slice must be different! Is this correct?

[ghost82]

It shouldn't...you must have conservation of mass in the domain: every section must have the same mass flow rate, otherwise the solution is not converged.
Moreover, if the fluid is incompressible (constant density in properties) also volumetric flow rate is the same for each section.
I'm not sure but you should have different mass flow rates in the 2 zones (smaller rotor on the right, other zone(s)).

Daniele

[amin.z]

Originally Posted by ghost82

It shouldn't...you must have conservation of mass in the domain: every section must have the same mass flow rate, otherwise the solution is not converged.
Moreover, if the fluid is incompressible (constant density in properties) also volumetric flow rate is the same for each section.

Daniele

Assume two periodic domains with 2 various angle of periodic! For example first domain 30 degrees and second domain 60 degrees!
Base on mass conservation low, the mass flow rate in first domain should be half of mass flow rate in second domain! ( [mdot 60]= 2 [mdot 30] )
Ok?

[ghost82]

Yes,
I added later

I'm not sure but you should have different mass flow rates in the 2 zones (smaller rotor on the right, other zone(s))

So in your case, I think that if you read the mass flow rate into the right rotor, you have to multiply this value by 15; if you read it on the left side you have to multiply by 6.
total mass flow rate must be equal for the mass conservation.

[amin.z]

This is the amazing point! The mass flow rate at left and right domain are equal! Value of both of them is 32gr/sec!

This value is logical for right rotor if multiple in 15! But it's too low for left rotor!

[ghost82]

mmm..then I don't know...The doubt now is that fluent can return the total mass flow rate yet...
You can test what fluent returns by a simple pipe simulation; you can fix the velocity inlet/pressure outlet, make a full 3d simulation and compute the total mass flow rate.
Then cut the pipe and make it periodic, fix the same v inlet/pressure outlet, recompute mass flow rate and compare the 2 results.
This is to see if fluent reports the total mass flow rate.

Or...create 2 sections into the 2 zones, calculate their area, compute and plot the mean velocity on these surfaces, and calculate the mass flow to compare.

Daniele

[amin.z]

Ok! Tnx for your help dear friend!
If you find any answer for this issue please inform me!