[asmita]

Hello,
I tried doing as you said. N it did created volumes.but my total mesh is in 100 KB. which should not be the case.I want mesh in 100 MB's and more. Also once when I tried to import that mesh in Fluent I couldn't see the rectangle.Only turbine was imported.This means my geometry wasn't good.

[-mAx-]

That means your volume has not been imported.
Your turbine should appear as surface and not as a volume.
Did you receive any warning while exporting mesh from Gambit (like warn unmeshed entity are not exported)

[asmita]

No. It did not gave me any warning. N when u say that turbine should be surface and not volume, what exactly do u mean ? Because when I sweep the face of turbine it creates volume.And i do want volume for both turbine and rectangle.
Do Split -Face option help? My friend suggested to split-face turbine from rectangle, then mesh and sweep it. But that is not helping me either.

[-mAx-]

You have 2 volumes: your outer domain and the impeller.
If you subtract the outer domain with the impeller, then you get the outer domain with impeller as hollow.
That means your impeller is only represented by its outside surfaces.
And the volume represents the fluid domain around the impeller.

[asmita]

Hii, thanks for the advice.. I got my geometry done. But now i have to restrict the motion of turbine in all directions i.e. translational and rotational except for rotation in x-direction. How do i do that..? Do i use the 'specify continuum types' in zones option in Gambit ? Do i define turbine as fluid or solid type for that?
Please help me

[-mAx-]

do you want moving mesh, Single or Multiple Reference..?
check here:
http://aerojet.engr.ucdavis.edu/flue...ug/node412.htm
http://aerojet.engr.ucdavis.edu/flue...ug/node436.htm

[asmita]

Moving mesh...

[-mAx-]

then you have to disconnect rotor zone to stator zone.
Doing this, you will able to set interfaces between both zones (one interface for rotor, and one for stator).
Then fluent will be able to move rotor zone, and data will be interpolated on interfaces (which you have to define "again" in fluent /define/grid-interfaces)

[asmita]

How to disconnect rotor from the rectangle ?

[-mAx-]

do a split to distinguish rotor from stator.
If the split is well done, then both domains are connected, which is not wanted.
So copy rotor zone with any translations-vector.
Delete original rotor zone.
Now you can see your stator with an hollow.
Define the interface face (stator side)
Define the interface face (copy of rotor side)
Move back the rotor zone.
That's it (Now both interfaces are stacked)

[asmita]

Hello,
What do you exactly mean by copy rotor zone with any translations-vector ? I did not understand that where should I copy and what rotor zone are you talking about.. What should I do before deleting the rotor?

[-mAx-]

if you copy your volume, it will be localised at it original place, and you won't see it
If you give a translation's vector, it will be copied and translated, so that you will be able to delete the original volume
http://aerojet.engr.ucdavis.edu/gamb..._volm_movecopy

[asmita]

Hii, You said to define the interface on rotor and stator.. Is that in Gambit or in Fluent ? and how do you define it? Also you said that - move back the rotor zone.. I did not get it. I will translate the rotor volume- delete original. Then I did not get the interface defining part and again moving back the rotor zone part...

[-mAx-]

You have to do that in gambit.
I give you an example:
-you have a square 100x100
-in the middle you create a rotor zone with radius 10 (just create a circle R10)
Sans titre.jpg
So you split your square (surface) with the circle. It gives you 2 connected zones: the rotor surface (disk R10) and the rest (stator).
Sans titre1.png
If you mesh both surfaces, they are connected and you don't have any chance to move the rotor zone.
For sliding mesh, you need to disconnect both zones and the data interpolation will be done through interfaces. In this case the interfaces will be circles (you need an interface for the stator, and one for the rotor).
Now both surfaces are still connected. Copy and translate the disk anywhere and delete the original. Doing that you disconnect both zones and you can assign interfaces easily.
Sans titre2.png Sans titre3.png
Just move back the copy of rotor.
Sans titre4.png
That's over: you have stator and rotor disconnected with interfaces

Then in fluent grid/interfaces...

[asmita]

Hii, I tried as you said.. N that was really well explained. Thank you for that. I have a doubt... When i copied the rotor and deleted the original, it did not got deleted in real coz I had used split option between outer box and rotor. So even when i deleted it,I could see the rotor as a whole volume with the box. Is that a problem ?

And after the interfaces are separated, how do i restrict the motion of rotor in all directions except in only one direction..? is that done in gambit itself or I have to use fluent?

[-mAx-]

Originally Posted by asmita

When i copied the rotor and deleted the original, it did not got deleted in real coz I had used split option between outer box and rotor. So even when i deleted it,I could see the rotor as a whole volume with the box. Is that a problem ?

pictures please

Originally Posted by asmita

And after the interfaces are separated, how do i restrict the motion of rotor in all directions except in only one direction..? is that done in gambit itself or I have to use fluent?

once stator and rotor zones are defined (with interfaces), then the rest of setup occures in fluent (define/dynamic mesh)

[yoooodarulez]

Good evening to everybody.

Im new to the cfd world so my questions may seem a bit newbish but i really cant help it...so here it goes!First of all id like to say that i am studying the airflow over a wing,namely a s809 3d airfoil,and my goal is to compare the results of this analysis with the experimental ones for various angles of attack as well as various turbulence models (SA,k-e realizable,k-w sst),as far as cl,cd,cm are concerned.Im modelling the wing in gambit and processing with fluent 6.3.My problem came up in 2nd order k-e realizable where i either get the error "turbulent viscosity ratio limited" or i do not get convergence.That is for most of the AoA anyway since ive come across some convergence in some others.My first question then is about the mesh itself.The worst element is in a critical region of the flow and i cant seem to get rid of it.Secondly id like some insight on how to mesh the flowfield next to the wing,meaning from where the wing ends till the boundary.I would be glad if some1 gave me some piece of information!