Different volume mesh zones
 

Hi guys,

I am working on a CFD problem and I need to create a small volume which has sliding properties inside a larger static mesh. I am unable to find any option to create separately. I tried to do it with slice tool but I doubt if I would get the new zone. I am attaching a picture to give an idea. Thank you very much :D

If you do not have to solve anything inside the rotating zone then you do not have to mesh it. You can simply have only outer region and declare the inner wall as moving/rotating wall.

@ vasava, my problem is modelling a stirred tank. so i need to give sliding mesh to stirrer and to some volume(which contains fluid) around it, and the outer static mesh also contains fluid. So I need to divide the mesh of fluid region into two parts: static(normal) and sliding one. The momentum from stirrer must be transferred to the fluid.

Aha.. you are trying for MFR case. I thought you are doing the dynamic mesh study. Anyways, what are you using to mesh generation?

Sliding mesh
 

@vasava: Im trying to use sliding mesh technique instead of MRF. I am using Fluent on Workbench. I have used the defaults mesh settings. But I want to have sliding mesh in the volume around the stirrer, so I can get more real results. So, can you tell me how to give the required part of the total mesh as sliding??

You can prescribe the rotation speed in the place where you select the material for each of the zone.

Sorry I am logged in to linux and cant point out the exact name of the window.

Sliding mesh
 

I have tried that by giving mesh rotation velocity in cell zone option. But the effect of stirring is not observed. Should I give any linking between the mesh of stirrer and that of fluid?

And my main question is how to demarcate a specific area in a volume and give it different mesh property than the whole?

Thank you :)

Dear abhishek kalu
you haven't answered which software you used for mesh generation.
It seems to me you have problems in pre-processing, I think you'd better write or move this post to ansys meshing and geometry.
If you want to use sliding meshes you must define two different and disconnected volumes, one for the outer static zone, and the other for the rotating zone.
In gambit for example you can create the big volume and then subtract (with unchecked "connected" option) the smaller one.
Then, in pre-processor sw, you have to assign interfaces as boundary condition to shared faces between static and rotating zones.

Then, also in fluent you must create interfaces, so you can use moving mesh.

Daniele

yes, ghost82 has explained everything you need to know about meshing such a case.

Sliding mesh
 

@ghost82 Thnk you very much. I believe your reply solves my question and your profile picture is probably which I am doing as the project :D I am using Fluent 14.5 on workbench, therefore I am using the Ansys meshing software. Can you give any such method in fluent as you have mentioned in gambit?

Coming to the mesh interfaces, what type of interface needs to be given so that there would be fluid and momentum exchange between two zones?

BTW initially, inorder to test if the stirrer effect is see,. I have given moving mesh to stirrer and gave the rotational velocity. But I did not find its effect on the fluid when I checked the contours and vectors in the solution module. Should I give any interface between the stirrer and fluid?

Again thank you very much.

Hi!
I'm sorry but I never opened the ansys meshing/workbench softwares in my life :)
But you can ask in the ansys meshing and geometry how to create different zones and how to assign interfaces as boundary conditions; or you can search for tutorials.

More into details (I will refer to gambit software, but same actions should be repeated into ansys meshing)

Pre-processing:
1- create the geometry, let's say you have the tank, the shaft, the impeller and the baffles
2- in your geometry you have to create 2 disconnected volumes: the outer "static" volume (let's call it "stator") and the central rotor zone, which includes the impeller and part of the shaft (let's call it "rotor")
3- mesh the geometry
4- assign boundary conditions: wall for the tank (let's call it "tank_wall"), wall for the baffles (let's call it "baffles"), wall for impeller (let's call it "impeller"), wall for the shaft which is included into the "rotor" zone (let's call it "shaft_rotor") and wall for the other part of the shaft (let's call it "shaft_stator"), which is into the "stator" zone;
create interfaces: I would create 6 interfaces: look at the picture; "top_interface_stator", "top_interface_rotor", "bottom_interface_stator", "bottom_interface_rotor", "side_interface_stator", "side_interface_rotor".
Assign other boundary conditions for top and vertical faces (PERIODIC! not simmetry!)

Fluent (I'm writing only the part on setting sliding mesh and velocity):
1- load the geometry into fluent and set models and fluid properties
2- in cell zone conditions panel select "rotor" zone and check motion type for moving mesh, and set the rotational velocity (take care of axis direction and origin vectors)
3- select "stator" zone and take care of axis direction and origin vectors

So now you have the rotor fluid zone that rotates.

4- in boundary conditions panel set the velocity of "tank_wall" and "baffles" to "absolute" and to zero, so they will have an absolute rotational velocity of 0 rpm; then set the velocity of "impeller" and "shaft_rotor" to "relative and to zero, so they will have the same rotational velocity as the adjacent fluid zone (i.e they will rotate at the same velocity of the "rotor" zone); finally set the velocity of "shaft_stator" to absolute and to xxx rpm (where xxx is the same as the "rotor" velocity), so also the part of the shaft in the "stator" zone will rotate
5- create interfaces in the mesh interfaces panel: you need to create 3 interfaces: call the first for example interface1 and select "top_interface_stator" and "top_interface_rotor", then call the second one interface2 and select "bottom_interface_stator" and "bottom_interface_rotor", then call the third one interface3 and select "side_interface_stator" and "side_interface_rotor".

Attached image: you will have 2x3 overllapping faces in your geometry (because "rotor" and "stator" are disconnected volumes!): blue text means that in boundary conditions you have to select the faces which belong to the "rotor" zone, red text means that you have to select the faces which belong to the "stator" zone.

Hope that is more clear now.

PS: if you search in google you can find a fluent tutorial on stirring tank: it's solved by mrf, so I think there aren't interfaces but the part on volume zones is the same as yours; also search for some tutorials on sliding meshes, you will understand better!

Daniele

In Ansys meshing if you have imported a model with two domains then the interfaces are created automatically. On the left panel look for 'connections'.

Now the automatically created 'connections' can be strange sometimes. So you have to check manually. Also ensure that you have declared them domain type solid or fluid properly in ansys meshing. Otherwise when you might face additional issues in Fluent.

meshing error
 

@ghost82 thanks for you comprehensive reply:) But im getting the following error while meshing:

"The mesh file exporter failed during translation. Please send your data to your support provider."

I guess it must be due to any interference, but I have given all the coponents according to perfect dimensions.
I am attaching the image of mesh generated. The error is seen while updating the mesh in order to work in fluent.
@vasava: any solution to this?? :D

You forgot the picture you said you will attach.

@vasava: sorry i have attached now :D

interface problem
 

@ghost82 I was trying another method i.e have created the geometry using surface(unlike the previous case wher I have used complete solid). I was wondering how to give the stator interfaces(top, side and bottom). The rotor interfaces can be given as I have created the inner rotor zone(using surface). I am attaching the image. Thank you very much for your support.:)

http://s17.postimg.org/fwzzetgqn/upload.jpg

Sorry, but I don't understand your question..if you have interfaces you have 2 disconnected volumes, so you have overlapping surfaces at interfaces: three are for the rotor zone, the other three are for the stator zone.

Daniele

Meshing
 

@ghost82:
In the first case, I have modeled the geometry as follows:
1)Create the stator part with recess.
2)Create rotor part. (Both of them solids)

So now I have the interface of rotor and stator separately.

In second case where I created using surfaces,
1)create a stator surface
2)create rotor surface
now I can only give interfaces pertaining to rotor zone..I dont have any inner surface of stator to give as interface.

http://s30.postimg.org/62sya6rox/upload_22.jpg

I see that you have three domains: the rotor (solid), fluid surrounding the rotor (fluid) and the tank (fluid). In my opinion you do not need that solid rotor.

And once again, I suggest you look for 'connections' on the left panel. In Ansys meshing the interfaces are referred 'connections' and are created automatically. You can also right click on 'connections' and chose the 'create connections' for manual creation.

One more question, which program have you used to create your CAD model??