# [GAMBIT] Mesh inner wall of a duct which rotates

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 19, 2013, 20:11 Mesh inner wall of a duct which rotates #1 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 Hi, I'm meshing this geometry: a duct which has inserted a twisted tape. I've designed the volumes, meshed the fluid and the twisted tape with cooper scheme (hex/wedge cells). The problem is the duct mesh: because of the rotation of the tape (and fluid and inner face of the duct), at the moment of mesh with cooper scheme, as the nodes of the destiny source face have rotated, it happens that outer cells don't rotate, they are meshed along the axis, but inner cells have rotated, in order to link the pairs of corresponding nodes due to twist angle; and this fact produces a growing number of cells with skewness>0.97, and negative volumes. I've meshed using TGrid, but I'd prefer cooper scheme. Do you have any idea how to do it? I'll attach a photo with my problem as faster I can. Thanks!

 April 22, 2013, 01:12 #2 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 Then I wait your picture for better understanding __________________ In memory of my friend Hervé: CFD engineer & freerider

June 15, 2013, 05:37
#3
Senior Member

Agustín Villa
Join Date: Apr 2013
Location: Alcorcón
Posts: 314
Rep Power: 15
At first place, I want to apologize for being late.

As you can see, I have two fluid zones with a solid one which separates them. All these are inside the tube, and above it you can see "my problem".

If I had this element I would mesh the fluid, solid and tube using a cooper scheme. The problems is that when I have the upper element, it relates some nodes between the outer and inner diameter.

I thought meshing the tube with tetrahedral, bus I usually get some problems, error codes... I tought this new idea:

- Create a mesh that includes the fluid, the tape and the tube, that I can mesh with cooper scheme easily, and apply the "Interface" B.C. to the outer wall.
- Create a mesh that includes the upper element, where I could use cooper too, and use "Interface" in the inferior face.
- In Fluent, link these interfaces.
Like that, I could mesh easily both elementes. It is possible my idea?

Thanks for all and sorry again!
Attached Images
 tramo.png (29.6 KB, 45 views)

 June 17, 2013, 01:20 #4 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 why do you want to mesh the solid volume? Can you post same picture with shaded mode on __________________ In memory of my friend Hervé: CFD engineer & freerider

June 17, 2013, 03:33
#5
Senior Member

Agustín Villa
Join Date: Apr 2013
Location: Alcorcón
Posts: 314
Rep Power: 15
Here I attach the shaded figure.

I want to mesh the solid volume because I have to study the heat transfer between the upper surface, where a heat flux is applied, and the fluid volume inside the duct.
Attached Images
 tramo2.png (36.9 KB, 33 views)

 June 17, 2013, 04:22 #6 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 ok bith green volumes should be automatically as cooper meshed. white volume should be decomposed (split): *do a split with cylinder (lower radius) --> it will isolate the volume which separates both green volumes *do a split with cylinder (higher radius) --> it will isolate the extrusion at the top of your domain. Now you have 3 separated white volumes. Mesh first the ring, then the others __________________ In memory of my friend Hervé: CFD engineer & freerider

 June 17, 2013, 04:38 #7 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 But after should I connect all of them? The fluid zones and the solid inner one rotate, and if I apply cooper scheme to them, their mesh rotate too. If I mesh the tube and the upper element using cooper scheme, I think it could be problems because these volumes don't rotate. All that if I connect the volumes. Anyway, I think I could do as you say if I don't connect them when I split all the volumes, and use an interface boundary condition at the walls that communicate the fluid zones and the inner solid one with the higher cylinder. Did you want to say that? Do you think that if I mesh the inner elements, the higher cylinder on a .msh file, and the upper element in other one, and I conect them in Fluent using "Grid Interfaces", I could get the same results?

 June 17, 2013, 04:47 #8 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 ah I forgot this point. Ok Then once you splitted the solid volume with cylinder (R lower), then you have to disconnect volumes. For that : copy both fluid volumes and solid one (which rotates) and delete all 3 orginal volumes. Take advantage of this moment to define your interfaces (interface stator side, and interfaces rotor side. But I assume on the rotor side you have to isolate interface from solid). Once it is done select all surfaces of volumes you have copied and connect them (I suspect Gambit to disconnect surfaces when you copy more than one volume). Then movy back the volumes at their original location. Should be ok __________________ In memory of my friend Hervé: CFD engineer & freerider

 June 17, 2013, 05:08 #9 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 At first place it is what I do: - Create the zones in the inner side (radius -> r) - Create volumes of radius R, the cylinder and the top element - Split these lasts zones with the previous, taking off the originals, and connecting all the volumes. My problem happens when I try to mesh the duct with radius R, because its internal face rotates with the fluid internal zones, and its external faces are fixed, because one of its faces is connectd with the top element, so if it rotates, nodes in external edges connect with oters that are rotating, giving problems of skew size, even negative volumes. So, you propose to me to: - Create volumes as I said - Split and NO connect the volumes, and create the interface BC on the faces at radius=r - Mesh the elements: the internal with cooper scheme, and they'll rotate; and the external by the same way, but they won't rotate. The problem is that when I connect the volumes, the meshes in faces at radius=r must be the same, so it becomes into a twisted face mesh in radius=r (where the duct connects with the fluid and solid inside of it) , and a no-twist face mesh at the volume at radius=R, and if I try to mesh it with cooper I have the problem explained above. For this reason I liked your idea (or at least the idea I've understood).

 June 17, 2013, 06:20 #10 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 disconnecting your domain with radius r (inner side), will allow you to use sliding mesh (that's why I talked about interfaces) Then no need for the rotor mesh to match mesh from stator. The solver will interpolate data across interfaces __________________ In memory of my friend Hervé: CFD engineer & freerider

 June 17, 2013, 08:04 #11 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 Thanks a lot for your idea! At first place, I'll try my idea (mesh tube and inner volumes and in other file the top element) because I did some journal before about that, but you idea I think is better because, if I've understood , I could mesh the inner tube in a .msh file, the tube in other one, and the top element in a third file. Do you want to say that? I've defined in other cases the inner side with a journal, and only y should create other one to the other elements, tube and top element, in a more easy way than create all of them in the same mesh; I drew the first one group, and I have to create more of them, with the rotating parts inside, and it is very dificult to "journalize" it (but I did it!). Anyway, I'll try your idea in this way: -Mesh inner side in a .msh - Mesh outer duct in a .msh file - Mesh top element in a .msh file (I prefer mesh it apart because I could prefer to use another form in this place) - Use in Fluent "Grid Interfaces", and join this three elements And Fluent will interpolate between all these meshes. Thanks again!

 June 17, 2013, 08:11 #12 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 you should have only 2 meshes: rotor and stator The top volume is attached and connected to the stator. If you want to work with 3 volumes, then you need to define another interfaces between stator and top volume __________________ In memory of my friend Hervé: CFD engineer & freerider

 June 17, 2013, 08:35 #13 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 I'll use three meshes, because I could change the shape of the last one. And at "Grid interfaces" menu, I need to select the interfaces of the inner side, and inthe other side, the interface of the stator, right?

 June 17, 2013, 08:38 #14 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,297 Rep Power: 41 yes it is right, only if you have 2 .msh files. If you have 3, you need other interfaces. Else Fluent will generate a wall between your stator and your top volume __________________ In memory of my friend Hervé: CFD engineer & freerider

 June 17, 2013, 08:54 #15 Senior Member   Agustín Villa Join Date: Apr 2013 Location: Alcorcón Posts: 314 Rep Power: 15 Ok, thanks for your help!

 Tags duct flow, gambit, twisted tape

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Ganesh FLUENT 15 November 18, 2020 06:09 hinca CFX 15 January 26, 2014 17:11 romekr ANSYS Meshing & Geometry 1 November 26, 2011 12:11 [snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 21:11 SSL FLUENT 2 January 26, 2008 11:55

All times are GMT -4. The time now is 16:50.

 Contact Us - CFD Online - Privacy Statement - Top