CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] U-bend Mesh in ANSYS

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree11Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 23, 2012, 14:41
Post U-bend Mesh in ANSYS
  #1
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
I'm trying to mesh a U-bend in ANSYS for later FLUENT simulations.

I can't think of a proper mesh to adopt in this case (180 degrees pipe).

I would believe a C-grid is the most reasonable. But I lake the expertise to do such complex grid using ANSYS MESH.

Anyone have good tutorial or idea of how to mesh this complex geometry, would be much appreciated?
John222 is offline   Reply With Quote

Old   June 24, 2012, 13:40
Default
  #2
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by John222 View Post
I'm trying to mesh a U-bend in ANSYS for later FLUENT simulations.

I can't think of a proper mesh to adopt in this case (180 degrees pipe).

I would believe a C-grid is the most reasonable. But I lake the expertise to do such complex grid using ANSYS MESH.

Anyone have good tutorial or idea of how to mesh this complex geometry, would be much appreciated?
Will I get an answer. Or just wasting my time here?
John222 is offline   Reply With Quote

Old   June 25, 2012, 07:38
Default
  #3
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 142
Rep Power: 10
jsm is on a distinguished road
Hi,
If I understood your question clearly, here is my comments.

For simple geometries, you can use sweep or multizone mesh method to get full hexa mesh. For complex geometries, multizone method with "ICEM CFD interactive option enabled" is the best way. You can move the block edges to get good quality meshes.

If you post image of geometry, you will get better comments and solution quickly.

with regards,
Subramanian
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Old   June 25, 2012, 10:31
Default
  #4
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,216
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
would you mind sharing your geometry ?
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 25, 2012, 11:21
Default
  #5
New Member
 
Abhipray Jain
Join Date: Mar 2012
Posts: 8
Rep Power: 4
abhiprayj is on a distinguished road
http://www.youtube.com/watch?v=tYrbScUH9RE

Part 1 2 and 3

Hope it helps and gives some idea.
abhiprayj is offline   Reply With Quote

Old   June 25, 2012, 17:46
Post
  #6
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
would you mind sharing your geometry ?

Attached Images
File Type: jpg Geometry.jpg (81.7 KB, 262 views)
John222 is offline   Reply With Quote

Old   June 25, 2012, 17:47
Default
  #7
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
I want to mesh the geometry using ANSYS WORKBENCH MESH not GAMBIT or anything else.
John222 is offline   Reply With Quote

Old   June 25, 2012, 19:20
Default
  #8
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,216
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
i'm not an ansys meshing expert (i really need to start playing with it a little bit). but i can mesh it with icem cfd. I'm sure that somebody with an expertise in ansys meshing will help you with this geometry.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 25, 2012, 19:41
Default
  #9
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
i'm not an ansys meshing expert (i really need to start playing with it a little bit). but i can mesh it with icem cfd. I'm sure that somebody with an expertise in ansys meshing will help you with this geometry.
If I do the mesh in ICEM CFD. Can I then save the case so I can run ANSYS FLUENT using the mesh done in ICEM CFD, or it has to be done in ANSYS WORKBENCH MESH?
John222 is offline   Reply With Quote

Old   June 25, 2012, 20:16
Default
  #10
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,216
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
of course you can use with fluent. you can export you mesh and specify as output parameters FLUENT. it doesn't have to be workbench
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 25, 2012, 20:56
Default
  #11
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Lausanne - Switzerland
Posts: 59
Rep Power: 5
Gweher is on a distinguished road
Can you please add your .agdb, I'll have a look with Ansys Meshing
diamondx likes this.
Gweher is offline   Reply With Quote

Old   June 25, 2012, 22:35
Default
  #12
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by Gweher View Post
Can you please add your .agdb, I'll have a look with Ansys Meshing

Please check mail. I have sent you the geometry please note it's a 2D model and mesh must be done in 2D and in ANSYS MESH.
John222 is offline   Reply With Quote

Old   June 26, 2012, 00:12
Default
  #13
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Lausanne - Switzerland
Posts: 59
Rep Power: 5
Gweher is on a distinguished road
I had a quick look at your geometry. Well basically if you want a C-grid then the quickest way is to split your geometry. I sliced the U bend into 5 sub-surfaces within DesignModeler, then select all the 5 sub-surfaces and right click >form new part.

After updating inside Ansys Meshing you can assign different element controls in order to get the mesh you want. As I didn't know exactly what you are trying to model I just generate a mesh and added a boundary layer just to show you how to play around with Ansys Meshing. There is not only one unique method to generate a C-grid, and there are lot of different ways to create your boundary layer like adding inflation layers, I did it this way but use the method that better suits you.

As I didn't know if I could upload the .agdb file I attach images of the splitting and the mesh and send you a private message with the .zip file.
Attached Images
File Type: jpg DMsplitting.jpg (16.9 KB, 66 views)
File Type: jpg AMcgrid.jpg (22.7 KB, 66 views)
File Type: jpg AMcgridzoom.jpg (62.3 KB, 92 views)
Far and John222 like this.
Gweher is offline   Reply With Quote

Old   June 26, 2012, 11:40
Default
  #14
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by Gweher View Post
I had a quick look at your geometry. Well basically if you want a C-grid then the quickest way is to split your geometry. I sliced the U bend into 5 sub-surfaces within DesignModeler, then select all the 5 sub-surfaces and right click >form new part.

After updating inside Ansys Meshing you can assign different element controls in order to get the mesh you want. As I didn't know exactly what you are trying to model I just generate a mesh and added a boundary layer just to show you how to play around with Ansys Meshing. There is not only one unique method to generate a C-grid, and there are lot of different ways to create your boundary layer like adding inflation layers, I did it this way but use the method that better suits you.

As I didn't know if I could upload the .agdb file I attach images of the splitting and the mesh and send you a private message with the .zip file.
Hi

I have ANSYS WB V13 not V14. What are the exact steps to do this kind of mesh?
John222 is offline   Reply With Quote

Old   June 26, 2012, 19:00
Default
  #15
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Lausanne - Switzerland
Posts: 59
Rep Power: 5
Gweher is on a distinguished road
Well you can either use slice material by plane and create several planes to cut your surface into sub-surfaces or create several sketches and use them with extrude by selecting the option "slice" within the extrude menu.

I'll explain the first method as you have a simple geometry (but both are basically the same in a way).

1) Starting with your geometry, >tool>freeze (or under your SurfaceSk1 choose "add frozen" instead of "add material"). This will permit to use the slice option (see first attachment - "TreeOutlinePlaneSlice").

2) Create the 2 planes, >create>New Plane, in the options select YZPlane, under transform 1 choose "Rotate about Global Z", and enter 45, >generate. Repeat the procedure 2) for the second plane changing 45 to 135.

3) Now that you have defined the 2 new plane hit >create>slice, under Slice Type select "Slice by Plane" (default) and select the YZ plane, click >generate. This will slice your U bend into 3 parts (see second attachment - "FirstSliceOperation").

4) Repeat point 3) changing the plane YZ to one of the 2 plane you created in point 2) AND change "All bodies" under Slice Targets to "Selected Bodies" and select only the small U bend sub-surface created in point 3) (in order to keep the other sub-surfaces as rectangles).

5) Repeat point 4) by selecting the last plane and only the sub-Ubend surface that needs to be sliced (see third attachment -"SecondAndThirdSliceOperations").

-> You will end with the 5 sub-surfaces you are looking for

6) Under Parts you will now have 5 parts, select them all, right click and >Form New Part, this is important for the next meshing step if you want to have a single mesh and no interfaces between the 5 sub-domains.

-> Now you can easily play with the meshing tool of Ansys Meshing.
Attached Images
File Type: png TreeOutlinePlaneSlice.PNG (8.0 KB, 41 views)
File Type: jpg FirstSliceOperation.jpg (19.3 KB, 51 views)
File Type: jpg SecondAndThirdSliceOperations.jpg (20.0 KB, 47 views)
Far, John222, diamondx and 1 others like this.
Gweher is offline   Reply With Quote

Old   June 26, 2012, 20:10
Default
  #16
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by Gweher View Post
Well you can either use slice material by plane and create several planes to cut your surface into sub-surfaces or create several sketches and use them with extrude by selecting the option "slice" within the extrude menu.

I'll explain the first method as you have a simple geometry (but both are basically the same in a way).

1) Starting with your geometry, >tool>freeze (or under your SurfaceSk1 choose "add frozen" instead of "add material"). This will permit to use the slice option (see first attachment - "TreeOutlinePlaneSlice").

2) Create the 2 planes, >create>New Plane, in the options select YZPlane, under transform 1 choose "Rotate about Global Z", and enter 45, >generate. Repeat the procedure 2) for the second plane changing 45 to 135.

3) Now that you have defined the 2 new plane hit >create>slice, under Slice Type select "Slice by Plane" (default) and select the YZ plane, click >generate. This will slice your U bend into 3 parts (see second attachment - "FirstSliceOperation").

4) Repeat point 3) changing the plane YZ to one of the 2 plane you created in point 2) AND change "All bodies" under Slice Targets to "Selected Bodies" and select only the small U bend sub-surface created in point 3) (in order to keep the other sub-surfaces as rectangles).

5) Repeat point 4) by selecting the last plane and only the sub-Ubend surface that needs to be sliced (see third attachment -"SecondAndThirdSliceOperations").

-> You will end with the 5 sub-surfaces you are looking for

6) Under Parts you will now have 5 parts, select them all, right click and >Form New Part, this is important for the next meshing step if you want to have a single mesh and no interfaces between the 5 sub-domains.

-> Now you can easily play with the meshing tool of Ansys Meshing.

I can't thank you enough. This is very helpful.

I'm trying to mesh the model and I tried doing a structured mesh the same one you made. But I keep getting non-uniformed mesh for some reason (see attached).



Would you be able to print screen your mesh tree outline so I can have an idea of what you have done to the mesh. Thanks!!
Attached Images
File Type: jpg Mesh.jpg (98.0 KB, 262 views)
John222 is offline   Reply With Quote

Old   June 26, 2012, 20:30
Default
  #17
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Lausanne - Switzerland
Posts: 59
Rep Power: 5
Gweher is on a distinguished road
You just need to add a mapped face (I think it uses pave by default if you don't specify anything), so right click on mesh, >insert>mapped face mesh, and then select all the faces. This should fix your problem.

I've also added a print screen of the mesh tree outline (as I told before I didn't know what you are trying to model so I just added several sizing in order to have more control in each sub-surface domain).
Attached Images
File Type: png MeshUbendSteps.PNG (8.6 KB, 57 views)
Far and John222 like this.
Gweher is offline   Reply With Quote

Old   June 26, 2012, 20:35
Default
  #18
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by Gweher View Post
You just need to add a mapped face (I think it uses pave by default if you don't specify anything), so right click on mesh, >insert>mapped face mesh, and then select all the faces. This should fix your problem.

I've also added a print screen of the mesh tree outline (as I told before I didn't know what you are trying to model so I just added several sizing in order to have more control in each sub-surface domain).

Thank you! I believe I know the basics now and will continue refining the mesh to meet my needs for later simulation.

Please check your mail box

Last edited by John222; June 26, 2012 at 21:37.
John222 is offline   Reply With Quote

Old   June 28, 2012, 12:00
Default
  #19
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,874
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Good information. Learned new things about AM.
Far is offline   Reply With Quote

Old   August 14, 2012, 12:39
Default
  #20
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
how can I generate a contour plots that looks like this;

John222 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 2 November 25, 2012 08:54
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09
Problem importing GAMBIT mesh to Ansys geometry David G. CFX 0 June 19, 2005 06:01


All times are GMT -4. The time now is 00:19.