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

[GAMBIT] is it possible to create this type of grid?

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

Like Tree2Likes
  • 1 Post By Far
  • 1 Post By BigBen

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2012, 12:55
Default is it possible to create this type of grid?
  #1
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Hi all,
is it possible in Gambit to create this type of grid (attached picture)?If yes, how?

Thank you,

Daniele
Attached Images
File Type: png multilayer.png (50.1 KB, 36 views)
ghost82 is offline   Reply With Quote

Old   January 4, 2012, 13:23
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
yes it can be done in gambit. but you need to make them in steps and then import into fluent and then create the interfaces. However this can be easily done in icem cfd by refining the domains by the factor of 2 and you have two nodes corresponding to one node to other side.
ghost82 likes this.
Far is offline   Reply With Quote

Old   January 4, 2012, 19:12
Default
  #3
New Member
 
Join Date: Dec 2011
Posts: 10
Rep Power: 5
BigBen is on a distinguished road
I confirm, it can be easliy done in Gambit but as said, you need to disconnect faces where the mesh is not conformed in Gambit and create interface in Fluent.

I may have another possibility. I would rather do everythng in Fluent using the Adapt/Region/refine in 3 steps.
Firts of all, create your mesh in gambit with the coarser mesh and import in Fluent.
In Fluent
1-adapt/region select by coordinates or by mouse button all the region which is refined (all the upper rectangular even the more refined). Press "refine" it will multiply by two the mesh in this region.
2-3 do it again for the small square on the upper left and upper right.

Hope it will help
ghost82 likes this.
BigBen is offline   Reply With Quote

Old   January 4, 2012, 22:28
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Yeah it is much better and easier method and does not require interfaces
Far is offline   Reply With Quote

Old   January 5, 2012, 11:07
Default
  #5
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Quote:
Originally Posted by BigBen View Post
I confirm, it can be easliy done in Gambit but as said, you need to disconnect faces where the mesh is not conformed in Gambit and create interface in Fluent.

I may have another possibility. I would rather do everythng in Fluent using the Adapt/Region/refine in 3 steps.
Firts of all, create your mesh in gambit with the coarser mesh and import in Fluent.
In Fluent
1-adapt/region select by coordinates or by mouse button all the region which is refined (all the upper rectangular even the more refined). Press "refine" it will multiply by two the mesh in this region.
2-3 do it again for the small square on the upper left and upper right.

Hope it will help
Thank you Bigben,
I knew that this could be done in fluent; however I was curious to know if that grid could be done directly in gambit.
Thank you all for replies.

Daniele
ghost82 is offline   Reply With Quote

Old   February 3, 2012, 05:55
Default
  #6
New Member
 
Davide
Join Date: Jan 2012
Posts: 2
Rep Power: 0
themeska is on a distinguished road
Hi everybody!

I think this is the thread i've been looking for...as you all said a local refinement is possible and even easier in Fluent, by using the Adapt panel...anyway, this wouldn't be the easiest way for my geometry, since it consists of buildings with different heights...
Everytime i try to vertically sweep the outer region (which is to time as coarse as the inner one), Gambit says it cannot sweep it...i think it's because of the different number of intervals between the inner and outer region...and maybe Gambit is not able to connect them, am i saying something wrong?
can anyone explain to me how to do that?

What i'd like to do is to impose in Fluent different BCs for the inlet flow (i mean, different roughness heights), using different values for the inner and outer region...
themeska is offline   Reply With Quote

Old   February 3, 2012, 11:03
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Everytime i try to vertically sweep the outer region (which is to time as coarse as the inner one), Gambit says it cannot sweep it...i think it's because of the different number of intervals between the inner and outer region...and maybe Gambit is not able to connect them, am i saying something wrong?
In mapping you cannot just change the nodes on one edge, you should change the no of nodes on parallel edges, but if you to make the mesh shown in 1st post, then you need to create different regions and save in different files and keep the region which you want to mesh and delete all other. Then export the mesh from all these files and read them in Fluent with append command. Got it?
Far is offline   Reply With Quote

Old   February 3, 2012, 11:10
Default
  #8
New Member
 
Davide
Join Date: Jan 2012
Posts: 2
Rep Power: 0
themeska is on a distinguished road
So, basically, what you're saying is that i should create as many meshes as the regions with different cells' sizes and then "put" them together in Fluent?
Thanks a lot for your fast reply, helped a lot!
Regards
themeska is offline   Reply With Quote

Old   February 3, 2012, 11:22
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
yes and at the common boundaries specify interface as boundary condition.

You muest read first mesh and for other meshes you must use the append command.
Far 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
compilation problem with "fvPatch::lookupPatchField" Ya_Squall2010 OpenFOAM Programming & Development 7 October 27, 2014 11:24
cgnsToFoam problems with "QUAD_4" cells lentschi OpenFOAM Meshing & Mesh Conversion 1 March 9, 2011 05:49
turbulent jet simulation antonio_ing OpenFOAM Running, Solving & CFD 5 September 16, 2010 02:31
Flow Around a Cylinder ronaldo OpenFOAM 5 September 18, 2009 08:13
Grid Independent Solution Chuck Leakeas Main CFD Forum 2 May 26, 2000 11:18


All times are GMT -4. The time now is 04:09.