CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Unwanted Walls inside domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 8, 2011, 09:13
Default Unwanted Walls inside domain
  #1
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Dear All, this is my first post here cause I started my master thesys about a comparison between sails and wings on a cruise boat, What I am tryng to do right now is to resolve the flux around the sail: I created the geometry with CATIA ( that I know at least a little) and meshed with CATIA mesher, I imported the mesh on gambit as NASTRAN mesh (So I should not have geometry information inside the file)to set up BC, but my problem is that I have surfaces generated with CATIA, they are visibles in the picture attached, that fluent converts as walls.
I tried setting them as "Internal " but I have errors with this kind of setting... I tried to delete them, I tried to heal the volumes but the volumes I guess are fixed with the mesh, any suggestion?
Thank you in advance
G.



bishop_house is offline   Reply With Quote

Old   February 8, 2011, 12:24
Default
  #2
Senior Member
 
Join Date: Nov 2009
Posts: 411
Rep Power: 10
DoHander is on a distinguished road
Load the Catia files in Gambit and define there the boundary conditions.
DoHander is offline   Reply With Quote

Old   February 8, 2011, 12:30
Default
  #3
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
I did it: I don't know how to set those internal faces
bishop_house is offline   Reply With Quote

Old   February 9, 2011, 01:58
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
could be a problem of non-connected surfaces.
You can fix it by connecting all the surfaces.
But I don't understand the purpose of importing your mesh in Gambit. (is it just a conversion into *.msh format?)
I would import your geometry in Gambit, and mesh it with Gambit. Then you won't have any surprise
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 9, 2011, 07:37
Default
  #5
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Yes mAx, I think it is something due to the fact that there are 3 different meshes, I see that setting those surfaces as interfaces it works, I am using gambit just to set the BC conditions, nothing more because i don't like the gambit mesher ( my limit I am not able to mesh a cube -.- )
If you can suggest me a good tutorial about gambit mesher I will offer you a beer
Thanks
bishop_house is offline   Reply With Quote

Old   February 9, 2011, 08:06
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
the default tutorials in gambit are quite good.
So in your case, you set the walls as interfaces? and then in fluent, you define the couple of interface (there should be superposed surfaces), right?
If you still have problem and you want to mesh it with Gambit, I can guide you.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 9, 2011, 10:59
Default
  #7
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Yes, I did as you explained, but I realized that it doesn't work because if I have complex intersections between faces, I can't use one part of a surface as interface with the surface of one region, and the other part of the surface as interface of another region.
So I modify the CATIA product to have simplied intersection between region,having each couple of surfaces as regions interface but gambit doesn't like infact when I try to import the mesh it finds tons of null lenght segments.

So I decided to mesh it directly in gambit but I can't mesh a cube with the sail-shape cavity inside because the cube is 40 meters long and the thickness of the sail is 1 mm, any idea about this?
bishop_house is offline   Reply With Quote

Old   February 9, 2011, 11:02
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
provide me your geometry file.
Step file, if you have.
I will take a look tomorrow
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 9, 2011, 11:28
Default
  #9
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
I sent you an email with the geometry.
Once I will solve the problem I will prepare a "tutorial" to help new user like I am, to thank the comunity
bishop_house is offline   Reply With Quote

Old   February 10, 2011, 02:44
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
ok I saw your geometry.
First question, how many cells did you generate with your mesh (CATIA)?
With this geometry your mesh will be huge, since you consider each sail has a thickness (for instance edge.60).
Thickness is 1 in comparison to height of sail which is about 40000.
In this state, it means that the first cell adjacent to the top (or bottom) of the sail (direct glued to the thickness) will have an edge of 1.
Your mesh will be quick huge, and you will have hardware problem for sure.
Maybe you should consider having sails without thickness (considered as baffle).
If you do, then you need to rebuild your entire volume.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 10, 2011, 03:50
Default
  #11
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
ok I saw your geometry.
First question, how many cells did you generate with your mesh (CATIA)?
Around 4 milions
Quote:
Originally Posted by -mAx- View Post
With this geometry your mesh will be huge, since you consider each sail has a thickness (for instance edge.60).
Thickness is 1 in comparison to height of sail which is about 40000.
In this state, it means that the first cell adjacent to the top (or bottom) of the sail (direct glued to the thickness) will have an edge of 1.
Your mesh will be quick huge, and you will have hardware problem for sure.
It runs smooth on a multicore machine
Quote:
Originally Posted by -mAx- View Post
Maybe you should consider having sails without thickness (considered as baffle).
I am pretty sure that the baffle model is the one used by sail producers, But I don't know how to implement it, just have a surface inside the domain and set it as wall?
Quote:
Originally Posted by -mAx- View Post
If you do, then you need to rebuild your entire volume.
Rebuild the volume with something that works will be a pleasure
bishop_house is offline   Reply With Quote

Old   February 10, 2011, 04:22
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
4 millions seem to be "small"
Can you import your mesh in Gambit and check the skewness.
Go to examine mesh (icon bottom right)
Select range and enable all kinds of elements
Click Update, you will see all your mesh colored by skewness (0..1)
set now the lower value with 0.95 and the max with 1.
I would be surprised that you dont have skewed elements touching all the "thickness".

if you want to switch with baffle model, let me know (yes this is just a surface in your model, considered as wall)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 10, 2011, 04:51
Default
  #13
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Yes! I have 8 active elements in that range, the worst one at the very top of the main sail, with a quality value of 0.99 ( but 8 bad elements are enough to mess up the model? )
About the baffle model, I am very interested to learn, but I don't want to waste your time, just a list of operation and tricks will be ok
Something like control volume 1 Km, split it in 3 regions, set 2 of them as laminar, set all the outflow surfaces as Pressure-outlet,
Thanks in advance
bishop_house is offline   Reply With Quote

Old   February 10, 2011, 05:54
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
with 0.99 the check mesh could failed, and you may not be able to start calculation.
But only 8 cells in that range, it's surprising.
Regarding the baffle, geometry is quite simple to generate.
Just delete the volume with sails (disable option lower entities, else it will delete also surfaces)
Then delete all the surfaces you don't need (thickness surfaces etc...) Finally your sails consist in 2 surfaces.
Create the surrounding volume, by stitching surfaces from the brick.
And split the volume with the 2 surfaces (sails)
Now the surfaces belong to the volume.
At this time I would only concentrate on this volume (with sails)
Then reagarding meshing, you have 2 options:
*Quick with tetra-hexcore (with size fonctions on sails for refining your mesh around them)
*Dedicate more time to a nice hexa mesh (you will need to decompose your volume)
Sans titre.png Sans titre1.jpg Sans titre2.jpg
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 10, 2011, 14:45
Default
  #15
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
I followed your explanation and I obtained the volume with the surfaces inside, I also meshed everything using gambit, and from your notes I increased the number of elements reaching 7 millions, the msh is something like 540 Mb, once loaded in fluent I have 1.8 GB of RAM occuped that reach 3.3 Gb when I try to initialize, with 3.3 giga of ram busy and a 32 bits version of fluent it crashes.
This memory usage sounds reasonable? if yes I have to enlarge the mesh, if not I have something wrong in the model
bishop_house is offline   Reply With Quote

Old   February 11, 2011, 02:04
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
with enlarge you meant coarse, isn't it?
Yes it is possible that you cannot initialize your model because you are out of memory.
What kind of error do you receive from Fluent?

What kind of meshing schema did you used?
If you used tetra, I would suggest you to use tetra-hexcore, it will reduce dramatically the size of your mesh.

Else you can handle your problem either by computing your model into parallel architecture (cluster where your model will be decomposed and distributed) or opening your case on a 64bit desktop with sometihing like 8GB Ram.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 11, 2011, 07:01
Default
  #17
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
yes, I meant coarse
I am using tetra-TGrid, I tried with Hex-core but the file seems bigger, but here I can in parallel, I have just to do a double step,
1) open the .msh with a normal version of fluent, the parallel version crashes: I guess that is due to something with the interfaces not jet set, and save as .cas with the interfaces properly set up
2) open the .cas with the parallel version and init and run
Yesterday evening I run the model with about 4M elements, it ddin't blow up, so this is a good starting point, but it didn't converged. I post three pictures, one is the residual plot, the second and third are the behavour of velocity and the turbolence intesity on a section of the control volume, looking this picture is clear that my flux is not "deployed" , one kilometer is not enough? And more important, I set the outer zone as laminar, so why I have the turbolence intesity not equal to zero far from my sails?

Last edited by bishop_house; February 11, 2011 at 07:36.
bishop_house is offline   Reply With Quote

Old   February 11, 2011, 07:57
Default
  #18
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
*tetra-hexcore gives less cells than tetra since gambit fills the domain with hexa
*you still have interfaces? for what?
*the pictures sound weird. Are you able to see the sails? especially overpressure on them. How is the velocity distribution around them?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 11, 2011, 09:36
Default
  #19
New Member
 
Giampiero
Join Date: Nov 2010
Posts: 15
Rep Power: 6
bishop_house is on a distinguished road
Here a detail of the flux around the sails, I don't like it.
I have interfaces because I have 2 zones, one, the inner, is the turbolent while the outer is the laminar, probably I didn't understand how to use them, I read that consider the entire volume as turbolent increases the error on the drag effect.

bishop_house is offline   Reply With Quote

Old   February 11, 2011, 09:50
Default
  #20
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,965
Rep Power: 30
-mAx- will become famous soon enough
ok the velocity at sails seem to be ok (eg: no velocity)
So your sails should be treated as wall. That's good.
What are your BC, and how did you initialized your domain?
I would first try to compute your domain without separating turbulent-laminar zone (ie: full turbulent or full laminar).
Just to catch something realistic (that's not the case here)

Then regarding interfaces, you don't need interfaces for defining 2 fluid zones.
If your volumes are splitted correctly (understand faces connected), then it's ok.
Just pick a volume a define it separately.
I don't know how you built the outer domains, but basically, once the volume with sails is meshed, then split the outer domain with the one with sails.
The surfaces will be automatically connected.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Reply

Tags
catia, fluent bc, nastran

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
Interface between fluid domain and porous domain windhair CFX 5 September 5, 2013 20:45
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
Howto Sphere solid as a subdomain inside a domain? jakjak CFX 0 October 24, 2007 23:31
how set a source inside a flow domain Jason FLUENT 1 August 8, 2003 16:23
meshing F1 front wing Steve FLUENT 0 April 17, 2003 12:37


All times are GMT -4. The time now is 10:41.