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

[GAMBIT] Meshing complex geometry (Hull)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2010, 16:25
Default Meshing complex geometry (Hull)
  #1
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hi,

I'm using Gambit 2.4.6 and I have to mesh the hull from a speedboat. (seen from under the hull)



This hull is situated in a "Flow Volume" (a brick with x:20m, y:10m and z:4m) The hull is substracted from this volume.

I've meshed the faces from the hull first with Quad/Tri Paved elements. Then i meshed the volume with a TGrid. This is the only way i succeeded so far. But i think there must be a better way to mesh?

Here's a picture of the mesh shade:




If there are suggestions about the meshing sheme i would be glad to hear it! Because now i'm quiete lost in the possibilities.

Vincent
vmeertens is offline   Reply With Quote

Old   March 5, 2010, 03:44
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
I would create a brick or ellipsoid around the hull for controlling the mesh growth (and also preventing for memory issue)
Then on this new volume (with the hull), create a Size Function on hull surfaces.
Mesh the volume with tetra hexcore.
I also assume you will have to merge surfaces, because of complexity of hull geometry (small edges, small angle, etc...)
For the accuracy, you also may apply a Boundary Layer (but I would try first without one)
Of course you can try meshing the whole stuff with hexa, but it will ask MUCH more time
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 5, 2010, 09:03
Default
  #3
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
The mesh i have now, counts about 1000000 cells. This is almost the limit for the pc i have. I've tried to create a little brick around the hull, but when i export the mesh, gambit makes a wall of the surfaces of that brick (default)
I don't use a boundary layer because the flow is turbulent so it's no use. (that's what my teacher said )

I didn't merge any surfaces yet, maybe i should do that first. But i wanted to keep the integrity of the hull during the meshing without changing the surfaces.

Thanks for the help!


Vincent
vmeertens is offline   Reply With Quote

Old   March 5, 2010, 09:17
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
Quote:
Originally Posted by vmeertens View Post
I don't use a boundary layer because the flow is turbulent so it's no use. (that's what my teacher said )
Check tubulence theory, especially log-law for wall treatment.
But maybe you wanted to say, that the flow is laminar
Anyway.
Regarding the mesh, you have to split the domain with your brick. If it's ok, your mesh won't contain any wall in place of outter-brick's wall.
I am also surprised that gambit didn't failed meshing your hull without any merge. Did you check the skewness of your mesh? (Examine Mesh icon)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 5, 2010, 12:58
Default
  #5
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Oké, next thing is using boundary layers... (In Fluent i use enhanced wall treatment to compensate)

I didn't know i had to split the volume, thx for that! Like i said, its the first time i have to mesh such a geometry. And we had maybe 5 hours off class for using Gambit. So i have to figure it out by my own.
I've meshed all the surfaces of the hull separatly using the appropriate interval size so i don't have to much skewness. (regarding the nodes from the neighbour surface are the same)

I'll try to mesh it better this time!
vmeertens is offline   Reply With Quote

Old   March 5, 2010, 15:42
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
up to you for using BL or not, I just reacted on the fact that your teacher said that you don't need any BL because of turbulence (and especially for extern flowfield).
If you want to use enhanced wall treatment, check the online help, there is a restriction about y+.
There is a online tool for estimating y+, (links/online-tool/y+-estimation)
On your second picture, your mesh is too coarse. Refine the mesh on the hull and apply a Size Function.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 7, 2010, 07:57
Default
  #7
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hey -mAx-,

Thx for your replies! I was wrong about the turbulence, what i ment was 'separation'...Sorry for the confusion.

I will have a look at the y+ restriction but my other case was correct.

Now I've merged the surfaces but Gambit makes it all virtual. I don't know much about virtual/real faces (I'm reading the users guide right now), but should i leave it virtual or try to make it real again?

I used a size function and meshed the volume. But i dont know if its correct? (With the virtual faces)

Thanks in advance!

Vincent
vmeertens is offline   Reply With Quote

Old   March 8, 2010, 01:54
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
you can work with virtual entities. You won't be able to use boolean operation (reserved for real entities), but splits and merge tools will work
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 8, 2010, 06:55
Default
  #9
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hey,

Oké, that's what i asumed

I've substracted the hull first and then i merged the faces. Works fine till now
vmeertens is offline   Reply With Quote

Old   March 8, 2010, 10:26
Default
  #10
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
I created a mesh, but i have 20 highly skewed elements (equisize skew > 0.97)
With a total of 1000.000 elements. Can i leave it like this or should i try to have 0 elements with to much skew?
How will that have an influence on my results in Fluent?
vmeertens is offline   Reply With Quote

Old   March 9, 2010, 04:07
Default
  #11
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
try to reduce the max skewness below 0.9
With high skewed cells, you may have convergence problems.
Try to localize the cells with high skewness. I am pretty sure they are on the hull (sharp angles).
If you can, you will have to merge some faces together
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 9, 2010, 08:48
Default
  #12
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hey MAx,

They are close to the hull on the top angle. I'll try to merge these surfaces and compare the skewness.
I've tried some different aspect ratios but i never could go less then 8 cells.
vmeertens is offline   Reply With Quote

Old   March 15, 2010, 07:08
Default
  #13
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hi,

I changed the situation like this:




I created a smaller volume (brick) and splitted the domain.
The dimensions of the brick are set to just 'surrounding' the hull (with a max gap of 0.25)
Then i substracted the hull from the little brick.
After that i merged the faces on the hull.


Now i created a SF on the hull and tried to mesh the brick.
But now i get errors when i try to mesh to brick.
Should i make the brick a little larger or what can i change?
I tried different sorts of SF but i can't mesh the little volume.

All help is welcome!

Vincent

Last edited by vmeertens; March 15, 2010 at 10:45.
vmeertens is offline   Reply With Quote

Old   March 15, 2010, 09:17
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
What kinds of error?
Do you get also error, if you try to mesh the brick without BL?
(was the hull not already substracted from the big brick?)
I give you a tip: merge surfaces, once you made boolean operation. Often merges result in cration of virtual entities. If you do the merges before boolean operation, you may not be able to substract volume for instance, since they aren't real anymore
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 15, 2010, 10:44
Default
  #15
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hi max,

I started from scratch so now the hull is substracted from the little volume.
The errors were due to connectivity of the 2 volumes. Meshing the little brick was no problem, but when i wanted to mesh the outer brick Gambit gave connectivity issues.

I managed to mesh it with a stairstep now; here's a picture of the mesh. (without SF)



Should i link the volume meshes?
I didn't use a SF so i assumed they were linked automatically.

And i merged the surface after the substraction, otherwise it doenst work. (Previous post is edited)

Thx for your replies, your help is really appreciated!
vmeertens is offline   Reply With Quote

Old   March 15, 2010, 12:18
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
yes the 2 volumes have to be connected, else gambit creates walls at the interface between the 2 volumes.
Go to Surface / Connect, and choose real-virtuals (the last one), and All entities.
It should connect your 2 volumes. (enable connectivity icon next to examine mesh: if the interface appear in pink, it is ok, else the volumes are still not connected)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 15, 2010, 14:30
Default
  #17
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hi,

I connected the faces and Gambit gave this Warning: 'The call to connect on list of faces resulted in no actual'

But i exported the mesh (before i connected the faces)and now i'm running a simulation.
When i look at the flow the inner brick isnt exported as wall so i think they were connected when i did the 'split'.
vmeertens is offline   Reply With Quote

Old   March 16, 2010, 07:55
Default
  #18
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
I'm starting to get the hang of it.
I meshed both of the volumes: The inner brick wit HexTcore and the outher brick with a TGrid. (without SF)

But i want to have accurate results so how can i improve my mesh? With a SF or should i try to use another type of mesh?

The problem is that the mesh arround the hull has to expand smoothly or i have a problem with the free surface.
(see: http://www.cfd-online.com/Forums/flu...ng-vessel.html)

Vincent
vmeertens is offline   Reply With Quote

Old   March 16, 2010, 12:40
Default
  #19
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,160
Rep Power: 32
-mAx- will become famous soon enough
are you sure that your 2 volumes are connected?
*click on the connectivity icon next to examine mesh, and check if the interfaces between your 2 volumes appear in pink
*else in fluent display the surfaces called "wall": if you see your interfaces in this group, then there the volumes aren't connected.
You can upload your dbs file on a share server, I can check your mesh
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 16, 2010, 13:43
Default
  #20
Member
 
Vincent Meertens
Join Date: Sep 2009
Location: Belgium
Posts: 41
Rep Power: 9
vmeertens is on a distinguished road
Send a message via MSN to vmeertens
Hi Max,

I assumed they were connected because in Fluent it isnt seen as a wall.
But here's a prtscrn of the connectivity:



When i splitted the volumes i had 'Bidirectional' and 'connected' clicked on.

That would be very nice of you if you want to check the mesh!


Vincent
vmeertens 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
[GAMBIT] Trouble meshing complex VOF geometry RPJones ANSYS Meshing & Geometry 2 February 14, 2011 19:54
[GAMBIT] complex geometry meshing 1682333 ANSYS Meshing & Geometry 7 August 31, 2009 12:44
Simulation of Flow through Complex 3D Geometry EmersonKB CFX 5 July 2, 2009 08:17
Gambit Meshing complex geometry Edwin FLUENT 2 July 19, 2006 15:02
Meshing a complex geometry AJG FLUENT 2 June 29, 2005 08:39


All times are GMT -4. The time now is 06:06.