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

[GAMBIT] Need advice on meshing technique to be used for this geometry

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2013, 19:42
Default Need advice on meshing technique to be used for this geometry
  #1
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi everyone,

I am new to Gambit and I wanted some advice on how to go about creating mesh for the geometry shown below.

Geometry Details: There is a rectangular furnace (5.5m X 4.5m X 12.5m) with inlets at the top and outlets along side walls at the bottom. Several cylindrical tubes are present inside the furnace with inlets at top and outlets at the bottom.

My concerns: 1) How to get relatively course mesh far from the tubes but a good enough quality mesh near the tubes (and in the narrow region between the tubes)
2) Bottom furnace geometry is slightly different from the top geometry. Should I split this part as a separate volume and mesh it separately? What scheme should I use?
3) How to get a course-enough mesh such that it can be handled by my laptop (8 GB RAM)
4) Is it recommended to first mesh all the faces before meshing the volume ?

Someone please help.

Thanks,
Ankur Kumar
UT Austin
Attached Images
File Type: jpg Model_geometry_1.jpg (62.6 KB, 32 views)
File Type: jpg Model_geometry_2.jpg (76.5 KB, 32 views)
File Type: jpg Model_geometry_3.jpg (81.0 KB, 24 views)
File Type: jpg Model_geometry_4.jpg (95.7 KB, 26 views)
ankur_kr is offline   Reply With Quote

Old   November 20, 2013, 00:49
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
do you want full hexa, hybrid or tetra-mesh?
If your BC are symmetric, you can also handle one half of your model, your laptop will enjoy this
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 20, 2013, 22:50
Default follow-up
  #3
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi Maxime,

Thanks for replying. Though I don't have any particular demand for a type of mesh (Hexa or tetra), from my previous experience (with simulation over smaller geometry) it seems Hexa mesh gave better chances of convergence.

Regarding the BC, the current geometry is actually the symmetric portion of the much bigger model. All the outer walls here (other than inlets and outlets) are symmetric.

Observations about mesh size limit:

I was trying to check the size-limit as to when would Gambit report memory deficit error. During one such trial, Gambit reported "Unable to allocate 51739272 bytes of memory". But this is just 50MB. Why does Gambit report memory error for such small size ? During another trial I was able to get a mesh with 2.5 million cells.
Can this problem be solved in general by dividing my geometry in smaller parts and meshing them separately ?

Meshing strategy/attempts:

I could mesh all the 32 tubes (with inside boundary layer) with total of 1.5 million cells. For meshing the region outside tubes, I have split the lower part (the 2 leg kind of structure) and will mesh them separately. Since, I will have combustion/flame (fast kinetic reaction) near the inlets (outside the tubes), I need relatively finer mesh there. So I am thinking of dividing the upper part also in 2 regions with gradual transition from fine to coarse mesh.

A big concern that I have is that very fine mesh on the tube's surfaces will cause unnecessarily very fine mesh outside the tubes. Could putting boundary layer outside the tube solve this problem ?

My first aim is to get a course enough mesh that will converge. Then I can use Fluent adaptive refine facility (no memory problem as it will run on a cluster) to get better result.

[Previously I tried to learn Icem-cfd for meshing but due to the limited graphic capability of the x-windows connection (screen would blank out when zoomed etc.), it became extremely difficult to learn and use strategies like blocking. So, I shifted to Gambit.]

Sorry for the long reply. Please let me know what you think of my observations. Right now I mostly simply accept the default suggestions of Gambit.

Thanks,
Ankur
ankur_kr is offline   Reply With Quote

Old   November 21, 2013, 02:49
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
I am not surprised from memory error if you want to mesh your volume on the fly.
For sure you need to split your domain, and you will have to use size fonction for having fine mesh in desired area and coarser where you don't have special interest.

If you check my picture you can generate 3 splits. Both at top and bottom will isolate domain where inlet/outlets are (there will be finer meshed)
The last split (expansion from small to big block) will make cooper mesh easier.
Thus you can generate an hybrid mesh. I would mesh all your tubes with cooper (caps surfaces with pave)
Then both coarser volumes also with cooper (source faces with pave).
The 2 last volumes (top and bottom), with tetra/hexcore and with size function on surfaces of interest.
Untitled.png
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 21, 2013, 03:06
Default
  #5
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 637
Rep Power: 13
ghost82 will become famous soon enough
Quote:
Originally Posted by ankur_kr View Post
Hi Maxime,

Gambit reported "Unable to allocate 51739272 bytes of memory". But this is just 50MB. Why does Gambit report memory error for such small size ? During another trial I was able to get a mesh with 2.5 million cells.
Hi,
50 mb is the size in eccess that gambit cannot allocate in your memory.
As suggested by Max split your volume and mesh the smaller ones; continue splitting untill you haven't memory error.
ghost82 is offline   Reply With Quote

Old   March 14, 2014, 19:45
Default How to decide if this mesh is good or not ?
  #6
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi Maxime and Daniele,

Using your above advices I had generated a mesh (link below) for my model. I could run steady-state simulations successfully (in the sense that it converged) in Fluent. Though it seems to give reasonable solution, it's not exactly what I was expecting. Also, my transient runs always give divergence error.

How can I decide whether there is a problem with my mesh (details below) ? My model BCs aren't that tricky, so I don't expect any problem with model specification.

Mesh Details:
6.7 million elements (takes 4 days for S.S simulation on 4 parallel CPUs)
Max Equisize Skew : 0.82 (only 5 elements above 0.8)
Max. Aspect ratio : 17.68
Minimum Orthogonal quality: 0.27

https://drive.google.com/file/d/0B6r...it?usp=sharing

Thanks,
Ankur Kumar
UT Austin
ankur_kr is offline   Reply With Quote

Old   March 19, 2014, 01:44
Default
  #7
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
what about your bc?
For instance how did you treat volume 17 in respect with volume 44?
If you don't specify any bc, gambit merges both volumes
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 19, 2014, 14:56
Default follow-up
  #8
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi Maxime,

Thanks a lot for replying. Please find below the link for the .dbs file with proper boundary conditions specified.

https://drive.google.com/file/d/0B6r...it?usp=sharing

I did give proper attention to the boundary conditions and zone definitions.

Thanks,
Ankur
ankur_kr is offline   Reply With Quote

Old   March 20, 2014, 01:39
Default
  #9
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
ok, 2 points:

* I wouldn't set all the symmetries in one set, but one symmetry for coplanar surfaces (eg: faces 446 403 456 & 2 are one symmetry bc)

* the tubes surfaces as wall (for instance rf_32) separates the furnace from tube refv_32 (volume 33), normally you should disconnect furnace from volume.33: wall shloudn't have 2 adjacent zones. But I believe Fluent is smart enough and create wall shadow for fixing this problem.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 20, 2014, 17:48
Default Follow-up
  #10
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi Maxime,

Regrading first point: I will try this out and see if it makes any difference. But just curious to know why you suggested this, as in doesn't symmetry BC simply gets stored as zero fluxes for every individual surface elements on these surfaces ? Moreover, if I plan to use Wall BC on these surfaces currently specified as symmetry surfaces, would you still recommend this coplanar segregation ?

Regrading second point: I had painstakingly deleted the extra surfaces that got created when I subtracted the tube from furnace as Fluent had that "Wall Shadow" feature automatically coupling the shadow surfaces for heat transfer which is what I needed.

So, Max the problems that I am facing isn't outright a case of 'Junk in Junk out' right ? That is my mesh is not outright of bad quality ?

Thanks,
Ankur
ankur_kr is offline   Reply With Quote

Old   March 21, 2014, 02:12
Default
  #11
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
your mesh is ok

But you mentionned that you wanted heat transfer. Then I think it might be your problem.
Disable the thermal BC on your walls, and check if you still have divergence as prior.
If it is ok, then it is definitvely your problem, and I would suggest you to check the help especially Thermal Boundary Conditions at Walls
https://www.sharcnet.ca/Software/Flu...ug/node253.htm
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 21, 2014, 18:52
Default follow-up
  #12
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 3
ankur_kr is on a distinguished road
Hi Maxime,

Sorry for asking a lot of question but what did you mean by "disable the thermal BC on walls" ? Do you mean to impose zero flux BC (which is what I kind of have right now as symmetry mean zero flux).

Thanks,
Ankur
ankur_kr is offline   Reply With Quote

Old   March 24, 2014, 01:31
Default
  #13
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
I meant, don't calculate anything on wall. (stationnary wall)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- 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
[ICEM] Geometry Tolerance and meshing Mitpostdoc ANSYS Meshing & Geometry 4 January 1, 2012 12:51
[ICEM] Meshing of 3d flywing geometry sfs ANSYS Meshing & Geometry 24 November 17, 2011 04:49
[ICEM] Meshing on a Complicated Geometry tav98f ANSYS Meshing & Geometry 2 August 17, 2011 11:15
Problematic geometry in Ansys Meshing ATOTA ANSYS Meshing & Geometry 1 October 9, 2010 11:51
Complex Geometry Meshing andreasp Main CFD Forum 2 September 26, 2010 15:16


All times are GMT -4. The time now is 00:32.