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

Prism mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 20, 2011, 06:43
Default Prism mesh
  #1
Member
 
Mohankumar.G
Join Date: Sep 2010
Location: Pune,India
Posts: 44
Rep Power: 7
Mohankumarg12 is on a distinguished road
Hi
I am doing a defrosting study of windshield, in the process I encountered a problem in creating a prism mesh.

In my geometry I have three material points
1.Fluid zone(inside the cabin)
2.Solid zone(Glass of the windshield)
3.Ice zone above the solid zone.

I created a TET mesh inside my fluid zone and prism on the wall(facing the fluid zone) of the windshield, here my wind shield is not connected edge to edge to the cabin(figure-2)

The problem is I have to create a prism mesh on the windshield and for the ice layer by extruding the surface mesh which is in the bottom of the windshield.

I tried different methods
1.I created a surface mesh on all the walls and I deleted the mesh on the unwanted walls on the windshield and I created volume mesh for the cabin, while creating the prism mesh on the walls the standalone surface mesh was deleted automatically.
So I made a advanced setting in the global parameter for prism, that not to delete the standalone mesh, In this settings my standalone mesh was not deleted but I am getting a worst pyramids on the edges.

How to rectify this problem.


Thanks in advance,
Mohan.G
Attached Images
File Type: jpg Picture1.jpg (26.9 KB, 51 views)
File Type: jpg Picture2.jpg (18.5 KB, 43 views)
Mohankumarg12 is offline   Reply With Quote

Old   July 22, 2011, 20:27
Default Steps...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I assume you are not meshing anything out side of what you described... You have a fluid zone in the cabin, air will be circulating and transferring heat to the glass which will then pass thru and transfer heat to the ice... The glass and the ice are just solids and are fully connected to the inside of the cabin...

I would start by just meshing the cabin... You don't even need the geometry for the glass or the ice... Just the cabin as a single volume. Mesh it. Set prism settings for the inside of the cabin since your heat transfer will depend on your boundary layer capture...

When you are all done with that fluid region...

Take the shells of the window and extrude them... You probably want 3 to 5 cells thick for the glass. Extrude them in such a way that the number of layers and growth ratio add up to the thickness you wanted for the glass... During the extrude operation, you can pick the name of the volume (pick GLASS) and the name of the top (Pick GLASS_OUTER or something like that...

Then go back and repeat... Extrude "GLASS_OUTER in such a way that it extrudes by the thickness of ICE that you want and the volume is called "ICE", etc.

In the solver, give GLASS and ICE the correct solid properties and you are all set.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   July 22, 2011, 23:46
Default prism mesh required area
  #3
Member
 
Mohankumar.G
Join Date: Sep 2010
Location: Pune,India
Posts: 44
Rep Power: 7
Mohankumarg12 is on a distinguished road
Hi Simon,
Thanks for your reply. I understand what you are saying, but my problem is I am unable to create prism mesh all over the windshield area.

Plz see the attached picture for the problem that I am facing

Many thanks,
Mohan.G
Attached Images
File Type: jpg Picture3.jpg (98.9 KB, 32 views)
Mohankumarg12 is offline   Reply With Quote

Old   July 23, 2011, 13:33
Default No problem...
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
OK, no problem. If the glass is not fully connected to the volume, I guess you do need that geometry (just the one surface(s))...

I am assuming that the windshield surface(s) must be split into two main regions. The part shared by the fluid volume and the perimeter outside of that (lets call it OUTER_W).

Start as before and mesh the volume with normal tetra/prism methods. This will also mesh the inner region of the windshield surface, but not the outer edge shown in your last image.

Then go into global parameters for surface meshing => Patch Dependent. Turn on the option about "respect line elements". This will make sure that any patch dependent shell meshing you do on the OUTER_W will attach to the previous mesh along the shared boundary, but you still need to set the sizes for the outside of the OUTER_W. To that with the Mesh => Curve parameters. Set them up to be the size you want for a smooth or zero transition. Then go to Mesh => Compute Mesh => Surface meshing. make sure it is Patch Dependent and selected surfaces... Pick the "OUTER_W" surface(s). Compute.

This should generate a nice patch dependent mesh around the perimeter that uses the outer perimeter curve sizing and the line elements from the tetra prism mesh for the inner perimeter sizing... In other words, a conformal mesh across the windshield...

Then proceed with the extrusion instructions I gave before using both regions...

Note: the previous instructions assumed a uniform window and ice thickness... With a little more effort, you can also handle varying thickness.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   July 25, 2011, 02:50
Default Meshing completed
  #5
Member
 
Mohankumar.G
Join Date: Sep 2010
Location: Pune,India
Posts: 44
Rep Power: 7
Mohankumarg12 is on a distinguished road
Hi Simon,
I got the mesh as you suggested. Plz see the attached picture.
I really struggled to make it, but as per your idea I made it within a minute.

Many thanks,
Mohan.G
Attached Images
File Type: jpg Picture1.jpg (97.6 KB, 27 views)
Mohankumarg12 is offline   Reply With Quote

Old   July 25, 2011, 09:44
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I am not sure this is right... I expected to see the perimeter of the volume mesh imprinted on the windshield... I don't see it... Perhaps it is just the image, but I suspect things were not done quite right yet... Is the volume mesh properly attached to this windshield?
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   July 27, 2011, 07:24
Default Mesh error rectified
  #7
Member
 
Mohankumar.G
Join Date: Sep 2010
Location: Pune,India
Posts: 44
Rep Power: 7
Mohankumarg12 is on a distinguished road
yes Simon, You are correct, my volume elements are not proper and I re meshed the whole geometry. Now I got the correct mesh and volume mesh both. Plz see the attached picture.

Many thanks,
Mohan.G
Attached Images
File Type: jpg Picture1.jpg (97.1 KB, 32 views)
Mohankumarg12 is offline   Reply With Quote

Old   July 27, 2011, 16:10
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Perfect... Good work.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN 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
Getting prism to inflate into mixed tet-hex meshes Joe CFX 16 October 10, 2011 07:06
[ICEM] Creation of hexa dominant mesh and prism layer gnuboard ANSYS Meshing & Geometry 5 May 18, 2010 10:27
Prism with anisotropic trimmed mesh fastwave STAR-CCM+ 1 May 9, 2010 10:29
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 03:09.