# [ICEM] how can mesh this geometry ?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

September 17, 2012, 11:34
how can mesh this geometry ?
#1
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Hi all , sorry for this question , i am new in ICEM ...
how can mesh this geometry ?

triangular channel in rectangulat solid , water inside the triangular channel ...

Attached Images
 303887_269711906481402_1292251685_n.jpg (62.9 KB, 135 views)

 September 17, 2012, 11:43 #2 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Are both domains fluid? Ie the entire box minus the triangular prism is one domain and the triangular prism is a second domain? The boxminus the triangular prism is the more interesting of the domains. There are two different topologies that spring to mind. The choice really comes down to your actual model; what surfaces are inlets/outlets/walls etc.? These will dictate the flow directions, then you can choose a mesh topology that aligns itself best with this. The first potential topology is a simple 3D block split three times along the length, and the assosiate vertices to the corners of the triangle The other potential topology is a C grid arond the triangular prism propogated out to the far walls. This will give you better alignment if the triangle is a source or a sink. Stu __________________ http://bc247.wordpress.com

 September 17, 2012, 12:11 #3 Member   ahmad Join Date: Feb 2012 Posts: 97 Rep Power: 6 yes the entire box minus the triangular prism is one domain( solid ) and the triangular prism is a second domain( fluid)

 September 17, 2012, 12:42 #4 Member   ahmad Join Date: Feb 2012 Posts: 97 Rep Power: 6 thanks stuart23 for reply , can more explain ?

 September 17, 2012, 15:03 #5 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,314 Blog Entries: 6 Rep Power: 43 simple possible solution, four blocks

September 17, 2012, 21:04
#6
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by Far simple possible solution, four blocks
thanks Far.... I did this blocks but the mesh quality appeared poor , especially at the corner of triangular prism ...
Attached Files
 rti2.zip (1.9 KB, 4 views)

September 17, 2012, 22:47
#7
Super Moderator

Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,366
Blog Entries: 23
Rep Power: 21
that's why you need to add a Y-grid. it is the best suitable for those kinf of corners.
Take a look at the project i attached
Attached Files
 rti2.zip (13.8 KB, 10 views)
__________________
Regards,
New to ICEM CFD, try this document --> https://goo.gl/NEbygB
Ali

September 17, 2012, 23:00
#8
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by diamondx that's why you need to add a Y-grid. it is the best suitable for those kinf of corners. Take a look at the project i attached

thanks ali .... can explain to me how you take the block for tringular prism ?? i mean how to devide the geometry to 5 blocks ( one of them to triangular prism ) ......

thank you so much ..

 September 17, 2012, 23:07 #9 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Tokyo, Japan Posts: 1,366 Blog Entries: 23 Rep Power: 21 take a look at this video: http://www.youtube.com/watch?v=InyeCmEuUVM y-grid is created, also some vertices are merged. everything you need is in this video. time to go to sleep... see you tomorrow __________________ Regards, New to ICEM CFD, try this document --> https://goo.gl/NEbygB Ali

September 17, 2012, 23:09
#10
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by diamondx take a look at this video: http://www.youtube.com/watch?v=InyeCmEuUVM y-grid is created, also some vertices are merged. everything you need is in this video. time to go to sleep... see you tomorrow

thank you so much my bro ..... good night ...

 September 18, 2012, 06:13 #11 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,314 Blog Entries: 6 Rep Power: 43 slide the vertices of the middle downward to improve the quality. Or 1. Insert Y Block 2. Put O-grid

September 18, 2012, 06:19
#12
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by Far slide the vertices of the middle downward to improve the quality. Or 1. Insert Y Block 2. Put O-grid

thanks Far ..... i get confuse when i try to make Y-block

 September 18, 2012, 11:39 #13 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,314 Blog Entries: 6 Rep Power: 43

September 18, 2012, 11:41
#14
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by Far

thank you so much ...

 September 18, 2012, 12:03 #15 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,314 Blog Entries: 6 Rep Power: 43 Few snapshots for your case (you have fluid and solid regions ?)

September 18, 2012, 23:18
#16
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by Far Few snapshots for your case (you have fluid and solid regions ?)
yes i have fluid and solid regions ....

thanks bro

 September 18, 2012, 23:24 #17 Member   ahmad Join Date: Feb 2012 Posts: 97 Rep Power: 6 when i finish making mesh by ICEM with fluid and solid i read it by fluent , but in fluent only one zone appear ( solid ) why ???

 September 19, 2012, 01:06 #18 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,314 Blog Entries: 6 Rep Power: 43 Because you don't have the fluid region!!! Right click on the parts then choose the last option (blocks). Rename to fluid and select the fluid blocks (blocks in Y-grid). Recreate premesh and convert to mesh. After that export the mesh and import into Fluent. You are done.

September 19, 2012, 01:17
#19
Member

Join Date: Feb 2012
Posts: 97
Rep Power: 6
Quote:
 Originally Posted by Far Because you don't have the fluid region!!! Right click on the parts then choose the last option (blocks). Rename to fluid and select the fluid blocks (blocks in Y-grid). Recreate premesh and convert to mesh. After that export the mesh and import into Fluent. You are done.
really i thank you so much ..... i get it

September 19, 2012, 02:20
#20
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Quote:
 Originally Posted by malay I did this blocks but the mesh quality appeared poor , especially at the corner of triangular prism ...
When you have the triangular prisms, dont compare their quality to hexa. With prism, quality of 0.01 is also good enough

Here I am quoting one of the Simon's post regarding quality. Low quality Tet prism mesh post # 15

Quote:
 If you haven't seen the inverted issue, then no worries... It happens only in 13.0 for redistribute prism, but is already fixed... In the mean time, the work around is to redistribute using the "Move => Redistribute Prisms" command. There isn't any more to tell. Min tetra quality should probably be above 0.2, but if you have some below, it is probably fine, particularly in a non critical area. CFX is pretty robust, you could try as low as 0.05. The Prism metric is really harsh in ICEM CFD. If you can get above 0.01, it will probably run fine in CFX... You could even go lower. (Maybe others can comment on their worst mesh that converged)... Hexa, you are usually looking at min angle and aspect ratio... We shoot for an angle over 18, but will take anything over 9.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Anorky ANSYS Meshing & Geometry 4 November 12, 2014 01:27 Ganesh FLUENT 13 January 22, 2014 05:11 froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52 eysteinn OpenFOAM Native Meshers: snappyHexMesh and Others 0 May 5, 2011 10:15 sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11

All times are GMT -4. The time now is 03:17.

 Contact Us - CFD Online - Top