# [ICEM] 2D Geom en street canyon model

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

February 17, 2011, 11:49
2D Geom en street canyon model
#1
Member

anonymous
Join Date: Jan 2011
Posts: 42
Rep Power: 7
As I explain to Simon and to shear my question with all CFD online users . I want to make a 2D Geom for a street canyon model ( see attached file) with a canyon aspect ratio equal to ( H/W =0.12m/0.12m). I am a begginer user of ICEM and I need steps to make geometry and meshing.
many thanks.
Attached Images
 2Dgeom2.JPG (70.1 KB, 45 views)

 February 23, 2011, 23:51 Geometry Steps. #2 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 OK, here it comes. I think I am getting to busy lately to help with this sort of thing. The work is quick, but explaining it takes time. I guess I should have run the replay scripting, but oh well, I guess I will for the blocking. This first post is about creating the geometry. ICEM CFD is primarily a mesher, but it has geometry tools that are useful. I started with Points at XYZ locations... It is a 2D model, so Z=0. fekih_01_Points.jpg Then I created lines between those points. fekih_02_Curves.jpg Then I created a Surface from those lines (the command is surface from 2 to 4 curves, but if they are coplanar, there is no limit). fekih_03_Surfaces.jpg Then I broke the model into various parts (INLET is a curve because it is the boundary to the AIR, which is a surface...) fekih_04_Parts.jpg Then I set some basic sizes based on the image you sent me of the problem. We will set sizes more carefully in Hexa later, so this is just a rough pass. fekih_05_PartMeshSetup.jpg

 February 24, 2011, 00:11 Blocking Steps... #3 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 So then you initialize 2D blocking... (sorry, no image, but it is the first option in the blocking tab). This gives you one big rectangle. I associated the vertex corners of this rectangle with the point corners of the model. Then I made 4 vertical splits based on the points at the corners of the buildings... In the script these splits will follow those points... fekih_06_SplitVertical.jpg Then I made 1 horizontal split based on the point at the top of the buildings. fekih_06_SplitHorizontal.jpg Then I deleted the two blocks within the buildings. fekih_07_DeleteBlock.jpg Then I set some basic edge parameters fekih_08_EdgeParams.jpg And here is my first very coarse premesh. If this is the topology you want, you would just need to go back and spend some time with the edge params getting things right... fekih_09_Coarse_Premesh.jpg

 February 24, 2011, 00:20 Ogrid #4 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 But you probably want some good boundary layer resolution... Time for the Ogrid... For Ogrid, you select all the blocks and then control it with the faces/edges... fekih_11_OGrid_Selection.jpg In this first case, I have also selected the edges on the inlet, far field (top) and outlet. This cause the Ogrid to pass out those faces and leaves a boundary along my ground and buildings... fekih_11_OGrid_Rough.jpg But you can do many different o grid topologies... In this next one, I additionally selected the edges on the ground ahead of and behind the two buildings... This caused the Ogrid to pass thru the ground and gave a different topology. fekih_11_OGrid-alternate_Rough.jpg You could not include the block between the buildings in the first Ogrid so it would pass across the top of the gap and then put a second Ogrid in the block between the buildings to capture recirculation. You could split off a block behind the second building and Ogrid that to capture a wake, etc. Then in the end, you would adjust final vertex locations, edge parameters, etc. Try some tutorials for the regular details...

February 28, 2011, 07:39
2D Geom mesh model
#5
Member

anonymous
Join Date: Jan 2011
Posts: 42
Rep Power: 7
Hi Simon ;
I am still with blocking Method you describe to me , but in stead I use Curve Mesh parameters--> selecting the building curves to make high resolution around building (See photo) . After Edit Mesh---> Check mesh, I still have problems as you see in image. What's wrong with me !
Thanks
Attached Images
 alltri_curve_mesh.jpg (98.9 KB, 37 views) errors.jpg (95.8 KB, 28 views)

 March 1, 2011, 02:31 #6 Senior Member   Join Date: Jun 2009 Posts: 100 Rep Power: 9 Hey, That is not a problem you need to be concerned with in 2D case. That diagnostic is for 3D cases. The single edges are bound to occur in a 2D mesh for all elements at the boundary of a CV.

 March 1, 2011, 09:07 #7 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 allastormoody11 is totally right... That is why that column is listed as possible problems. Just check it and make sure the single edges are around your perimeter and you are all right.

 March 2, 2011, 10:47 #8 Member   anonymous Join Date: Jan 2011 Posts: 42 Rep Power: 7 I want to use CFX PRE to import a *.msh file is it possible what is the way

March 3, 2011, 19:01
#9
Retired from CFD Online

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
@ fek66

Yes,

After creating an new case, import mesh. When you go to browse for your files, you will see an import file filter and can change it to "ICEM CFD" to get the options for *.cfd5 or *.msh

Best regards,
Attached Images
 OutputToCFX_SelectFile.jpg (70.2 KB, 16 views)

June 23, 2015, 05:22
#10
New Member

Jindo
Join Date: Mar 2011
Location: Germany
Posts: 25
Rep Power: 7
Quote:
 Originally Posted by PSYMN @ fek66 Yes, After creating an new case, import mesh. When you go to browse for your files, you will see an import file filter and can change it to "ICEM CFD" to get the options for *.cfd5 or *.msh Best regards,
Hi all,

I have some troubles about boundaries condition in street canyon. Especially, it is an infow condition, i.e. equation of inflow condition?

Thanks and best regards

Phuc

 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 chiven OpenFOAM Bugs 7 August 23, 2011 02:52 qascapri FLUENT 0 January 24, 2011 11:48 sherifkadry CFX 2 September 7, 2009 20:51 rystokes CFX 3 August 9, 2009 19:13 Margherita Cadorin CFX 0 October 29, 2008 06:24

All times are GMT -4. The time now is 18:45.