CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] 2D Geom en street canyon model (http://www.cfd-online.com/Forums/ansys-meshing/85109-2d-geom-en-street-canyon-model.html)

fek66 February 17, 2011 11:49

2D Geom en street canyon model
 
1 Attachment(s)
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.

PSYMN February 23, 2011 23:51

Geometry Steps.
 
5 Attachment(s)
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.
Attachment 6615

Then I created lines between those points.
Attachment 6616

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).
Attachment 6617

Then I broke the model into various parts (INLET is a curve because it is the boundary to the AIR, which is a surface...)
Attachment 6618

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.
Attachment 6619

PSYMN February 24, 2011 00:11

Blocking Steps...
 
5 Attachment(s)
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...
Attachment 6620

Then I made 1 horizontal split based on the point at the top of the buildings.
Attachment 6621

Then I deleted the two blocks within the buildings.
Attachment 6622

Then I set some basic edge parameters
Attachment 6623

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...
Attachment 6624

PSYMN February 24, 2011 00:20

Ogrid
 
3 Attachment(s)
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...
Attachment 6625

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...
Attachment 6626


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.
Attachment 6627

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...

fek66 February 28, 2011 07:39

2D Geom mesh model
 
2 Attachment(s)
Hi Simon ;
thanks for reply ;
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

alastormoody11 March 1, 2011 02:31

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.

PSYMN March 1, 2011 09:07

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.

fek66 March 2, 2011 10:47

I want to use CFX PRE to import a *.msh file is it possible what is the way

PSYMN March 3, 2011 19:01

1 Attachment(s)
@ 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,

phuchuynh June 23, 2015 05:22

Quote:

Originally Posted by PSYMN (Post 297857)
@ 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


All times are GMT -4. The time now is 08:49.