# structured domains

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

July 6, 2013, 08:24
structured domains
#1
New Member

Elham
Join Date: Jun 2013
Location: Germany
Posts: 8
Rep Power: 4
Hello Guys,
How can i create a structured domain for my simple 2D Geometry? How should i define the Domain and mesh it? Left edge is Velocity inlet and right edge is pressure outlet. The circle is wall. I hope that someone can help me.
Thanks!
Attached Images
 K1024_image.JPG (87.2 KB, 42 views)

July 7, 2013, 14:28
#2
Senior Member

Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
While this topology is possible with a single O-grid, I prefer to mesh it with 12 domains - as seen in the attached picture. Sounds like a lot more but it doesn't take much effort and you can achieve a much higher quality mesh around the circle and in the wake.

-Chris

Quote:
 Originally Posted by Corleone84 Hello Guys, How can i create a structured domain for my simple 2D Geometry? How should i define the Domain and mesh it? Left edge is Velocity inlet and right edge is pressure outlet. The circle is wall. I hope that someone can help me. Thanks!
Attached Images
 box-cyl-struc-mesh.jpg (59.1 KB, 68 views)

July 9, 2013, 14:01
#3
New Member

Elham
Join Date: Jun 2013
Location: Germany
Posts: 8
Rep Power: 4
Quote:
 Originally Posted by cnsidero While this topology is possible with a single O-grid, I prefer to mesh it with 12 domains - as seen in the attached picture. Sounds like a lot more but it doesn't take much effort and you can achieve a much higher quality mesh around the circle and in the wake. -Chris
Hello Chris,
Thanks for your answer you helped me a lot. My plan was also to create the Domain like the one you created. I am already created a domain around the cylinder. I want to know how you could create 12 Domains in a rectangle.
I appreciate if you could help me.

July 10, 2013, 08:31
#4
Senior Member

Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
My general steps are:

1) Create the rectangular box around the circle with 4 connectors (don't worry about dimension and spacings yet)

2) Split the circle connectors (and/or domains) around the circle in 90 deg increments - as shown in mine. Be sure to have the first point 45 deg above the horizontal.

3) Split each of the 4 connectors from step 1 at two locations. The two locations will correspond to the two closet split points on the circle. When splitting a connector, you will notice that the split marker can only slid along the connector however you can still move the cursor unrestricted. Use this to your advantage by moving the cursor to one of the two closest circle split points until the snap circle highlights on your cursor and click on the circle split location. By doing this, the split location on the connector will line up with the split location on the circle.

4) Draw 2-point connectors from each new split location from step 3 to it's corresponding point on the circle.

5) Finally, adjust dimensions and spacing on the new connectors from preceding 4 steps so structured domains can be assembled.

Let me know if you have any more questions, Chris

Quote:
 Originally Posted by Corleone84 Hello Chris, Thanks for your answer you helped me a lot. My plan was also to create the Domain like the one you created. I am already created a domain around the cylinder. I want to know how you could create 12 Domains in a rectangle. I appreciate if you could help me.

July 10, 2013, 10:47
#5
New Member

Zhengbing
Join Date: Apr 2013
Posts: 20
Rep Power: 4
Hi,

I am also meshing this similar kind of geometry, but it's 3D.
I mesh the geometry with 14 blocks, 4 blocks around each cylinder, another 6 in the upsteam, middle and downstream of the channel.

Now I am a little confused about setting the boundary, exactly the domains on the symmetry plane. Should i see it as boundary or not.
If so, how should i give boundary to the symmetry plane? like interface or something else, but i cannot find it in Gridgen boundary settings.

If I don't set give boundary on the symmetry plane, wrong results will emerge when i do the simulation.

Thanks.

Quote:
 Originally Posted by cnsidero While this topology is possible with a single O-grid, I prefer to mesh it with 12 domains - as seen in the attached picture. Sounds like a lot more but it doesn't take much effort and you can achieve a much higher quality mesh around the circle and in the wake. -Chris
Attached Images
 Mesh.jpg (42.2 KB, 38 views)

July 10, 2013, 13:49
#6
Senior Member

Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
You should not have to nor need to set a CAE boundary condition on the symmetry because it will ultimately be part of the internal mesh, i.e. flow through.

Quote:
 Originally Posted by jimbean Hi, Now I am a little confused about setting the boundary, exactly the domains on the symmetry plane. Should i see it as boundary or not. If so, how should i give boundary to the symmetry plane? like interface or something else, but i cannot find it in Gridgen boundary settings. If I don't set give boundary on the symmetry plane, wrong results will emerge when i do the simulation. Thanks.

July 12, 2013, 12:05
#7
New Member

Elham
Join Date: Jun 2013
Location: Germany
Posts: 8
Rep Power: 4
Quote:
 Originally Posted by cnsidero My general steps are: 1) Create the rectangular box around the circle with 4 connectors (don't worry about dimension and spacings yet) 2) Split the circle connectors (and/or domains) around the circle in 90 deg increments - as shown in mine. Be sure to have the first point 45 deg above the horizontal. 3) Split each of the 4 connectors from step 1 at two locations. The two locations will correspond to the two closet split points on the circle. When splitting a connector, you will notice that the split marker can only slid along the connector however you can still move the cursor unrestricted. Use this to your advantage by moving the cursor to one of the two closest circle split points until the snap circle highlights on your cursor and click on the circle split location. By doing this, the split location on the connector will line up with the split location on the circle. 4) Draw 2-point connectors from each new split location from step 3 to it's corresponding point on the circle. 5) Finally, adjust dimensions and spacing on the new connectors from preceding 4 steps so structured domains can be assembled. Let me know if you have any more questions, Chris
@ Chris , it worked. thank you ever so much!

July 12, 2013, 21:26
#8
New Member

Zhengbing
Join Date: Apr 2013
Posts: 20
Rep Power: 4
Thank you, Chris.
Quote:
 Originally Posted by cnsidero You should not have to nor need to set a CAE boundary condition on the symmetry because it will ultimately be part of the internal mesh, i.e. flow through.

 July 13, 2013, 05:31 #9 Senior Member   Lefteris Join Date: Oct 2011 Location: UK, Greece Posts: 187 Rep Power: 5 Hi jimbean! Don't be confused by the geometric symmetry. The flow field is not symmetrical so you can't use this plane as a symmetry plane and set BC for symmetry. __________________ Lefteris

 July 13, 2013, 08:56 boundary conditions #10 New Member   Elham Join Date: Jun 2013 Location: Germany Posts: 8 Rep Power: 4 Hi I have a question about boundary conditions. Now i have 12 domains in Pointwise. in ansys, i get 3 different faces as inlet. I want to determine the inlet boundary condition for faces together. How can i connect these domains into a single boundary conditions? Thanks!

 July 13, 2013, 10:14 #11 Senior Member   Lefteris Join Date: Oct 2011 Location: UK, Greece Posts: 187 Rep Power: 5 In pointwise, you can select domains that are adjacent to each other and join them. __________________ Lefteris

July 15, 2013, 09:15
#12
Senior Member

Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
You group together multiple domains to form a single, coherent boundary condition in the CAE>Set Boundary Conditions menu. Be sure to set your solver first (CAE>Set Solver) because the BC physical types will be solver specific.

In short, go to the panel I mention, create a BC (click New), select the domains that form the BC you want (e.g. inlet), click in the check box in your new BC's row to assign them. Repeat for remaining BCs.

The same idea applies in 3D for blocks with volume conditions. For some solvers, volume conditions aren't necessary but others the are, e.g. Fluent. Because Pointwise allows one to create multiple 3D mesh regions, called blocks, but often represent a single fluid (or solid) region, blocks can be assigned to a single "volume condition". This is done is similar manner as boundary conditions.

Quote:
 Originally Posted by Corleone84 Hi I have a question about boundary conditions. Now i have 12 domains in Pointwise. in ansys, i get 3 different faces as inlet. I want to determine the inlet boundary condition for faces together. How can i connect these domains into a single boundary conditions? Thanks!
I would not recommend joining domains just to get the boundary conditions you desire in the solver. First, because it's not always possible to join structured domains due to topology. Second, because it can be more difficult to modify you mesh subsequently. Third, because getting the boundary conditions you desire is best accomplish by the above procedure.

Quote:
 Originally Posted by Aeronautics El. K. In pointwise, you can select domains that are adjacent to each other and join them.
Good luck. Let me know if have any more questions.

-Chris

 July 16, 2013, 05:22 #13 Senior Member   Lefteris Join Date: Oct 2011 Location: UK, Greece Posts: 187 Rep Power: 5 Chris you're right and your help is always invaluable. This is a simple domain though and that's why I said he could join the three domains together. __________________ Lefteris

 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 Kryo Pointwise & Gridgen 2 January 16, 2013 17:49 [ANSYS Meshing] Displaying solid domains in CFD Post without meshing them. hda ANSYS Meshing & Geometry 2 January 24, 2012 00:21 kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45 Chander CFX 3 November 27, 2011 17:24 Scott CFX 8 July 31, 2008 15:20

All times are GMT -4. The time now is 07:03.