CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

Multi meshing blocks

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 19, 2010, 10:31
Exclamation Multi meshing blocks
  #1
Member
 
Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Davahue is on a distinguished road
Hi, I've been trying to use some blocks at the same simulation. First, I have fixed some points to enhance the blocks and I've restricted manually the ratio between both block's cells near the unity.

But when I simulate, it's like the flow stops at the boundary, like a wall!
I've been trying with outflow B.C. allowing inflow, and continuity B.C. but the problem persists...

What's Wrong? Could anybody help me please?
thanks in advice!
Davahue is offline   Reply With Quote

Old   October 20, 2010, 03:18
Default Multi meshing blocks
  #2
New Member
 
Renaud GORRIA
Join Date: Oct 2010
Posts: 3
Rep Power: 6
Renaud GORRIA is on a distinguished road
Hello,

You should set Symetry BC between the different blocks of your simulation. It will works

(symetry means "by default" in this case, the solver reads it corretly as a condition between multi-blocks)
Renaud GORRIA is offline   Reply With Quote

Old   October 21, 2010, 07:52
Default
  #3
Member
 
Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Davahue is on a distinguished road
I've checked symmetry BC at the Boundary tabs for the block #2 (that is into the block #1), I run simulation and I still get the same problem, what happens? is this the BC you told me? or can I edit another kind of BC between blocks?

thanks in advice!

Quote:
Originally Posted by Renaud GORRIA View Post
Hello,

You should set Symetry BC between the different blocks of your simulation. It will works

(symetry means "by default" in this case, the solver reads it corretly as a condition between multi-blocks)
Davahue is offline   Reply With Quote

Old   October 22, 2010, 02:52
Default
  #4
New Member
 
Renaud GORRIA
Join Date: Oct 2010
Posts: 3
Rep Power: 6
Renaud GORRIA is on a distinguished road
You must check all the six-BC of the block 2 as Symmetry BC.

And if the block 2 considers one side which is the same plane that a side of the block 2 (for example your block 2 is inclued in Blk1 but both start on X=0), so you have to check the same BC on the 2 sides (blk1 ande blk2). For my example Specified Presssure on X=0.

Is it your case? Is your blk2 totally inclued in blk1?
Renaud GORRIA is offline   Reply With Quote

Old   October 23, 2010, 15:02
Default
  #5
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
One possible reason two adjacent mesh blocks not to be connected properly is a gap between them, so make sure that the coordinates of the mesh boundaries on both blocks are identical.

The definition of the inter-block block boundaries depends only on the relative position of the blocks, i.e., the coordinates of the boundaries. Once the pre-processor determines that the two mesh blocks are adjacent, it set the boundary type to inter-block irrespective of the user input.

The parts of an inter-block boundary that are NOT facing another block are always treated as a wall.
MuxaB is offline   Reply With Quote

Old   October 24, 2010, 09:25
Default
  #6
Member
 
Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Davahue is on a distinguished road
Quote:
Originally Posted by MuxaB View Post
One possible reason two adjacent mesh blocks not to be connected properly is a gap between them, so make sure that the coordinates of the mesh boundaries on both blocks are identical.

The definition of the inter-block block boundaries depends only on the relative position of the blocks, i.e., the coordinates of the boundaries. Once the pre-processor determines that the two mesh blocks are adjacent, it set the boundary type to inter-block irrespective of the user input.

The parts of an inter-block boundary that are NOT facing another block are always treated as a wall.
My block 2 is completly into de block 1, I've set 2 fixed points in each direction, and I've set simmetry boundary conditions in Boundaries... but it still don't run as I want.. it runs the boundaries as a wall.

When I start to simulate, I get that message:

open area mismatch at inter-block boundaries of all blocks as % of total open area at these mesh boundaries = 5.96348E-12

so I think, I've put correclty all.. but there should be a problem at the BC so I've copied here my text information:
&bcdata

wl=11, wr=8, wf=2, wbk=2,
flrbct(1,1)=16.,

/


&mesh


nxcelt=80, px(2)=-3., nycelt=40, nzcelt=10, pz(2)=1.0, px(1)=-10., py(1)=-4., py(2)=-2., pz(1)=0.0, px(3)=7., px(4)=20., py(3)=2., py(4)=4.,

/

&bcdata

iobctp(1)=1, iobctp(2)=1, iobctp(3)=1, iobctp(4)=1, iobctp(5)=1, iobctp(6)=1, ipbctp(1)=0,

/

&mesh

nxcelt=100,
px(1)=-3., px(2)=7., nycelt=100, py(1)=-2., py(2)=2., nzcelt=10, pz(1)=0.0, pz(2)=1.0,

/


Another appointment is that when I see the results, the solid that is into the block 2,
don't seem to have the resolution it must have, it has the definiton that the block 1 gives it...
I've also tried to put interblock BC manually and doesn't happen anything different!

Could help me please?

thanks in advice!
Davahue is offline   Reply With Quote

Old   October 26, 2010, 04:54
Default
  #7
New Member
 
Renaud GORRIA
Join Date: Oct 2010
Posts: 3
Rep Power: 6
Renaud GORRIA is on a distinguished road
In your prepin I can see that the top and the bottom of the blk1 and blk2 are adjacent. I think it comes from this point... try to set up a blk2 strickly IN the blk1.
Renaud GORRIA is offline   Reply With Quote

Old   October 29, 2010, 00:27
Default
  #8
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Even with coincidental bottom and top boundaries in z-direction, it looks in order to me. The flow should proceed along the x-direction. Could you please attach an image of the solution you receive?

One other question. When you post-process do you have both blocks selected under Mesh Block button in Analyze tab or just block 1 (which would be the default in earlier versions of FLOW-3D).
MuxaB is offline   Reply With Quote

Old   October 30, 2010, 16:03
Default
  #9
Member
 
Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Davahue is on a distinguished road
Quote:
Originally Posted by Renaud GORRIA View Post
In your prepin I can see that the top and the bottom of the blk1 and blk2 are adjacent. I think it comes from this point... try to set up a blk2 strickly IN the blk1.
Quote:
Originally Posted by MuxaB View Post
Even with coincidental bottom and top boundaries in z-direction, it looks in order to me. The flow should proceed along the x-direction. Could you please attach an image of the solution you receive?

One other question. When you post-process do you have both blocks selected under Mesh Block button in Analyze tab or just block 1 (which would be the default in earlier versions of FLOW-3D).
Now it runs ok, the problem was in the postprocess, I didn't konw that I had to check both meshes, I hadn't seen this tab in Analyze, now it's all OK. Thanks!!
I'm very gratefull with both of you, I hope it could help somebody else!
Davahue is offline   Reply With Quote

Old   November 1, 2010, 00:50
Default
  #10
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
You are very welcome, Davahue. Glad it worked.
MuxaB 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
dsmcInitialise - dsmcFoam archymedes OpenFOAM Pre-Processing 93 February 11, 2014 02:22
fluent3DMeshToFoam bego OpenFOAM 27 May 29, 2013 13:08
Multi region meshing & recovering the original patch names fluidpath OpenFOAM Native Meshers: snappyHexMesh and Others 4 May 19, 2013 19:13
Problems meshing wedge type blocks Alan OpenFOAM Native Meshers: blockMesh 0 July 27, 2009 20:05
How to creat Chimera structured multi blocks grid jeevan kumar CFX 1 April 22, 2008 00:45


All times are GMT -4. The time now is 23:33.