# Multi meshing blocks

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

 October 19, 2010, 10:31 Multi meshing blocks #1 Member   Daniel Valero Join Date: Sep 2010 Location: Valencia, Spain Posts: 35 Rep Power: 6 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!

 October 20, 2010, 03:18 Multi meshing blocks #2 New Member   Renaud GORRIA Join Date: Oct 2010 Posts: 3 Rep Power: 6 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)

October 21, 2010, 07:52
#3
Member

Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
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?

Quote:
 Originally Posted by Renaud GORRIA 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)

 October 22, 2010, 02:52 #4 New Member   Renaud GORRIA Join Date: Oct 2010 Posts: 3 Rep Power: 6 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?

 October 23, 2010, 15:02 #5 Senior Member   michael barkhudarov Join Date: Mar 2009 Posts: 331 Rep Power: 9 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.

October 24, 2010, 09:25
#6
Member

Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Quote:
 Originally Posted by MuxaB 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!

 October 26, 2010, 04:54 #7 New Member   Renaud GORRIA Join Date: Oct 2010 Posts: 3 Rep Power: 6 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.

 October 29, 2010, 00:27 #8 Senior Member   michael barkhudarov Join Date: Mar 2009 Posts: 331 Rep Power: 9 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).

October 30, 2010, 16:03
#9
Member

Daniel Valero
Join Date: Sep 2010
Location: Valencia, Spain
Posts: 35
Rep Power: 6
Quote:
 Originally Posted by Renaud GORRIA 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 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!

 November 1, 2010, 00:50 #10 Senior Member   michael barkhudarov Join Date: Mar 2009 Posts: 331 Rep Power: 9 You are very welcome, Davahue. Glad it worked.

 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 archymedes OpenFOAM Pre-Processing 93 February 11, 2014 02:22 bego OpenFOAM 27 May 29, 2013 13:08 fluidpath OpenFOAM Native Meshers: snappyHexMesh and Others 4 May 19, 2013 19:13 Alan OpenFOAM Native Meshers: blockMesh 0 July 27, 2009 20:05 jeevan kumar CFX 1 April 22, 2008 00:45

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