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] Meshing pipe with different diameters (http://www.cfd-online.com/Forums/ansys-meshing/116701-meshing-pipe-different-diameters.html)

Axlex April 23, 2013 11:02

Meshing pipe with different diameters
 
Hello,

i'm pretty new to icem cfd. I am trying to mesh a pipe, in which the diameter jumps from d1 to d2 and after some distance back to d1.

First thing i tried, was to split the block into 3 parts and then do the mesh refinement. The problem is, that at the transition of the blocks the mesh is "compressed" to the smaller diameter and therefore is of poor quality.

Any suggestions, how to do it right?

Best Regards
Robert

diamondx April 23, 2013 11:46

can we get a picture of what it looks like ?? your case is easy, make sure you have an o-grid...

FJSJ April 23, 2013 11:52

I don´t know if your doubt is about blocking or edge params...

Take a look at this video:

http://www.youtube.com/watch?v=tAMMnJKYG7c

And, if the doubts are about edge params.. try "match edges" between cylinder d2 and d1.

Axlex April 24, 2013 08:53

5 Attachment(s)
Hallo,

thanks for the answers so far. I was watching your video and the merge vertices option was new to me. thanks for this. But the problem is still there.
picture 1 shows the case, picture 2 blocking, picture 3 the mesh from the front before smoothing, picture 4 the mesh after smoothing and the quality and picture 5 the ligned blocks

my blocking strategy is:
  1. split the main block into 5 pieces and delete the even ones
    or
    split the main block into 3 piece, ogrid block 2 and remove the outer ogrid-blocks (delete the connecting blocks between the main blocks, which are generated)
  2. associate the edges to curves (block 1 and 3 to the outer circles and block 2 to the inner circles
  3. ogrid on block 1 and 3 and associate the inner blocks to the inner circles
  4. ogrid on the inner blocks of block 1 and 3 in the same manner as block 2

Where is my mistake?

RodriguezFatz April 24, 2013 09:54

Looks like some confusion with edge associations. Right click on edges and chose "show associations". All edges that are associated to the geometry will get an arrow and show you where they are linked to. It looks like one of your "inner" edges is accidentally linked to the outer surface.
ps: blocking is perfect

Axlex April 24, 2013 10:15

2 Attachment(s)
thank you for the answer.

the edges are associated to the right curves like shown in picture 1. In picture 2 is a closer look at the inner associations. Could this be aproblem or is this only a "graphical feature" of icem.

FJSJ April 24, 2013 10:41

Hi Alex,
I would say two things. Firstly, make sure you don't have overlap sufaces when diameter jumps from d1 to d2. Secondly, make sure you´ve not compressed a face from o-grid.

RodriguezFatz April 24, 2013 10:46

In picture 2 you can see the problem: The gray arrows shouldn't be there. Chose "dissociate from geometry" and then click on all the inner edges and points!

Axlex April 25, 2013 05:37

These arrows really were the problem, but i was not able to erase them all. After some time i noticed, that these associations were only at the transition to the middle pipe. The only difference was, that i didn't set a surface there, because i thought it is not needed. After inserting a surface the associations were gone.

Thank you very much for the help.

Far April 25, 2013 06:57

Quote:

After inserting a surface the associations were gone.
Do you have baffle there ? If not don't insert surface inside the fluid domain.


The blocking where you have problem was made using extrude along curve option?

Working solution which I have implemented yesterday is:

1. Draw two scan planes perpendicular to cross sectional area.

2. If there is problem in mesh and try to locate those problem blocks

3. Delete them

4. Create new block through vertices (for 3d you have 8 vertices for each block).

Axlex April 25, 2013 07:59

Thanks for your reply. You are right, i am facing this problem now, because the fluid domain gets divided and therefore the solver doesn't start, showing "3 isolated fluid regions were found in domain Fluiddomain" message.

Declaring these both surfaces as opening and not defining them as parts doesn't work.

I made the geometry with DesignModeler from workbench and imported it via workbench reader.

As shown in my 3rd post, the problem occurs when i associate the edges to the circle. When i delete these blocks and create new ones, i still need to associate them to the geometry and the same problem will occur.

Edit:
It happens, when i apply an ogrid to the blocks associated to the circles, then the inner block gets associated to the circles too

RodriguezFatz April 25, 2013 08:19

Can you upload the ICEM files (the original ones, without that extra surface)?

Axlex April 25, 2013 08:39

1 Attachment(s)
Sure, here it is. :D

RodriguezFatz April 25, 2013 09:14

Something is wrong with your faces. Some of the inner faces are associated to the surfaces of the geometry. But once I fixed that, I get "uncovered faces" error for the transition from the small to the larger pipe... In Design modeler, do you have several (3d) parts? Or did you joined them (group)?

Axlex April 25, 2013 09:24

i only made 3 cylinder and named the parts.

I also tried to build the geometry in ICEM and the same problem occured.

BrolY April 25, 2013 09:32

You did it in the wrong way. You have multiple block at the intersection of your 2 tube. Besides, the edges and vertices should not be black, but blue because they are inside the fluid.

How to block this geoemtry :

1) create a whole block around your tubes.
2) split the block at the tube intersections.
3) create o-grid inside to capture the geoemtry of the small tube.
4) create another o-grid inside the 1st one to improve the cells quality inside the small tube.

Far April 25, 2013 09:37

Every thing is fine when blocked with top-down approach. Did you make blocking through bottom-up approach?

Axlex April 25, 2013 10:46

@Far
If you mean with top down method to create one main block and divide it, then yes.

@BrolY
Your approach seems similar to the one in my second post with 1 b), but i cant reproduce yours.
When are u making associations. If i only associate the outer circles, then the inner block of the first o grid wont be circular and therefore wont catch the geometry of the small pipe.

sorry for the inconvenieces.

RodriguezFatz April 25, 2013 10:58

5 Attachment(s)
Grid in 8 steps:
Attachment 21134
Attachment 21135
Attachment 21136
Attachment 21137
Attachment 21138
...

RodriguezFatz April 25, 2013 10:59

3 Attachment(s)
...
Attachment 21139
Attachment 21140
Attachment 21141
Here we go!

Step 1: Create a single block.
Step 2: Snap-associate the outer edges (green) to the circles.
Step 3: Create an o-grid - select the inlet and outlet under "faces" to let the o-grid enter end leave the pipe.
Step 4: Cut the block at the two large circles and associate the inner edges to the inner circle.
Step 5: Line all inner edges parallel.
Step 6: Do the same (4) with the inner block.
Step 7: Delete the outer blocks around the small pipe.
Step 8: Grid!


All times are GMT -4. The time now is 23:08.