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

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

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.

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?

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

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.

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.

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!

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.

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).

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

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

Sure, here it is. :D

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)?

i only made 3 cylinder and named the parts.

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

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.

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

@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.

Grid in 8 steps:
Attachment 21134
Attachment 21135
Attachment 21136
Attachment 21137
Attachment 21138
...

...
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!

AT LAST!!! This was a difficult birth like we say here. :D

I almost got the working steps from the pictures, but this took some time. The explanations were helpful.

I still don't get the difference, but thats ok. I will repeat that for different geometries and then i hopefully understand it.

Thanks for the kind help.

From what I understood, your mistake was to associate the o-grid you created in block 1 and 3 and associated the edges of those o-grids with the curves of the small tube. Because before that, you already associated the edges of the o-grid of bloc2 with the curves of the small tube.
So you have 2 edges for 1 curve, which is wrong. It created a 0-volume at the junction of the tubes.

I hope my explanations were clear ...

OK, i think i understand it now.

Thanks for the help! :)

In addition to that there were duplicate blocks as well. Once I merge them and made the inner edges black (surface associated edges) problem was solved.

hi there, im trying to mesh a geometry very similar to this, the only difference being that the central pipe section is very short and behaves like an orifice. The steps are very clear in this post but could someone please further clarify step 6 please.
thanks in advance

Hello, is it possible to do this grid on workbench mesher?

Regards,
Tanjina

Hi Tanjina,

I think you could try to do it but you need to split your geometry to get parts as O-grid topology approach. Take a look at this thread:

[ANSYS Meshing] Problem with structured meshing pipe elbow

:)

Thanks ! I am trying..... but it seems I have some problem.