CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ANSYS Meshing] Advice for meshing of corrugated tubes (

subsemitonium June 17, 2011 08:16

Advice for meshing of corrugated tubes needed
1 Attachment(s)

I'm simulating turbulent tube flows. Until now I only tried smooth pipes which worked well! I generated a hexa mesh (multizone) with prism layers.

Now I attempt to simulate a flow through corrugated tubes (twisted/spiral and not twisted). But I encounter some difficulties while meshing:
- When I use sweep method (help read: reduces amount of knodes when geometry is repeating...) it smoothes all waves out until I have a completely straight pipe...
- When I use Multizone method, the geometry gets completely out of shape
- When I use automatic, everything seems fine (attachment), apart from the fact that I get about 4 million knodes for 10cm pipe... since my model shall be about 1m long that's obviously too much. I assume hexamesh - which i used for the smooth pipe - is better?

I need high density at the boundaries (which is why I tried with inflation) and low growth rates.
But I'm not sure which options are best and beg for advice, since my experience in meshing is still limited and i was glad to get the turbulence model for the smooth pipe the way i wanted it to be :(. Thanks for any hints.

PSYMN June 18, 2011 20:30

I would have recommended the Sweep method for this. But I don't understand what you mean by "it smooths all the waves out"...

Sweep should follow your geometry, not straighten it out. Can you post a pic of that?

The mutlizone method could work well, but you will probably need to use virtual topologies to group together some of the patches...

subsemitonium June 20, 2011 04:56

2 Attachment(s)
Thanks for you reply, I've been away over the weekend, so i just read it.

What I meant by 'straightened out' is, that the meshing method I tried converted the corrugated pipe into a smooth tube (without waves). I'm sure it's my fault but I simply don't know how to change that. Attached you'll find both geom files (corrugated and spiraled pipe) as well as some pics of the problem.

In the not spiraled corrugated tube I couldn't use sweep - it caused errors not being able to find source and targets. Manually selection could not solve that. Propably my mistake is that I added a symmetry plane in the centre which can not be used with sweep (?). I'll check that today!

Worse is the spiraled tube. This morning, I cutted the pipe to only 4 twists and retried. Multizone totally deforms the net, while sweep only produces errors reading 'net could not be finished because of elements with bad quality...'.

Thanks in advance!

P.S.: ...geometry file for normally corrugated tube was too big to be attached. I'll try to cut it and mesh without symmetry plane...

sac June 20, 2011 12:35

  1. Slice in half in DM and then make a multibody.
  2. Apply a Multizone control
  3. Apply a sizing control of 0.0005m

subsemitonium June 21, 2011 04:37

Thanks for your hint, can you give a little more information as I didn't use such method before and I'm not familiar in multibody/multizone combination.

Sweep method kepps on producing errors... I use manually source selection and choose the pipes inlet. Anyway Ansys is not capable of finding target planes... are spirals not ideal for sweep meshes?
Thanks in advance!

sac June 21, 2011 05:25


Originally Posted by subsemitonium (Post 312857)
Thanks for your hint, can you give a little more information as I didn't use such method before and I'm not familiar in multibody/multizone combination.

The basic idea is this.

If you have a body that is not sweepable then you need to slice it into sweepable sections to get a hex mesh. This making sweepable sections is the basis for ANY hex meshing tool - automated or otherwise.

The sweep method assumes that you already have sweepable sections. If you do not then it can't sweep it and you need to go back and slice your model up into sweepable sections.

The Multizone method uses an automated blocking method. This achieves the same purpose as the above but without changing the geometry. Instead it creates internal blocks that define the "sweepable" sections.

In this case MZ was having problems blocking this geometry. So I introduced a slice to help it out. In ANSYS meshing if you want a conformal mesh you need to put them in a multibody part (hence why I put them in that part).


Sweep method kepps on producing errors... I use manually source selection and choose the pipes inlet.
Well that's the problem with any automation - sometimes it will get it wrong or cannot find a source. That's why you have manual methods of doing things.

subsemitonium June 21, 2011 06:23

1 Attachment(s)
Thanks for your explanation, this sounds somehow logical. Yet, I'm doing something wrong. I attached a pic with my settings and the error that keeps on occuring. (I hope you can read it, since the 97kb treshold is quite low...)

What I did:
- In DM I sliced the cylinder in the middle (in two halfs)
- In Ansys Meshing [AM] I selected the components IN OUT and PIPE (wall)
- I added Multizone and selected both bodies (upper and lower half)
- Since a structured net seems to make sense I set structured net to heax/prism (I need prism to simulate turbulence and heat transfer)
--> The mesher does not seem to like those settings... did I get you wrong?

subsemitonium June 22, 2011 10:42

Wow, now I got my mesh quite appropriate. I did as you said and sliced the cylinder, applying the sweep method to every hald-cylinder seperately. The mesh look not bad, though I still have to think about reducing the amount of nodes - that's another problem :)

One more question: When I have that wavy structure, is there a possibility to plot (in cfx-post) something along the wall? In a straight tube, I can add a line at the wall and can use it for plotting... how do I manage that having such wavy structure?

subsemitonium June 28, 2011 03:51

1 Attachment(s)
Hi, I have to reconsider my happiness... simulation results show that the mesh I generated is not appropriate yet.
I sliced the body in two halfs and applied sweep method for each one. The mesh looks quite good, but at the point where the two halfs meet (the attached pic shows a second attempt with four quarters which results in the same effect) the mesh behaves "differently" which I can later see in the simulation results...
Do you have any ideas how I can get the mesh more structured and more 'even' ?

PSYMN June 28, 2011 08:52

You could set finer sizes along the interior edges...

Or you could subdivide into an ogrid type structure...

subsemitonium June 28, 2011 09:50

I read the helpfile and I am not sure whether I got the facts about O-grids:

- O-grids are the inflation layers of a multizone mesh?

...but I couldn't figure out how to build one. I selected the body (all in one body), added a multizone method and chose tetra/prism for structured mesh.
Is that all?? :confused:

PSYMN June 28, 2011 13:40

1 Attachment(s)
I just meant you could subdivide the model into blocks that would be mappable... like an ogrid configuration.

Right now, you have triangles... You can't map triangles.

But if you divided it into an OGrid shape, you could map each section...

Attachment 8209

subsemitonium June 29, 2011 04:39

That sounds interesting! I'm trying to slice as you said, but I assume there is some sort of autofunction for creating o-grid shapes? I'm studying the help files right now but can't find anything appropriate... do you have any more hints?

Edit the question: I just saw your video on youtube. Is O-grid generation in Ansys Meshing possible? Or do I have to learn ICEM? Can't find any help about O-grid/blocking in Ansys meshing...

PSYMN June 29, 2011 11:36

We have the auto-function in ICEM CFD, but for WB (DM), you just need to slice it manually and then the mesher can map the faces and sweep the 5 components.

subsemitonium June 30, 2011 05:35

I sliced exactly as you said, but still I can't get it meshed... you said "the mesher can map and sweep it". I selected the five bodies and added the method "multizone (hex dominant - quads/triangles)" and got errors like the program had a communication problem, do you want to send the report to microsoft?...
I changed the method to sweep for all five bodies (as you proposed) but for half an hour nothing seems to happen - though I chose the cell size much greater than I need it? I also added a "element size on surface" method - without success. The central body needs about 10 seconds to mesh, but the outer bodies don't seem to work properly... can you explain the method a little or do you see any mistakes?

edit: may be it's important to mention that when I chose sweep, ansys claims that there are NURBS surfaces which might take longer. I followed the advice and set smoothing to low...

PSYMN July 1, 2011 16:12

Sorry, not sure. It should have worked just as your previous sweep had done, except that the source mesh could be mapped...

pradeeppandeygbpec March 4, 2016 03:49

Advise for using swept multizone mesh for complex geometries
Dear Simon,
Many Greetings. I want to mesh a moderately complex geometry : venturi with nozzles on throat placed inside a tank.

My strategy for multizone hex meshing is :
1. Initiate 2D surface blocking & create surface mesh
1.1 Method : Swept
1.2 Free face Mesh type : Quad dominant
1.3 Free face mesh method: Gambit Pave

2. Create volume mesh using 2D to 3D Multi-zone fill (Fill type is swept) and create O-Grid around faces.

However, when I am following the above steps, the 2D surface mesh is very poor. Some of the surfaces are not meshed and some are meshed horribly weird.

I think I will have to manually define "Swept Surfaces", (but I donít know what surface to select). Can you suggest some trick for above situation. Please redirect if there is any tutorial example.

All times are GMT -4. The time now is 05:46.