CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Blocking topology for pipe flow with a butterfly valve

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

Like Tree8Likes
  • 2 Post By PSYMN
  • 1 Post By PSYMN
  • 1 Post By Far
  • 1 Post By Far
  • 1 Post By snpradeep
  • 1 Post By snpradeep
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   September 15, 2011, 06:43
Default [ICEM] Blocking topology for pipe flow with a butterfly valve
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Hi,

There's a tutorial in CFX for flow through a pipe with a butterfly valve, which uses an unstructured mesh. So for mesh generation practice I'm trying to make an ICEM Hexa mesh for this type of geometry. Can anyone suggest a blocking topology for around the open valve?

I can never work blocking topologies out, goodness knows how anyone can learn this stuff

Thanks.
siw is offline   Reply With Quote

Old   September 16, 2011, 03:51
Default
  #2
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Could you post a picture of the geometry ?
BrolY is offline   Reply With Quote

Old   September 16, 2011, 09:09
Wink Blocking gene?
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I used to give a lot of training classes before I got into product management and I was starting to formulate a theory about a "hexa" gene. It just seemed like some people just naturally took to hexa blocking and others could never wrap their heads around it...

In this case, the pipe requires an Ogrid along its length (with faces at the corners...

The butterfly valve can be imagined as in a sphere (so you could move it to any angle...) so we would usually put the sphere in the geometry and do it as two blocking files, one to the outside of the sphere and one within the sphere and then we could rotate the inner blocking to any angle...

If you want a single volume and you know your valve is mostly open, then you could imagine it as a second pipe perpendicular to the first... This can be easily blocked by splitting upstream and downstream of the valve and then putting an OGrid in that block. You could do it with our without faces on two sides of the pipe (pretend there is a perpendicular pipe and the butterfly is just a slice of it...)

Then you slice that imaginary perpendicular pipe to cut out the butterfly valve and put it into a solid part (or just delete those blocks).

If you are modeling the pin for the butterly valve, then that is another Ogrid in that direction...

Best regards,

Simon
Far and snpradeep like this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   September 16, 2011, 09:13
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Oh yes, to be clear...

When doing the Ogrid for the valve or the pin, you will need the ogrid to start around the object to capture boundary flow. However, for the valve, which has mesh on its side also, you will need the central Hgrid to be well within the valve where it is not associated to any curves. Otherwise you will have 180 degree elements at the corners of the valve. The same would apply to the pin if you are modeling the solid for FSI...

So, make the Ogrid start outside the valve and extend to well inside the valve, then split it for the edge of the valve and associate that...

Get it?

If not, start down the path and send pics. It is easier to steer a moving car.
Far likes this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   November 23, 2012, 15:55
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
How to draw the sphere ...
Far is offline   Reply With Quote

Old   November 24, 2012, 22:37
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
There are options under create surfaces to create primitives such as a sphere or cube... Usually, I create two points first (to be the "poles" of my sphere) and then select them during the sphere creation process...

Put the sphere in a new part, something like "INTERFACE"...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   November 25, 2012, 01:53
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by PSYMN View Post
There are options under create surfaces to create primitives such as a sphere or cube... Usually, I create two points first (to be the "poles" of my sphere) and then select them during the sphere creation process...

Put the sphere in a new part, something like "INTERFACE"...
Previously I understood that you are talking in terms of the blocking.

Creating the sphere in the circular pipe would create the single point contact with the pipe? Circular hinge will be the part of the that sphere or not? Where this sphere should be created?


Here I have made the blocking for butterfly vavle geometry from the CFX tutorial.

https://dl.dropbox.com/u/68746918/project5tin.zip
Attached Images
File Type: jpg butterfly_valve001.jpg (77.3 KB, 48 views)
File Type: jpg butterfly_valve002.jpg (76.3 KB, 42 views)
File Type: jpg butterfly_valve003.jpg (66.3 KB, 45 views)
File Type: jpg butterfly_valve004.jpg (91.5 KB, 40 views)
File Type: jpg butterfly_valve005.jpg (66.6 KB, 34 views)
snpradeep likes this.
Far is offline   Reply With Quote

Old   November 25, 2012, 02:37
Default
  #8
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by PSYMN View Post
There are options under create surfaces to create primitives such as a sphere or cube... Usually, I create two points first (to be the "poles" of my sphere) and then select them during the sphere creation process...

Put the sphere in a new part, something like "INTERFACE"...
Should I make the two fluids : fluid1 and fluid2 and then make the shared wall?


Here is the blocking after making the o-grid around the valve and hinge, but quality is no good.

What is main idea/trick behind blocking the such cases?

https://dl.dropbox.com/u/68746918/Bu...e_project6.rar
Attached Images
File Type: jpg butterfly_valve2.jpg001.jpg (89.6 KB, 26 views)
File Type: jpg butterfly_valve2.jpg002.jpg (84.2 KB, 23 views)
File Type: jpg butterfly_valve2.jpg003.jpg (94.9 KB, 26 views)
File Type: jpg butterfly_valve2.jpg004.jpg (55.5 KB, 17 views)
File Type: jpg butterfly_valve2.jpg005.jpg (91.6 KB, 16 views)
snpradeep likes this.
Far is offline   Reply With Quote

Old   November 25, 2012, 03:12
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I read about the FE modeller that is very efficient to get the good quality geometry from the mesh file. Used following steps:

1. Import mesh file (.def in my case)
2. Skin the mesh using the option "curves"
3. Create the initial goemetry
4. Convert to "Paralsolid"

But got the problem in parasolid, where geometry is distorted (last pic). Any hint please...
Attached Images
File Type: jpg butterfly_valve3.jpg001.jpg (23.8 KB, 13 views)
File Type: jpg butterfly_valve3.jpg002.jpg (76.5 KB, 13 views)
File Type: jpg butterfly_valve3.jpg003.jpg (90.1 KB, 18 views)
File Type: jpg butterfly_valve3.jpg004.jpg (87.9 KB, 18 views)

Last edited by Far; November 25, 2012 at 05:05. Reason: spelling mistake
Far is offline   Reply With Quote

Old   November 25, 2012, 07:12
Default
  #10
New Member
 
Pradeep
Join Date: Nov 2009
Location: Duisburg
Posts: 23
Rep Power: 7
snpradeep is on a distinguished road
I think starting with quarter geometry is a good idea..Once you have made blocking for quarter section properly, delete unwanted blocks and generate a quality mesh..Later copy the blocking for full model and reassociate and merge nodes if required..This can be quite effective..But only problem with this is it will lead to lot of splits..
Attached Images
File Type: jpg valve1.jpg (97.1 KB, 21 views)
File Type: jpg valve2.jpg (38.1 KB, 22 views)
Far likes this.
snpradeep is offline   Reply With Quote

Old   November 25, 2012, 07:21
Default
  #11
New Member
 
Pradeep
Join Date: Nov 2009
Location: Duisburg
Posts: 23
Rep Power: 7
snpradeep is on a distinguished road
Quote:
Originally Posted by BrolY View Post
Could you post a picture of the geometry ?
Dear Mr. Boles,

Please find the eclosed pic. of the geometry..
I am sorry for the wrong post..

Regards,
Pradeep
Attached Images
File Type: jpg Geometry.jpg (14.9 KB, 19 views)
Far likes this.

Last edited by snpradeep; November 25, 2012 at 07:30. Reason: apology.
snpradeep is offline   Reply With Quote

Old   November 27, 2012, 11:21
Default
  #12
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
When I suggested a sphere, I was assuming that you would have a non-conformal interface...

I was assuming you would add a sphere around the moving valve, call that INTERFACE. The sphere should not go to the wall of the tube, but should cut across the bar between the valve and the wall. Then you block the model in two parts.

One part is just the pipe assembly and the outside of the sphere... (blocking is just an ogrid in the pipe, delete the central block.)

The other part is the valve inside the sphere. This starts with an Ogrid to capture the sphere, then split to capture the valve. You will probably need to drill an ogrid tube thru the sphere for the bar in the valve, and the valve its self is just a couple splits...

Then output the mesh from both of these models and either bring them together in ICEM CFD, adjust the position of the valve and output to the solver, or load them into the solver separately. Set up the two zones and the interface. The one zone can rotate about an axis controlled by a udf or something like that ...

Get what I mean?
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   November 27, 2012, 11:25
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Got it...

Can we get the good quality hexa mesh with this valve setting for full geometry without inserting interface i.e.. full conformal mesh.
Far is offline   Reply With Quote

Old   November 27, 2012, 13:07
Default
  #14
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yes, you can do it as one piece, but you end up needing 2 or 3 different blockings to cover different ranges in the valve motion...

You may have one blocking where the valve is a split along the duct direction. As the valve closed, This would get deflected upward until the quality was considered too poor... THen you would switch to another blocking, perhaps one with a vertical split for the valve, or perhaps some intermediate and more advanced blocking would be needed first...

You would then select the blocking based on the angle of the valve.

I have seen it done in WB where the geometry system is connected to 3 mesh systems (each of which loads an ICEM CFD replay file corresponding to a specific topology) and then those all connect back to a solver. The solver selects which mesh to use based on the valve angle.

Best regards,

Simon
blackmask likes this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN 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
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31
Flow visualization vs. Calculated flow patterns Francisco Saldarriaga Main CFD Forum 1 August 2, 1999 23:18
Question on 3D potential flow Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18
computation about flow around a yawed cone Tylor Xie Main CFD Forum 0 June 9, 1999 07:33
CFD Application in hydraulics valve flow Roger Yang Main CFD Forum 11 February 11, 1999 17:53


All times are GMT -4. The time now is 04:44.