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

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

 September 15, 2011, 06:43 [ICEM] Blocking topology for pipe flow with a butterfly valve #1 Senior Member   Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 484 Rep Power: 15 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.

 September 16, 2011, 03:51 #2 Senior Member   AB Join Date: Sep 2009 Location: France Posts: 323 Rep Power: 14 Could you post a picture of the geometry ?

 September 16, 2011, 09:09 Blocking gene? #3 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 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

 September 16, 2011, 09:13 #4 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 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

 November 23, 2012, 15:55 #5 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,285 Blog Entries: 6 Rep Power: 43 How to draw the sphere ...

 November 24, 2012, 22:37 #6 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 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

November 25, 2012, 01:53
#7
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Quote:
 Originally Posted by PSYMN 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
 butterfly_valve001.jpg (77.3 KB, 60 views) butterfly_valve002.jpg (76.3 KB, 52 views) butterfly_valve003.jpg (66.3 KB, 58 views) butterfly_valve004.jpg (91.5 KB, 53 views) butterfly_valve005.jpg (66.6 KB, 45 views)

November 25, 2012, 02:37
#8
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Quote:
 Originally Posted by PSYMN 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
 butterfly_valve2.jpg001.jpg (89.6 KB, 32 views) butterfly_valve2.jpg002.jpg (84.2 KB, 29 views) butterfly_valve2.jpg003.jpg (94.9 KB, 37 views) butterfly_valve2.jpg004.jpg (55.5 KB, 23 views) butterfly_valve2.jpg005.jpg (91.6 KB, 25 views)

November 25, 2012, 03:12
#9
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,285
Blog Entries: 6
Rep Power: 43
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
 butterfly_valve3.jpg001.jpg (23.8 KB, 19 views) butterfly_valve3.jpg002.jpg (76.5 KB, 20 views) butterfly_valve3.jpg003.jpg (90.1 KB, 25 views) butterfly_valve3.jpg004.jpg (87.9 KB, 25 views)

Last edited by Far; November 25, 2012 at 05:05. Reason: spelling mistake

November 25, 2012, 07:12
#10
New Member

Join Date: Nov 2009
Location: Duisburg
Posts: 23
Rep Power: 8
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
 valve1.jpg (97.1 KB, 32 views) valve2.jpg (38.1 KB, 31 views)

November 25, 2012, 07:21
#11
New Member

Join Date: Nov 2009
Location: Duisburg
Posts: 23
Rep Power: 8
Quote:
 Originally Posted by BrolY 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,
Attached Images
 Geometry.jpg (14.9 KB, 25 views)

Last edited by snpradeep; November 25, 2012 at 07:30. Reason: apology.

 November 27, 2012, 11:21 #12 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 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

 November 27, 2012, 11:25 #13 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,285 Blog Entries: 6 Rep Power: 43 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.

 November 27, 2012, 13:07 #14 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 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

 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 ram Main CFD Forum 5 June 17, 2000 21:31 Francisco Saldarriaga Main CFD Forum 1 August 2, 1999 23:18 Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18 Tylor Xie Main CFD Forum 0 June 9, 1999 07:33 Roger Yang Main CFD Forum 11 February 11, 1999 17:53

All times are GMT -4. The time now is 22:50.