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

[ICEM] Very Different Length Scales

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 18, 2010, 09:29
Default Options...
  #21
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry, I missed your post from May 25th. Certainly it is possible to combine Hexa and tetra mesh... There is a tutorial about it (HVAC tutorial), and there are several more slides about it in the Tips and tricks presentation (I have posted the link on CFD Online a number of times, but don't recall it right now).

If you now want to hexa mesh the Far field, you can block it separately and then load both blockings at once (with all the geometry so the blocking has something to associate with). Then you can merge the two blocking files into one file (using the topology branch of the blocking tree), and then you can merge verts at the interface to sew the blocking together. Since you must merge vert with vert, you need a 1 to 1 correspondence that demands the same topology on both sides, at least for the interface. I think I covered this in the tips and tricks also, but if not, let me know and I can post some slides about it.

The downside to merging is that your index control gets really mixed up. It is workable, but awkward.

As I said before, for this model, it really wouldn't be difficult to just block the inside and outside all at once, but you have options.
PSYMN is offline   Reply With Quote

Old   June 18, 2010, 09:49
Default
  #22
Member
 
Join Date: Feb 2010
Posts: 50
Rep Power: 8
mannobot is on a distinguished road
Dear Simon,

I think blocking all at once will be possible but in the end I do not want to have the complete geometry within the same case file because this will result in too many cells. I would like to seperate both problems. The flow within the die and the flow at the outside of the die. Therefore I am now trying to setup a grid for the outside but I need exactly the same meshing at the face which do combine both parts because I think FLUENT does store the information at the center of the cell. Now I do have a split which passes through the entire domain because of the inlet. I could try to reblock the die and use index control to not let the split pass until the outlet and then use the match edges feature. But in that case I would have to mesh anything a second time and also the solver has to re-calculate. Therefore I am asking wether it is possible to add geometrical parts match blocking and then delete the old blocking. As I tried I was ask to merge and that resulted in a loss of the bunching information. Would you recommend to remesh the die so that I get a non splitted outlet block?
Or do you know that FLUENT is able to transfer that data neglecting the blocking?

Sincerely
mannobot is offline   Reply With Quote

Old   June 18, 2010, 11:40
Default Lots of options.
  #23
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You have lots of options... I am pretty sure you can map the output from the first case as an input to the second via interpolation that doesn't require the same mesh... Fluent is really good at that actually. Look up load mapping or ask on the Fluent Users Forum.

You could also block the entire model at once, but put the two halves in different volumes and output the volumes separately to Fluent.

You could merge the two blockings to make sure the faces matched, but then only output one of the volumes at a time...

If you know your topology at the interface (Ogrid or what ever), you could create some curves and points and associate each side separately to those geometry entities (like construction geometry)... Then make sure you have the same mesh distributions, etc. and you don't ever need to load both blockings to ensure that things will match... For example, if you created points where all the verts were on blocking A, then you could just copy those same interface points to Geometry B and associate blocking B with them... (to copy geometry between tetin files, Just turn off the other parts and File => Save Geometry => Only Visible. Then load the Geometry B tetin file (replace Geometry A) and then load/merge this Visible portion of Geometry A.)
PSYMN is offline   Reply With Quote

Old   June 19, 2010, 08:30
Default
  #24
Member
 
Join Date: Feb 2010
Posts: 50
Rep Power: 8
mannobot is on a distinguished road
Dear Simon,

these are really lots of options. I think I will first try to use FLUENT to interpolate. I will report the experience I gonna make.

Thank you very much.
mannobot is offline   Reply With Quote

Old   August 25, 2010, 10:32
Default
  #25
Member
 
Join Date: Feb 2010
Posts: 50
Rep Power: 8
mannobot is on a distinguished road
Hi everyone, Hi Simon,

I do have another problem..

Did change the configuration of the geometry. Now I have the problem that at a certain point two curves meet tangentially. There I do have just one edge but two curves. I tried to associate both curves with the single edge but that did not work out very well. I attached a picture of the situation. Do I have to change the model? But it can't be possible to adabt the geometry on ICEM. Is there a possibility to block that thing shown in the picture?

I am happy for any advice
Attached Images
File Type: png How to Block.png (17.0 KB, 10 views)
mannobot is offline   Reply With Quote

Old   August 25, 2010, 15:07
Default Wedges?
  #26
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
How do you feel about wedges?

I would block that with an Ogrid thru the cylinder and thru the block, then add wedges for the corners of the blocks. You would get prisms (Penta-6) elements in the cusp areas.

You would probably find that quality improves a little if your mesh jumps off the circle as it nears the wall, at least for the last element or so... You don't need to change the geometry, but maybe plan your geometry so that the opposite wedges (on either side of the cusp) don't actually meet, but rather have a couple extra splits thru the cylinder to keep them on either side of the theoretical meeting point.

I would block it out for you, but I am really swamped this week.

Simon
PSYMN is offline   Reply With Quote

Old   August 26, 2010, 07:05
Default
  #27
Member
 
Join Date: Feb 2010
Posts: 50
Rep Power: 8
mannobot is on a distinguished road
Thank you so much Simon..

Think wedges would be great but I am not sure how to apply. So far I just cut orthogonal to existing edges. I do start with a cube surrounding the entire model (3D bounding Box). Is it possible to just cut a wedge from an existing cube? If so, how would I allow ICEM to allow prisms?
To apply the O-Grid you have in mind, would I just need to create a 3D bounding box, block and from there choose the blocks and faces? Or would I first have to cut the wedges? Would you cut the main block where the cylinder and the cube meet? What is with the possible edges that will be created by that action. Would you associate those to the curves of the cylinder or to the curves of the cube?
How would I allow the mesh to jump near the wall?

Thank you so much in advance..

What do I have to do in case penetrating elements do appear where everything looks fine to me? May I neglect?

And a problem I do have with the settings. ICEM is running on several Computers. Every installation except of mine does allow by associating vertices and edges to neglect the apply button. What is wrong with my settings. I really enjoy that the association is accepted by chosing the respective point. Hope you understand.. Just want to chose vertice and point and go on with the next point without the need to apply..

Sincerely..
mannobot is offline   Reply With Quote

Old   June 21, 2011, 13:07
Default hi everybody
  #28
New Member
 
Olusogo fire
Join Date: Jun 2011
Posts: 9
Rep Power: 7
phire is on a distinguished road
I really need ur advice on this
I am try to model scour under pipelines lying on a seabed using FLUENT
I intend to use eulerian multiphase model which requires me to create two zones(water and soil).
I have used projection to split a surface into two under Design modeller to create the two faces.
The issue i have is that when i try to mesh the surrounding of the cylinder, the mesher; the mesh under the pipe is scattered because of the projection line that is there.
I have attached the picture of the mesh i got
pls i will appreciate any contribution
Attached Images
File Type: jpg FFF-6.1.jpg (86.8 KB, 10 views)
phire 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
Length Scales in Flame leaf Main CFD Forum 1 September 1, 2008 04:20
Getting Filter Length scales CFDtoy Main CFD Forum 0 February 15, 2008 12:53
Getting Filter Length scales CFDtoy Main CFD Forum 0 February 15, 2008 12:39
turbulence length scales T FLUENT 1 August 13, 2007 15:48
length scales in turbulence bajjal Main CFD Forum 9 May 24, 2006 02:19


All times are GMT -4. The time now is 06:45.