CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Multi Region CHT Simulation

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

Like Tree3Likes
  • 1 Post By ashokac7
  • 1 Post By cwl
  • 1 Post By pavko718

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 14, 2020, 03:43
Unhappy Multi Region CHT Simulation
  #1
New Member
 
akarfirath's Avatar
 
gago
Join Date: Jul 2019
Location: Turkey
Posts: 8
Rep Power: 3
akarfirath is on a distinguished road
Hello everybody. I am trying to simulate CHT phenomena which has got solid parts, liquid domain with boiling and also gas flow. I had a assembly of solid parts and I need to extract the volumes of gas and liquid in STAR CCM+. However operation>extract volume command is very sensitive to geometry. And generally ends up with "Can not find topology....." error message. I tried also Surface Wrapper Tool but in that case I had non conformal interfaces at where I have very thin sections and details which leads to poor accuracy in CHT simulations.
Is there any body who worked with this kind of CHT simulations and performed the preparation of the volumes in STAR CCM+? I would be appreciate if you can share your experience with me for this painfull task
akarfirath is offline   Reply With Quote

Old   January 21, 2020, 05:19
Smile
  #2
Senior Member
 
Ashok Chaudhari
Join Date: Aug 2016
Location: Pune, India
Posts: 243
Rep Power: 6
ashokac7 is on a distinguished road
Send a message via Skype™ to ashokac7
Quote:
Originally Posted by akarfirath View Post
Hello everybody. I am trying to simulate CHT phenomena which has got solid parts, liquid domain with boiling and also gas flow. I had a assembly of solid parts and I need to extract the volumes of gas and liquid in STAR CCM+. However operation>extract volume command is very sensitive to geometry. And generally ends up with "Can not find topology....." error message. I tried also Surface Wrapper Tool but in that case I had non conformal interfaces at where I have very thin sections and details which leads to poor accuracy in CHT simulations.
Is there any body who worked with this kind of CHT simulations and performed the preparation of the volumes in STAR CCM+? I would be appreciate if you can share your experience with me for this painfull task
Yeah!! It could take days for geometry preparation itself. Take solid parts, clean one by one, even intersecting faces are bad during volume extraction. Remove all the red patches for each geometry.
Then create multi-part interfaces, check for intersecting faces during interface formation too. It is better to combine 2 parts with same material as a single part if possible.
Exclude small parts wherever possible. Like Nuts and bolts.
For interface formation, take 2 parts at time, and don't use imprint all command, rather imprint each pair, and manually check each pair.
when interfaces between all these solid parts are formed, check for all the solid parts in single surface repair. everything should appear zero here.
Then combine all parts, delete interfaces, and close all the openings for fluid volume.
Now split by surface topology (there will be manifold edges between each part and also between new filled holes, but don't worry)
After splitting you should get solids as well as fluid volumes and also interfaces between each parts in contacts.
It is quite complicated, but keep patience, the end result is quite satisfying.
akarfirath likes this.
ashokac7 is offline   Reply With Quote

Old   January 21, 2020, 07:41
Default
  #3
cwl
Senior Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 183
Rep Power: 10
cwl is on a distinguished road
Send a message via Skype™ to cwl
Quote:
Originally Posted by ashokac7 View Post
Then combine all parts, delete interfaces, and close all the openings for fluid volume.
Now split by surface topology (there will be manifold edges between each part and also between new filled holes, but don't worry)
After splitting you should get solids as well as fluid volumes and also interfaces between each parts in contacts.
The thing is that - this way breaks the idea of Parts Operations pipeline.

Since Extract Volume is a fussy operation - for simplicity you could use Extract Internal Volume in 3D-CAD module.

In general it is possible to do that with Extact Volume operation,one just needs to practice first on simple cases and to learn dealing with the Imprint operation, which actually can work at least in three ways.
akarfirath likes this.
cwl is offline   Reply With Quote

Old   January 24, 2020, 03:17
Default
  #4
New Member
 
akarfirath's Avatar
 
gago
Join Date: Jul 2019
Location: Turkey
Posts: 8
Rep Power: 3
akarfirath is on a distinguished road
Thank you very much for your answer. I am following your reccomendations right now and it seems like it working. but when you have 100 different parts, this task become very sensitive to any small mistakes could be happen during work.
akarfirath is offline   Reply With Quote

Old   January 24, 2020, 14:19
Default Extract Volume
  #5
New Member
 
PK
Join Date: Oct 2010
Posts: 9
Rep Power: 11
pavko718 is on a distinguished road
Parts which enclose the volume you are attempting to extract must be topologically connected and completely enclose the volume of interest. If there are openings, they must be closed with patches or solid parts. One way to do that is to imprint parts together, check that everything imprinted correctly and then extract the volume. The volume extraction will create the part-to-part contacts which will be used to automatically create interfaces when parts are assigned to regions. The method described earlier (slit-by-topology) is another way to do it, but has many disadvantages: it's not a pipeline operation, part names will be lost (a big deal for 100 parts), and this method can become tedious when part connections are complex. For some difficult to imprint assemblies it can be the only way, but is usually a last resort. It's best to improve your existing parts in order to then imprint them using mesh operations, several if necessary, using various tolerances.
akarfirath likes this.
pavko718 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How I can introduce my power heat (W) in chtMultiRegionFoam? aminem OpenFOAM Pre-Processing 32 August 29, 2019 02:23
Some questions about a multi region case run in parallel zfaraday OpenFOAM Running, Solving & CFD 5 February 23, 2017 10:25
Thermal simulation of multi chip module with components phurba Main CFD Forum 1 July 26, 2015 13:34
Unstabil Simulation with chtMultiRegionFoam mbay101 OpenFOAM Running, Solving & CFD 13 December 28, 2013 13:12
[Gmsh] Import gmsh msh to Foam adorean OpenFOAM Meshing & Mesh Conversion 24 April 27, 2005 08:19


All times are GMT -4. The time now is 05:32.