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

Local Initial Conditions

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 25, 2019, 01:29
Default Local Initial Conditions
  #1
New Member
 
Join Date: Mar 2019
Posts: 1
Rep Power: 0
Flowmax is on a distinguished road
I am trying to create a transient simulation in which different parts of the mesh will be initialized with different initial conditions. Specifically, one area is to have a high initial temperature and pressure, while the rest of the mesh should be at a lower temperature and pressure, before the two eventually equalize as gas discharges from the high pressure area. There should be no inlet, but there will be an outlet to prevent pressure buildup in the low pressure area. From what I have seen, the only way to have multiple areas with different initial conditions is to have separate physics continua, but this doesn't seem to allow for gas to flow from one area into the other. The image I have attached shows my domain. The cylinder highlighted by the red box is the high pressure area, the gas should then flow out through the narrow tube into the larger cylindrical area.
Attached Images
File Type: jpg Domain.jpg (29.6 KB, 7 views)
Flowmax is offline   Reply With Quote

Old   March 25, 2019, 12:16
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 776
Rep Power: 12
fluid23 is on a distinguished road
I have posed this question (on a very different application) to our star-ccm support engineer before and was told that it was a fool's errand. For my application, the best thing was to use the grid sequencing function. However it requires that you use a coupled solver. If you have coupled implicit solver enabled you can go to Solvers > Coupled Implicit > Expert Initialization > Grid Sequencing to enable/configure.

That being said, I don't think that will work for the equalization problem you described. It will try to solve the boundary conditions and march your solution along rather than pressurize one chamber vs the other.

Just spit balling here, but one thing that comes to mind that you might try, and I have NO idea if this will actually work, is to place a porous baffle between the two regions and assign a restriction which is very very high (effectively infinite within the limits of the software) and then changes over time (probably not instantly) to zero allowing the high p/T flow to move past. That way your boundary conditions can set the conditions in the separate areas before the 'wall' between them 'disappears'.

Can you explain what it is you are trying to get out of this model? The community may be able to offer suggestions for a better geometry/setup.
fluid23 is offline   Reply With Quote

Old   March 25, 2019, 20:52
Default
  #3
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,190
Rep Power: 18
me3840 is on a distinguished road
You can easily specify different initial conditions in different areas of the mesh by using field functions. Your geometry would lend itself well to using a cylindrical coordinate system. You would then specify different values of pressure and temperature for varying axial position.

I don't really see anything foolish about the setup, it seems logical to me. Since it depends heavily on getting the initial transients resolved the timestep will have to be quite small in the beginning.
me3840 is offline   Reply With Quote

Old   March 26, 2019, 10:07
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,571
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
1) Field functions if you can come up with the appropriate boolean logic

2) csv tables and/or a data mapper into a field function
3) again data mappers but utilizing shapes to in combination with field functions to map everything into a new field function. This is quite convoluted. The easiest way is to do a simple field function such that T=low for x< number and T = high for x > number etc.


Quote:
Originally Posted by fluid23 View Post
I have posed this question (on a very different application) to our star-ccm support engineer before and was told that it was a fool's errand. For my application, the best thing was to use the grid sequencing function. However it requires that you use a coupled solver. If you have coupled implicit solver enabled you can go to Solvers > Coupled Implicit > Expert Initialization > Grid Sequencing to enable/configure.

That being said, I don't think that will work for the equalization problem you described. It will try to solve the boundary conditions and march your solution along rather than pressurize one chamber vs the other.

Just spit balling here, but one thing that comes to mind that you might try, and I have NO idea if this will actually work, is to place a porous baffle between the two regions and assign a restriction which is very very high (effectively infinite within the limits of the software) and then changes over time (probably not instantly) to zero allowing the high p/T flow to move past. That way your boundary conditions can set the conditions in the separate areas before the 'wall' between them 'disappears'.

Can you explain what it is you are trying to get out of this model? The community may be able to offer suggestions for a better geometry/setup.

ummm what? This is a very practical question of how to initialize a non-uniform field. What does grid sequencing and porous baffles have to do with initialization? smh
LuckyTran is offline   Reply With Quote

Old   March 26, 2019, 19:40
Default
  #5
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,190
Rep Power: 18
me3840 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
2) csv tables and/or a data mapper into a field function

While using a table by itself can be used to initialize a domain, I would strongly recommend against doing so. The reason is that tables in STAR are not parallelized; each process gets a copy of the table. So if your table is large (say, the size of the volume mesh) you would be storing one copy of the table for each parallel partition in memory, which is often very expensive.

Fortunately the data mappers are an excellent alternative which are implemented in a parallel fashion, and there's even a table data mapper. Just remember to delete the table if you choose to use it (and if your table is large).
me3840 is offline   Reply With Quote

Reply

Tags
initial condition, initial conditions, transient, transient 3d

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
courant number increases to rather large values 6863523 OpenFOAM Running, Solving & CFD 21 November 10, 2019 11:14
Segmentation fault when using reactingFOAM for Fluids Tommy Floessner OpenFOAM Running, Solving & CFD 4 April 22, 2018 13:30
Compressor Simulation using rhoPimpleDyMFoam Jetfire OpenFOAM Running, Solving & CFD 107 December 9, 2014 14:38
Help for the small implementation in turbulence model shipman OpenFOAM Programming & Development 25 March 19, 2014 11:08
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 19:32.