CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Best practice for transient simulations?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2010, 07:56
Default Best practice for transient simulations?
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Hi,

I'm going to be modelling a transient external aerodynamics flowfield. To start I made a mesh (in ICEM CFD) that I thought had reasonable element sizings and clusterings. But to make sure I do things correctly and accurately in CFX I have a few questions:

1. Initially, I shall run a steady-state simulation with this mesh as this will be needed as the initial conditions of the transient simulation. However, although the flowfield is transient (I do not know at this stage the frequency of the transient flowfield features) should I conduct a series of steady state simulations with ever increasing mesh resolutions to get a mesh independent result and thereby obtaining a mesh that I can be confident to return a good transient result?

2. Or should a mesh independent solution be obtained during the transient solution? However, I'm thinking that the mesh refinements could be depenedent upon the time. And in at this stage the mesh from the steady state solution would no be that important.

3. Once the mesh independence is assessed the time step indepenence must be conducted. Should this be conducted by refining the physical timestep or the transient timestep? I think it would be a long process if both had to be assessed.

I'd be interested in the process/sequence of these assessments that other people use to make sure that I get solution independent meshes and times for my transient simulations.

Thanks
siw is offline   Reply With Quote

Old   January 18, 2010, 17:55
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,656
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Is the transient flow caused by vortex shedding? If so then you will not get steady state simulations to converge. In this case the only use for steady state simulations is to use upwinding advection (which puts so much damping into it that it should converge but be quite inaccurate) to get an initial condition for the transient simulation.

So Q1 - No, it cannot be done for the reason I explain above.
Q2 - Yes, this is what is required.
Q3 - Yes. As you will only be doing a transient simulation you only have the transient simulation to determine. But it will have some coupling to the mesh - as the mesh resolves smaller features you will need a smaller timestep to resolve these smaller features. So when you change the mesh, scale the timestep to keep the Courant number about the same.
ghorrocks is offline   Reply With Quote

Old   January 19, 2010, 03:40
Default
  #3
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Glenn, thanks for your comments.

Yes, vortex shedding is occuring in a couple of places because of the geometry of the object in the flowfield.

I'll now have to find out what an apporopriate Courant number is (<= 1?) for this case and change the timestep accordingly as the as element size decreases. However, in the Courant equation would I use for delta_X the minimum element spacing in the entire domain, which possibly would be the first element height on the wall boundaries?
siw is offline   Reply With Quote

Old   January 19, 2010, 04:31
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,656
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No, you should establish what Courant number to use by a sensitivity analysis. You should be able to use a Courant number quite a bit higher than 1, but exactly how much higher you will have to determine. Then when you check other mesh sizes you can scale the timestep keeping the Courant number constant. Then it you want to be thorough you can check timestep size again as the best timestep size will probably have moved a bit.

Courant number is a variable available in the solver and post-processing. Use either the maximum Courant number or the RMS average Courant number.
ghorrocks is offline   Reply With Quote

Old   October 30, 2010, 00:30
Default
  #5
Member
 
Derwin Parkin
Join Date: Feb 2010
Posts: 30
Rep Power: 7
derz is on a distinguished road
Hi - a question about Courant number. When you say use either RMS or Maximum, what exactly do you mean? I'm running a sim at the moment, the RMS is 16, and the Max is 102. I read somewhere saying the Courant number should preferably not be in the 100s...does that mean Max or RMS?
derz is online now   Reply With Quote

Old   October 30, 2010, 05:45
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,656
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The maximum Courant number allowable is problem dependent, so general figures are useless. You have to establish what Courant number your simulation likes to run at by a sensitivity analysis.
ghorrocks 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
Swirling flow simulations Ugo FLUENT 19 July 16, 2012 15:59
Timestepping in two - phase Simulations using RSM challenger85 CFX 0 January 4, 2010 06:00
Modelling Airfoil Flow Best Practice Ian Main CFD Forum 0 October 3, 2007 07:19
who has ERCOFTAC Best Practice Guidelines ? sarah_ron FLUENT 1 September 27, 2004 07:17
URANS and Transient Simulations bob Main CFD Forum 0 October 1, 2003 03:54


All times are GMT -4. The time now is 23:28.