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

CHT. Cooled blade. Different time steps.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 11, 2008, 03:40
Default CHT. Cooled blade. Different time steps.
  #1
Georg
Guest
 
Posts: n/a
Hi all, I model cooled turbine blade. There are two fluid domains (flows inside and outside blade) and solid domain with heat conductivity. When I solve steady-state problem I use three time scales (individual for every domain) and have a good convergence and calculation time. When I model transient I obligated to use only one time step for all domains and I choose smallest time step (estimated for fast flow outside blade). Solid domain is slow heated so time duration is big enough. Therefore total amount of time steps is enormous and calculation time is huge! Has CFX any ways to set different time steps for various domains? Do you know any approaches to reduce calculation time? May be submodeling or FSI (CFX for outside flow and ANSYS Thermal for solid and outside flow)? Thanks a lot for your advices.

  Reply With Quote

Old   December 11, 2008, 19:16
Default Re: CHT. Cooled blade. Different time steps.
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Yes, CFX can do different timesteps for different domains in steady-state simulations. You want to set the "solid timescale factor" CCL object. This is a standard trick to accelerate CHT simulations.

Glenn Horrocks
  Reply With Quote

Old   December 12, 2008, 03:23
Default Re: CHT. Cooled blade. Different time steps.
  #3
Georg
Guest
 
Posts: n/a
Thanks Glenn. But I need accelerate Transient simulation (please see first post)
  Reply With Quote

Old   December 14, 2008, 20:38
Default Re: CHT. Cooled blade. Different time steps.
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Some comments:

1) In the solid the only equation to be solved is temperature and it much easier than fluid domains as the equation is linear and there is only one variable (fluid domains usually have 7 variables of more). This means that unless you have a huge amount of mesh points the solid domain does not add much computational load to the simulation.

2) Can the simulation be decoupled somehow? Maybe get heat transfer coefficients from a fluid simulation and put them as boundaries for a heat transfer simulation?

3) I guess the fluid flow sorts itself out quickly but the solid stuff takes much longer. You can solve the coupled thing until the fluid has reached steady state, then turn the fluids solver off and just continue with the heat solver. This will evolve the fluid/solid system in temperature but will not couple back to the fluid system. If the coupling is weak you could just turn the fluids solver on for just a short time and off for a while. Use the expert parameter "solve fluids = t or f" to do this.

Glenn Horrocks
  Reply With Quote

Old   December 26, 2008, 08:26
Default Re: CHT. Cooled blade. Different time steps.
  #5
Igor-a
Guest
 
Posts: n/a
Hi Georg! What kind of interface (for fluid-solid surface) do you use in your model?
  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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Time step size, number of time steps and max iterations per time step guido_88 FLUENT 4 August 30, 2012 14:49
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48
A variable expressing time steps in UDF? lcw FLUENT 4 January 16, 2006 12:19
unsteady calcs in FLUENT Sanjay Padhiar Main CFD Forum 1 March 31, 1999 11:32


All times are GMT -4. The time now is 00:14.