# CHT. Cooled blade. Different time steps.

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

 December 11, 2008, 04:40 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.

 December 11, 2008, 20:16 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

 December 12, 2008, 04:23 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)

 December 14, 2008, 21:38 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

 December 26, 2008, 09:26 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?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 guido_88 FLUENT 4 August 30, 2012 14:49 skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48 lcw FLUENT 4 January 16, 2006 13:19 Sanjay Padhiar Main CFD Forum 1 March 31, 1999 12:32

All times are GMT -4. The time now is 20:36.