# negative density when star cd>-power couple

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

 September 19, 2007, 09:13 negative density when star cd>-power couple #1 whitemelon Guest   Posts: n/a when star cd and gt power couple to solve the intake manifold, negative density exists at 1000rpm,time step is 0.5deg,no negative density at 6000rpm,time step is 1 deg.i don't know the reason,can everybody give me some suggestions?

 September 24, 2007, 07:53 Re: negative density when star cd>-power couple #2 whitemelon Guest   Posts: n/a who have experience in starcd and gtpower couple simulation?

 September 24, 2007, 09:20 Re: negative density when star cd>-power couple #3 Steve Guest   Posts: n/a GT-POWER is an explicit code. 0.5 degrees at 1000 rev/min is 3 times the timestep length of 1 degree at 6000 rev/min. This is why it's unstable.

 September 25, 2007, 09:34 Re: negative density when star cd>-power couple #4 whitemelon Guest   Posts: n/a steve,thanks a lot.could you give me some suggestions for the solution to the problems? just decrease the time step size?

 September 25, 2007, 09:39 Re: negative density when star cd>-power couple #5 Steve Guest   Posts: n/a You have to decrease the Courant number at the boundary. I have no idea how the GT-P coupling works, but I suspect (as with all couplings like this) you could either decrease your timestep or coarsen your mesh. They both have the same effect.

 September 26, 2007, 18:11 Re: negative density when star cd>-power couple #6 Kyle Guest   Posts: n/a Steve is right. Star/GTPower coupling is very sensitive to the courant number at the coupled boundaries. I had a mesh that would give me negtive densities with any timestep over .1 degrees. After I increased the length of the cells I extruded off for the runners to the boundaries, I can get away with .5 degree timesteps. This was at 1500 RPM. At your higher RPM, even though the actual timestep is smaller, it is more a of shock to the boundary cells when the intake port opens. Either increase the length of the cells near the boundary or decrease the timestep. Gamma suggested that I try a density function other than ideal gas, but that did not help me.

 September 26, 2007, 18:16 Re: negative density when star cd>-power couple #7 Kyle Guest   Posts: n/a Also, if you are getting negative densities in the first couple iterations, you may want to try and restart from a steady state solution. Run it steady with all the flow going out of the ports that are open at the start of the transient simulation, then just set the coupled run to do a standard restart from this .pst as initial conditions.

 September 27, 2007, 06:42 Re: negative density when star cd>-power couple #8 Steve Guest   Posts: n/a If the coupled simulation is being started from stationary, consistent conditions (no motion in 1D or 3D sections, constant P,T throughout) and is still crashing, you lose. No amount of fiddling with initial conditions will make it run at the step being used. It's often useful to know if you are wasting your time trying to get an inherently unstable simulation going.

 September 27, 2007, 07:10 Re: negative density when star cd>-power couple #9 whitemelon Guest   Posts: n/a i am calculating intake manifold from 1000rpm to 6000rpm,when speed over 3000rpm,the starcd and gt-power work well,the pipe dx=20mm.when engine speed below 3000rpm,the calculation goes well,but about 100 CA,you will find the CFD to gt (such as pressure,temperture,velocity),temperature is below 273K,after a while ,the calculation diverged.Now,i changged the dx=30mm in gt model,time step size =0.5 deg in starcd,it can works very well.

 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 Alena FLUENT 0 March 3, 2008 02:03 hosseini CFX 0 February 21, 2008 05:04 cfd_newbie FLUENT 1 December 10, 2007 01:53 whitemelon FLUENT 0 June 3, 2006 05:40 Le Dinh Vu Siemens 4 August 31, 2005 02:14

All times are GMT -4. The time now is 08:53.