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?

who have experience in starcd and gtpower couple simulation?

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.

steve,thanks a lot.could you give me some suggestions for the solution to the problems? just decrease the time step size?

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.

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.

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.

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.

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.