Very high or negative pressures
Dear All,
I am modeling a pipe with dynamic mesh. One end is a piston, the other end is an outlet/outflow. Case setup: k-epsilon incompressible: air density = 2.33 kg/m^3 = constant. Operating pressure = 265kPa at piston; also tried 0 Pa. I tried the open pipe end as outlet as well as outflow. The first step of the motion ends always with wrong static pressures. Next to piston they are very high (>1E+6). If the open end is an outflow, then the pressure there becomes negative. Please help me correct the errors in this case. |
*switch to pressure-outlet
*check your units (scale) *what kind of method are you using for moving mesh (layering/remeshing/...) display the grid while plotting the pressure, and check if the high pressures aren't linked with bad cells |
Hello mAx,
thank you for your time. * switched to pressure outlet, still calculated static/absolute pressure at piston is > 1E+7 * my pressure unit is Pa * I am using layering, it is a hex mesh on a rectangular pipe * equiangle/equivolume skew is < 0.2 |
*check the scale: grid/scale
*how fast is your piston moving? *do you see any discontinuity in the fluid domain (display pressure)? *does the fluid flows out? |
* grid/scale: all scales = 1, unit = [meter]
* piston moves with 32 m/s * no discontinuity: pressure is 265kPa at outlet and grows smoothly to 5E+7 at piston * mass flux at outlet converged to -8.5kg/s Pipe/duct has rectangular cross section, 0.3m x 0.1m, length ~20m |
post a picture with pressure and grid.
did you check the mesh motion? |
Yes, the mesh motion is fine.
If the time step is dt=1E-4, mass flux at outlet is -8.5kg/s, pressure at piston is 5E+7Pa If the time step is dt=1E-6, mass flux at outlet is -600kg/s, pressure at piston is 3E+11Pa This is totally bogus. Something seems to be conceptually wrong. |
disable the MDM, switch to steady solver.
Change your moving piston to massflow inlet and give the 8.5kg/s. Iterates and check the pressure distribution. are you working 2d or 3d? |
Apologies for the delayed reply.
Solution: start the simulation with ideal-gas on, run for sufficient number of time steps. Switch to incompressible. It works now. Many thanks, mAx for the useful analysis; it has helped me tackle the problem from many aspects. Cheers, -jpo |
All times are GMT -4. The time now is 16:00. |