Simple pipe flow - max velocity too low
Altair EmployeeHello,
I'm currently examining the results of a simple pipe flow case and comparing several solvers. One of the test cases is a simple pipe flow with a mean inflow velocity of 0.1m/s and an outlet pressure of 0.0Pa. The pipe is 0.1m in diameter and 1m in length, the fluid is an oil with a density of 900kg/m^3 and a dynamic viscosity of 0.1Pa*s. The resulting max. velocity should be 0.2m/s, but it only reaches 0.1893m/s. The exact same model and mesh calculated with Abaqus 6.14-3 reaches 0.1984m/s, which is a lot closer to the target value. The pressures differ as well between both solvers. I tried a steady state and transient analysis type (10 seconds in Acusolve and Abaqus), but no difference in Acusolve. I've attached the model and results and I'd appreciate any help leading to a better result. I deem Acusolve to be more advanced in CFD than Abaqus, so the error is probably my model setup.
PS: Somehow, Hyperview only shows the last time step and I'm unable to create an animation. How come? I didn't disable surface outputs.
Answers
-
The difference you're seeing is likely due to the Inlet boundary condition. The 'velocity' type creates essentially a constant /plug velocity at the inlet, but with zeros at the wall boundary. This also creates a bit of a problem with pressure at the edges of the boundary. You may need a longer pipe for the flow to develop completely.
If you switch to average-velocity for the inlet, the results should be closer to what you expect, even for steady-state with the default 1.e10 time increment. This type creates a profile at the inlet, rather than a constant velocity.
If you want to animate a transient, you need to request more frequent nodal output.
0 -
You're right, with an average velocity of 0.1m/s, the resulting radial velocity profile is exactly as to be expected. Although now the velocity profile is also developed at the inlet, as you mentioned. Is there a possibility to get a correct result with the profile developing along the pipe axis or is this the nature of Acusolve?
0 -
If you revert back to velocity = 0.1 m/s, set the precedence to 2 on the inlet Simple Boundary condition. This should force the 'edge' nodes also to 0.1 m/s instead of 0. (With 0.0 velocity at the edge where it meets the wall, the average velocity is a little below 0.1.) You may also need to increase the length of the pipe for it to develop fully.
0 -
Sorry for the delayed reply. It worked just as you said, thank you.
0