Simple pipe flow - max velocity too low

Hello,

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.

Unable to find an attachment - read this blog

Find more posts tagged with

AcuSolve

English

Accepted answers

All comments

acupro

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.

Altair Forum User

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?

acupro

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.

Altair Forum User

Sorry for the delayed reply. It worked just as you said, thank you.