[smshin]

Domain Name : FLD inlet
Global Length = 2.5031E+00
Minimum Extent = 1.0000E+00
Maximum Extent = 1.0000E+01
Density = 9.8902E+02
Dynamic Viscosity = 5.7331E-04
Velocity = 9.5566E-06
Advection Time = 2.6193E+05
Reynolds Number = 4.1266E+01

+--------------------------------------------------------------------+
| ERROR #002100004 has occurred in subroutine Out_Scales_Flu. |
| Message: |
| The Reynolds number is outside of the range expected based on the |
| Option selected for the TURBULENCE MODEL. Check this setting, |
| the values of the properties, mesh scale, consistency of units |
| and solution values in the input file. Execution will proceed. |
+--------------------------------------------------------------------+


I would like to analyze a semicircular pipe with a radius of 1 mm.
The inlet mass flow rate is 0.02 kg/s, and the Reynolds number calculated by hand is about 20,000.
The calculation method in cfx seems to be different. This has caused post processing problems.
In cfx solver, the above error message is displayed. The calculated inlet velocities and Reynolds numbers are different in the solver. What is the problem?

[ghorrocks]

The message says error but it really is just a warning.

The solver estimates a Reynolds number by averaging fluid properties and velocity over the domain, and taking the cube root of the volume for the length scale. Obviously a Reynolds number based on these vague numbers are not going to match your calculations where you use carefully chosen parameters. So do not be concerned if your Re number does not match the solver reported Re number.

[Gert-Jan]

Originally Posted by smshin

Domain Name : FLD inlet
Global Length = 2.5031E+00
Minimum Extent = 1.0000E+00
Maximum Extent = 1.0000E+01
Density = 9.8902E+02
Dynamic Viscosity = 5.7331E-04
Velocity = 9.5566E-06
Advection Time = 2.6193E+05
Reynolds Number = 4.1266E+01

+--------------------------------------------------------------------+
| ERROR #002100004 has occurred in subroutine Out_Scales_Flu. |
| Message: |
| The Reynolds number is outside of the range expected based on the |
| Option selected for the TURBULENCE MODEL. Check this setting, |
| the values of the properties, mesh scale, consistency of units |
| and solution values in the input file. Execution will proceed. |
+--------------------------------------------------------------------+


I would like to analyze a semicircular pipe with a radius of 1 mm.
The inlet mass flow rate is 0.02 kg/s, and the Reynolds number calculated by hand is about 20,000.
The calculation method in cfx seems to be different. This has caused post processing problems.
In cfx solver, the above error message is displayed. The calculated inlet velocities and Reynolds numbers are different in the solver. What is the problem?

You are talking about a radius of 1 mm, but the length says 1 m and 10m. Also the inlet velocity is 1e-5 m/s.
So, I suspect you created your geometry in mm, and imported it as m? Check the ruler in the bottom of the screen.............
If so, go the Pre, select the imported mesh and scale it down by a uniform scale of .001.