reversed flow (backflow)

Table of Contents

• 1. Reverse flow   reversed_flow
  • 1.1. reasons
  • 1.2. solutions

1 Reverse flow   reversed_flow

It is common to encounter the regions of reversed flow at the initial stages of the simulation – This is normal.

However, if the “reversed flow” warnings do not disappear as the simulation progresses, then one needs to address the issue and move the outlet boundaries to a location where the inflow is no longer encountered.

Normally, it has to do with the outlet boundary condition.

if you were to use the "pressure outlet" boundary condition at the outlet, your outlet must be set far away from the object of interest.

In Fluent, I normally use the " outflow" boundary condition at the outlet and it does not give me reverse flow.

1.1 reasons

It is virtually impossible to prescribe correct values for varying turbulence characteristics, temperature and species concentrations in those cells where the backflow occurs.

• The number of such “backflow” cells might vary from one iteration to another,

and any discontinuity in calculated turbulence, species and temperature values for the neighbouring “outflow” and “inflow” cells is very likely to have an adverse effect on convergence.

• The accuracy of the solution can also be affected, especially if the area of interest is located close to the outlet with the “backflow”.

1.2 solutions

> if vortex formation/recirculation of flow near an outlet boundary, 1.2.

> check the mesh quality, improve it.

> use higher order scheme

> At last reduce the relaxation factor if necessary.

• At preprocessor (mesh generation) – too costly and inconvenient.
• Directly in ANSYS Fluent by extruding the outlet boundaries.

Calculation steps:

• Set up the model and calculate a solution on the initial mesh
• Please write the interpolation file first.
• Close the existing Fluent session.
• Open a new Fluent session and read the case file only.
• Perform 1.2
• Check the new zones and ensure that the prescribed outlet boundary conditions are set and named consistently.
• Initialise the flow.
• Read in the interpolation file.
• Continue simulation.

• The original data file cannot be read onto the new mesh.
• The new case file need to be initialised.
• Old data can still be recycled and used again by interpolation:

 file interpolate read-data original_ip_file_name.ip

Mesh/modify-zones/extrude-face-zone-delta 
#specify the face zone id/name i.e. inlet boundary name or zone ID 
distance delta 1 0.2[1]
#first extrusion layer edge length
distance delta 2 0.25 
distance delta 3 0.3 
distance delta 4 
#press “Enter” once a sufficient outlet section has been built[2]***. 

[1] − The offset value does not need to be 0.2 and should be equal to the typical cell edge length close to the original outlet [2] – total extrude layers, 3 cells. To minimise the amount of cells an expansion ratio of 1.2 can be used

1. Reference
   
   • 5.9.8. Extruding Face Zones, user guide
   • File “prevent backflow at outlet.fss”
2. Note:
   
   • This text command is not available in the parallel version of ANSYS Fluent.

   extrusion is not possible from boundary face zones that have hanging nodes.

   • Extruding face zones is not allowed on polygonal face zones.
   • Extruding face zones is only allowed in the 3D version of ANSYS Fluent.
3. outlet Extrusion error
   

   Problem description:

   • mesh/modify-zones/extrude-face-zone-delta
   • Face zone id/name [] 27 #outlet face zone
   • Distance delta(1) [()] 0.1
   • Distance delta(2) [()]
   • Extrude face zone? [yes]
   • Warning: the base thread has multiple adjacent threads!
   • Please separate the extruded side threads manually, and set the boundary condition accordingly.
   • Error: received a fatal signal (Segmentation fault).

Created: 2018-06-24 Sun 15:55

Validate