Fluent Meshing problem

57 Views
Last Post 12 December 2018
Topic Is Solved

sianov posted this 09 December 2018 - Last edited 09 December 2018

Hello everyone. I tried to make 3D mesh in Fluent Meshing of FS vehicle. Every time I made mesh and started calculations there was information turbulent viscosity ratio to 10e5 in X cells. In each iteration number of cells were increasing for few hundred to milions. I simplified model CAD few time but it didn't help.

I tried also to calculate flow in simple box but still was same problem. I meshed same simple box with standard Ansys Meshing and there wasn't any problem.

Have anyone idea what could be wrong?

#Permalink
0
0
0

5 Comments

Order By: Standard | Newest | Votes

Admin

kkanade posted this 10 December 2018

this is not problem of fluent meshing.

as i have not seen your model, here are few general guidelines.

please refine the mesh further.

make sure that you have min ortho quality greater than 0.1 when you check the mesh in fluent.

if quality is bad, please improve the mesh.

please reduce inlet velocity and check.

please change the input parameters for turbulence.

if this helps you, please mark this as 'is solution' to help others on forum.

#Permalink
1
0
0

Liked by

sianov posted this 10 December 2018 - Last edited 10 December 2018

Thanks for replay.

Mesh quality generated in Fluent Meshing.

Max skewness 0.7940125

Minimum Orthogonal Quality = 2.05987e-01

Maximum Aspect Ratio = 1.46347e+01

velocity = 14m/s

I tried Your sugestion and when I decrease inlet velocity number of cells where turbulent viscosity ratio is limited to 10e5 is decreasing. I set inlet velocity 0.5 m/s and there weren't problems with turbulent viscosity ratio.

Mesh quality generated in Ansys Meshing

Max skewness = 0.754

Minimum Orthogonal Quality = 2.06180e-01

Maximum Aspect Ratio = 1.56531e+01

velocity = 14m/s

In this case there isn't any problems with turbulent viscosity ratio.

I'm using k-epsilon model.

Any advices?

#Permalink
0
0
0

ANSYS

rwoolhou posted this 10 December 2018

Please can you post some images of what the model looks like (in line so ANSYS staff can view them) with a few dimensions. Also a few plots of velocity contours so we can see what's going on.

Viscosity ratio warnings can mean that you've got a poorly resolved flow (mesh quality is OK there just isn't enough of it), that the boundary conditions are unsuitable or the domain is very large.

#Permalink
0
0
0

sianov posted this 11 December 2018

Thanks for replay.

I discovered what was wrong. I set in Fluent Meshing unit of length mm. Basic unit of length in Fluent is m here is a problem. When dimension in Fluent meshing was 10 mm, in Fluent was 10m. I set unit of length m in Fluent Meshing and then everything was ok.