CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

ICEM Boundary Layer & CFX Wall Roughness Problem

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   August 23, 2021, 10:23
Question ICEM Boundary Layer & CFX Wall Roughness Problem
New Member
Join Date: Aug 2021
Posts: 5
Rep Power: 4
Puschkin is on a distinguished road
Hello dear CFD Online Members!

Currently I'm facing a problem regarding the boundary layer mesh generation in ICEM. For my case I'm simulating a simle CD-Nozzle as a 2.5d Problem. Therefore I did the blocking, created a hexa-pre-mesh, converted it to unstruct mesh and finaly extruded it to 4.

I use CFX to simulate my case and everything works like it should as long as I work with a smooth wall BC. I pre-calculated the wall distance and my y+ value (I'm using the SST-Model) is in the desired range of 0.4-0.7 over the whole domain with a "first layer thickness"/spacing of 1e-7 [m]. Everything converges fine and the results are very promising.

As soon as I add a wall roughness (3 micron) the y+ value goes through the roof. I get values of up to 50 and I'm not able to reduce the y+ value properly.

What I tried to overcome the problem:

Different "first layer thickness"/spacings (lower and higher than 1e-7 [m])
Different growth ratios between 1.05 and 1.2.

Lowering the "first layer thickness"/spacing helped to reduce the max. y+ value to 33 but min. y+ is still above 10. The problem now is, that as soon as I try to lower the "first layer thickness"/spacing any further, the mesh in the first layer(s) is getting distorted (see attached picture) and the extrusion of the unstructed mesh in the future steps fails.


So currently I'm limited regarding the "first layer thickness"/spacing (min spacing 2e-8 [m] before the problems occur). Since I'm trying to investigate the heatflux over the nozzle I would like to resolve the boundary layer correctly.

I read the manual of ICEM and ANSYS CFX and also the modeling guide and I'm aware of how ANSYS CFX models the wall roughness.

But sadly I'm currently out of ideas.
Maybe someone experienced a similar problem.
Any help would be appreciated!

Thank you!
Puschkin is offline   Reply With Quote

Old   August 23, 2021, 17:47
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quoting the CFX Solver Modelling Guide (section 4.2.4): "For rough walls, the logarithmic profile exists, but moves closer to the wall.", in other words, a given mesh will have a smaller y+ value with rough walls activated compared to smooth walls.

In addition, I think you need to consider whether integrating to the wall (ie, using a mesh with y+ ~1) is appropriate for a rough wall model. The turbulence models have wall functions, so why not use them - then a y+ ~1 mesh is not required. In addition, as the roughness you are modelling is likely larger than your first few element sizes you need to consider whether your mesh has got too fine.

Wobbly prism mesh - I agree, I also find that the mesh smoothing in ICEM can sometimes lead to wobbly mesh like what you show. Sometimes I get better results by turning prism mesh smoothing off and remeshing. Alternately, try a different prism mesh smoothing algorithm.
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 24, 2021, 02:56
Senior Member
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
Alternatively, take a mesh that works fine and then in 'Edit mesh', split your inflation layer. As a result, the mesh won't get distorted.
Gert-Jan is offline   Reply With Quote


boundary layer thickness, cfx, icem, yplus

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Radiation in semi-transparent media with surface-to-surface model? mpeppels CFX 11 August 22, 2019 07:30
Multiphase flow - incorrect velocity on inlet Mike_Tom CFX 6 September 29, 2016 01:27
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 05:15
Very technical question about solving wall boundary layer ... jlb001 FLUENT 6 December 27, 2014 05:56
natural convection mehrdadeng CFX 10 February 25, 2011 05:25

All times are GMT -4. The time now is 07:39.