CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Inlet profile becomes uniform

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 14, 2015, 16:18
Default Inlet profile becomes uniform
  #1
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
It seems I've succeeded in applying a time-varying BC via profile data, but the profile becomes uniform as as it travels through an empty cylinder (modeled as a 1/6 axisymmetric wedge). I don't have enough experience to have a sense of what's wrong, but surely somebody doues? Something to do with the domain setup?

In the picture, the left edge is the center and the right edge, the wall. Thanks.

bongbang is offline   Reply With Quote

Old   February 14, 2015, 18:20
Default
  #2
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Free slip walls, maybe?
brunoc is offline   Reply With Quote

Old   February 14, 2015, 22:34
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Could also be:
* the scale is wrong (metres not mm)
* The fluid properties are wrong
* The input velocity is wrong
* The flow at this condition has a very thin boundary layer, not the thick boundary layer you prescribe on the inlet.
ghorrocks is offline   Reply With Quote

Old   February 19, 2015, 12:46
Default Same result even in steady case
  #4
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
I applied the simplest of test cases, a pressure driven flow in a tube with a parabolic profile (input as profile data, not CEL), and got the same result. I'm new at this, so I must've done something wrong, but I don't know what. The expected correct result, of course, is a fully developed flow with the same profile at the inlet as at the outlet and everywhere in between.

The material is water. The geometry is 1/6 of a tube, with symmetry conditions applied to the two sides of the wedge. The no slip condition at the wall does hold, as you will see a thin blue line running all the way along the wall.

Now that I think about it, I suspect that my outlet boundary condition is at fault. I just followed the tutorials I've seen and set "Average Static Pressure" to 0 to the reference pressure (which I didn't change from the default). I don't understand why CFX insists on some type of condition. Why can't outlet be set to "outflow" as in Fluent? How can I fix this? Thank you.

bongbang is offline   Reply With Quote

Old   February 19, 2015, 18:13
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If I look at your water model I guess the diamater is about 6mm, the input velocity around 1m/speak so let's say an average velocity of 0.5m/s, and for water density is 10000 kg/m3 and viscosity is 8.9e-4 Pas. That gives a Re number of about 3500. At this Re I would expect the flow to start going turbulent and so you should have boundary layers forming. In other words your Re is too high to have a parabolic profile.

If you run the flow at a low Re (maybe 10) and you should get a good parabolic profile.
ghorrocks is offline   Reply With Quote

Old   February 20, 2015, 10:33
Default
  #6
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
Thanks, ghorrocks, you made a good point, but I'm afraid it didn't do it for me. I divide the inlet velocity by 1000 and roughly the same thing. The flow just becomes uniform even faster, which I suppose is internally consistent.

What else should I look at? Outlet condition (0 avg static pressure relative to reference)? Initial conditions (auto)? I got even more bizarre results when the initial condition is given the parabola profile as well.

bongbang is offline   Reply With Quote

Old   February 21, 2015, 06:23
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Did you look at Bruno's post right back at the start? Are you SURE you have not defined slip walls?
ghorrocks is offline   Reply With Quote

Old   February 21, 2015, 10:37
Default
  #8
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
I'm positive. Velocity at the wall is indeed 0, as you can see below.

bongbang is offline   Reply With Quote

Old   February 21, 2015, 13:24
Default Works in Fluent!
  #9
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
For what it's worth, Fluent solves the same case without trouble. The only thing that's different is the outlet is set to "outflow," an option that isn't available in CFX.

bongbang is offline   Reply With Quote

Old   February 22, 2015, 00:49
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Pleas upload your output file and an image of your mesh.

This is a trivial simulation and CFX can model it fine. There will be a mistake on the setup which is causing this. The outlet boundary condition is not the problem, the effect happens a long way away from the outlet.
ghorrocks is offline   Reply With Quote

Old   February 22, 2015, 10:29
Default
  #11
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
Okay, here there are. Your investigative effort is very much appreciated.

Output file.

bongbang is offline   Reply With Quote

Old   February 22, 2015, 11:08
Default
  #12
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Hi,
I'm not a CFX user (fluent user), but I think message n. 5 is the key.
When in fluent you set the outflow boundary condition you are imposing a zero diffusion flux and so a fully developed flow at exit (fluent doesn't care if this is true or not, it applyes your bc).
But are you sure you have a fully developed flow at inlet which preserves on exit?
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   February 22, 2015, 20:01
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I have set up a version of this myself and had a play. I am pretty sure I know what is going on now.

You are using a k-e turbulence model. This is a high Re turb model and not suitable for low Re applications. You will never get a parabolic velocity distribution with k-e. When I run my model with k-e turb model I get similar results to you where the parabolic inlet distribution quickly disappears.

Parabolic velocity distributions are a laminar flow thing so you will need to use a laminar flow model. When I use a laminar flow model I get the parabolic velocity distribution going the entire length of the domain as expected.

You might also consider turbulence models more suited to low Re flows such as SST. Its results are intermediate between the k-e and laminar models.

So this problem appears to be incorrect selection of turbulence model. It is nothing to do with the outlet boundary.
ghorrocks is offline   Reply With Quote

Old   February 23, 2015, 17:14
Default
  #14
Member
 
NC
Join Date: Jan 2015
Posts: 49
Rep Power: 2
bongbang is on a distinguished road
Many many thanks, Glenn. That was the problem.
bongbang is offline   Reply With Quote

Reply

Tags
boundary condition, transient analysis

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
boundary conditions for simpleFoam calculation foam_noob OpenFOAM Running, Solving & CFD 8 July 1, 2015 08:07
Pulsatile profile at inlet Josyula Fluent UDF and Scheme Programming 4 May 6, 2012 10:09
singularity? mihaipruna OpenFOAM Running, Solving & CFD 5 April 24, 2012 17:18
Problem with rhoSimpleFoam : exploding enthalpy and density at the walls david39 OpenFOAM Running, Solving & CFD 6 January 18, 2011 12:49
turbulent jet simulation antonio_ing OpenFOAM Running, Solving & CFD 5 September 16, 2010 02:31


All times are GMT -4. The time now is 01:14.