Inlet profile becomes uniform

bongbang · February 14, 2015, 15:18

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.

brunoc · February 14, 2015, 17:20

Free slip walls, maybe?

ghorrocks · February 14, 2015, 21:34

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.

bongbang · February 19, 2015, 11:46

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.

ghorrocks · February 19, 2015, 17:13

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.

bongbang · February 20, 2015, 09:33

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.

ghorrocks · February 21, 2015, 05:23

Did you look at Bruno's post right back at the start? Are you SURE you have not defined slip walls?

bongbang · February 21, 2015, 09:37

I'm positive. Velocity at the wall is indeed 0, as you can see below.

bongbang · February 21, 2015, 12:24

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.

ghorrocks · February 21, 2015, 23:49

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.

bongbang · February 22, 2015, 09:29

Okay, here there are. Your investigative effort is very much appreciated.

Output file.

ghost82 · February 22, 2015, 10:08

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?

ghorrocks · February 22, 2015, 19:01

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.

bongbang · February 23, 2015, 16:14

Many many thanks, Glenn. That was the problem.

February 14, 2015, 15:18	Inlet profile becomes uniform	#1
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	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.

February 19, 2015, 11:46	Same result even in steady case	#4
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	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.

February 21, 2015, 12:24	Works in Fluent!	#9
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	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.

February 22, 2015, 10:08		#12
ghost82 Senior Member Rick Join Date: Oct 2010 Posts: 1,016 Rep Power: 26	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!

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

February 14, 2015, 17:20		#2
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	Free slip walls, maybe?

February 14, 2015, 21:34		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,697 Rep Power: 143	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.

February 19, 2015, 17:13		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,697 Rep Power: 143	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.

February 20, 2015, 09:33		#6
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	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.

February 21, 2015, 05:23		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,697 Rep Power: 143	Did you look at Bruno's post right back at the start? Are you SURE you have not defined slip walls?

February 21, 2015, 09:37		#8
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	I'm positive. Velocity at the wall is indeed 0, as you can see below.

February 21, 2015, 23:49		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,697 Rep Power: 143	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.

February 22, 2015, 09:29		#11
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	Okay, here there are. Your investigative effort is very much appreciated. Output file.

February 22, 2015, 19:01		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,697 Rep Power: 143	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.

February 23, 2015, 16:14		#14
bongbang Member NC Join Date: Jan 2015 Posts: 49 Rep Power: 11	Many many thanks, Glenn. That was the problem.

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 11:49
turbulent jet simulation	antonio_ing	OpenFOAM Running, Solving & CFD	5	September 16, 2010 02:31