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

CFD-ACE laminar flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 10, 2005, 17:38
Default CFD-ACE laminar flow
  #1
Mahesh
Guest
 
Posts: n/a
Hi, I am trying to simulate laminar flow in a pipe using CFD-ACE. The boundary conditions are 1atm for outlet and 1atm+100Pa at the inlet. The velocity conditions are kept zero. The initial condition for the fluid is kept at 1 atm pressure with 0 velocity. The results for velocity and pressure in the pipe are correct but I see no entrance region. Could anyone please explain why this is happening? Thank you Mahesh
  Reply With Quote

Old   January 10, 2005, 22:05
Default Re: CFD-ACE laminar flow
  #2
Jim_Park
Guest
 
Posts: n/a
I've had a similar experience in the past. I forgot to impose the no-slip velocity condition on the pipe walls, or I specified the viscosity to be zero.

Easy to do. Don't know if YOU did it.
  Reply With Quote

Old   January 11, 2005, 15:20
Default Re: CFD-ACE laminar flow
  #3
Mahesh
Guest
 
Posts: n/a
Hi Jim, Thank you for your reply. I assigned viscosity to 0.000855 Kg/ms which corresponds to water. How do i assign no slip boundary condition for the walls?....presently all walls are at 0 velocity. I get an entrance region if i specify fixed velocity BC for inlet and fixed pressure for outlet....but here i need to specify inlet pressure too. Since this is like providing redundant information, i was trying to just specify only the pressure at the inlet and outlet. Please reply, Mahesh
  Reply With Quote

Old   January 11, 2005, 20:53
Default Re: CFD-ACE laminar flow
  #4
Jim_Park
Guest
 
Posts: n/a
Mahesh,

No slip and zero velocity at the boundary are the same thing for your problem. So both my guesses were wrong. Good!

Something to try:

Specify uniform velocity across the inlet - call it Uo. In a laminar tube flow the calculated pressure should be constant across the inlet, so let the solution find that value for you, po.

Likely po will not be the inlet value you want. So change Uo to a different value, U1. Then calculate the inlet pressure p1.

Repeat until selecting inlet velocity Un yields the inlet pressure that you wish for the problem.

Without knowing something about the code (besides its name!), that's my best shot at solving your problem.

Good luck!
  Reply With Quote

Old   January 12, 2005, 10:22
Default Re: CFD-ACE laminar flow
  #5
MG
Guest
 
Posts: n/a
If your BCs are correct (I assume they are), then next thing you want to check is the Re number. If it's too small, you'll get (very) small entrance region.
  Reply With Quote

Old   January 12, 2005, 13:40
Default Re: CFD-ACE laminar flow
  #6
Mahesh
Guest
 
Posts: n/a
Hi Jim, Well, thats exactly what i tried after mailing you. When I worte my last mail, i thought that there cannot be an entrance region until I specify a uniform velocity condition. The interesting thing is that even if I specify a pressure value when I mention a uniform velocity profile the software ignores that value and calculates the inlet pressure based on the given velocity and outlet pressure (which i fixed for the outlet). On the other hand when I give constant pressure at both the BCs it doesnt assume a uniform velocity profile because of which there is no entrance region. I guess I have understood it right. It is very frustrating to use a BLACK BOX :-D Anyways, is there any way to provide a uniform velocity profile by giving values only for pressure gradient? I tried 0 velocity and 10Pa pr.gradient but it shows no flow at all (thats obvious afterall)

Thank you very much, Mahesh
  Reply With Quote

Old   January 12, 2005, 13:43
Default Re: CFD-ACE laminar flow
  #7
Mahesh
Guest
 
Posts: n/a
Hi MG, I had verified the Re....though it was small, I have tried increasing it but for constant pressure condition for both BCs gives me either laminar or turbulent flow. It is something like a cut section of an infinite pipe with flow...... Thank you, Mahesh
  Reply With Quote

Old   January 12, 2005, 15:50
Default Re: CFD-ACE laminar flow
  #8
Jim_Park
Guest
 
Posts: n/a
What does CFD-ACE tech support say about your problem? The problem is one that they should have tried with the code before they went commercial!
  Reply With Quote

Old   January 12, 2005, 17:50
Default Re: CFD-ACE laminar flow
  #9
Mahesh
Guest
 
Posts: n/a
Havent asked them yet...will do so

Thank you, Mahesh
  Reply With Quote

Old   January 12, 2005, 18:40
Default Re: CFD-ACE laminar flow
  #10
noName
Guest
 
Posts: n/a
I have been using CFD-ACE for about 2 years now (after using Fluent for 2 years before that). I must say they have the worst tech support that exists.

I have also done several numerical experiments to try and validate the code. E.g. Laminar flow over a circular cylinder, LES for turbulence flow over a square cylinder. CFD-ACE will very rarely match data available for such well known solutions, and tech support will have no answers. I have encountered relative errors larger than 100% when comparing test data and CFD-ACE output.
  Reply With Quote

Old   January 12, 2005, 21:22
Default Re: CFD-ACE laminar flow
  #11
Mahesh
Guest
 
Posts: n/a
well, thats strange.

strangely some of the results are wierd. When i plot graphs for pressure gradient the graph seems to start from the origin but it actually goes the other way....i realized this when i plotted the contour. Anyways, i am kinda used to it. But yes...there are definitely some problems.

Mahesh
  Reply With Quote

Old   January 13, 2005, 01:48
Default Re: CFD-ACE laminar flow
  #12
Jim_Park
Guest
 
Posts: n/a
Mahesh,

Even if "I must say they have the worst tech support that exists", ask them anyway.

Another idea. Do you have enough resolution (cells or mesh points) in the axial (flow) direction to resolve the entrance region?

I know Schlichting's "Boundary Layer" text (an old but good book) has an asymptotic solution for a laminar entrance region - and I think some verifying data. That will help you verify that your axial mesh is adequate.

I know you've probably already done this, but there's got to be an answer to your problem somewhere ...
  Reply With Quote

Old   January 13, 2005, 10:14
Default Re: CFD-ACE laminar flow
  #13
MG
Guest
 
Posts: n/a
Mahesh,

I'd suggest you check these 2 references: 1) H.Morihara, R.T.-S. Cheng, "Numerical solution of the viscous flow in the entrance region of parallel plates", J. Comp. Physics, vol. 11, pp. 550-572 (1973). 2) J. Gillis, A.Brandt, "The numerical integration of the equations of motion of a viscous fluid", Air Force European Office of Aerospace Research Scientific Report 63-73, 1964. You'll find numerical results for Re=20 and 200 for the developing flow between two parallel plates. Compare your data with their solutions to see how far you are off. Meanwhile, for a quick check, the entrance region size should be approximately x/Re=0.08 for Re=20, and x/Re=0.07 for Re=200. Here, Re=2hU/vis, h is the half of the channel height, U is the inlet bulk velocity, and x is the non-dimensional distance (scaled with h). The problem is pretty simple, so you should be able to get correct (laminar) solutions, if ACE is really the ace not a$$. You'd be surprised how many com. codes fail these simple tests. MG
  Reply With Quote

Reply

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
Flow meter Design CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33
How to enforce laminar flow while using k-e Grzegorz Kondora FLUENT 0 January 28, 2009 11:35
modelling laminar and turbulent flow in the same Ol FLUENT 2 November 25, 2005 03:52
Divergence of Laminar Flow With Eddy ??? Peter Kostka Main CFD Forum 3 May 9, 2002 17:02
CFD Design...The CFD Future John C. Chien Main CFD Forum 19 October 6, 1999 11:57


All times are GMT -4. The time now is 19:18.