CFD Online Logo CFD Online URL
Home > Forums > FLUENT

Concerning the setup of axisymmetry 2D simulation.

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

LinkBack Thread Tools Display Modes
Old   January 26, 2007, 13:00
Default Concerning the setup of axisymmetry 2D simulation.
Posts: n/a
For the axisymmety 2D model with the following boundary conditions: -----------------------------------------------------

name id type


interiorfluid 2 fluid

inlet 6 velocity-inlet

symm 3 symmetry

outlet 4 outflow

wall 5 wall

default-interior 8 interior -----------------------------------------------------

Why does Grid "check" report the warning of negative vaue if I choose "axisymmetric" (define/moldels/solver...) and make the simulation not to perform? However, if I select "2D"(define/moldels/solver...). Then, everything goes normally. So, my question is that:

(1)what is the explanation for this phenonenon?

(2)How to define the axisymetry 2D simulation? I mean, should I define it as symetry in Gambit or define it as "axisymmetric" in Fluent GUI? Gnerally, how to make these two methods consitent so as to avoid the above mentioned error which is often not easy to find out. At least, it takes me one week to find this problem.

Please give your idea.

  Reply With Quote

Old   January 26, 2007, 14:30
Default Re: Concerning the setup of axisymmetry 2D simulat
Posts: n/a
For axisymmetric problems, there should be a boundary of the type axis and it should lie on x axis. The domain should lie above this axis. You can make a your geometry with the one edge along x axis and all faces above this edge. Define this edge as axis in gambit itself. Symmetry and axisymmetry are different concepts.

  Reply With Quote

Old   January 30, 2007, 12:27
Default Re: Concerning the setup of axisymmetry 2D simulat
Posts: n/a
Just a note, the axis BC is only used if the axis lies in the fluid domain (i.e. a circular pipe). If the flow is annular, then the axis BC will not be used. Fluent will always treat the X Axis as the center of rotation. The "axis" BC avoids a singularity if the fluid goes all the way to the center of rotation.

Hope this helps, Jason
  Reply With Quote

Old   January 31, 2007, 11:13
Default Re: Concerning the setup of axisymmetry 2D simulat
Posts: n/a
For a cylinderical geometry, there are three options for simplfying the simulation as 2D:

(1) H*R (or: H*x) (symmetry);

(2) H*R (axisymemmetry);

(3) H*(2R) or H*D (2D). (Note: H-height, R-Radius, D-Diameter)

Actually, all these options are related physically to the centerline or the axis.It seems that the three options were accepted and adopted indifferent literature and to some extent they all reflect the symmetry treatment for the cylindrical geometry.

In the above discussion, we only touch on the specifical seeting according to Fluent protocol. However, here I would like to question about the choice of the "symmetry treatment". That is:

(1) How to choose one from the three options? Which one is better? Why?

(2) Do you think the "axisymmetric" (as defined in FLuent, i.e.) is prefered than the other two options?

These are what I am wondering. I hope to get helps from you. Thanks in advance.

  Reply With Quote

Old   January 31, 2007, 17:23
Default Re: Concerning the setup of axisymmetry 2D simulat
Posts: n/a
Option (3) is the 2D approximation and works in the X-Y (Cartesian) coordinates. In this case, you can picture your geometry as extending into your screen to infinity. The assumption is that there's no curvature as the geometry moves out of the modeling plane (i.e. d/dz = 0, no change in the Z direction). This has nothing to do with axisymmetric geometry. And Option (1) isn't a way of representing axisymmetric geometry, because it's really just Option (3) with a symmetry BC. All of the flow equations are solved in the Cartesian coordinates, and since d/dz=0 for all properties, there is no allowance for curvature. If either Option (1) or Option (3) were used to model axisymmetric geometry, then they made some major assumptions, and if you're not sure what the assumptions are, then this can be VERY dangerous. Think of the flow profiles coming out of a pipe versus the flow coming out of a rectangular slit (assuming that the end walls are negligible), or flow over a sphere versus cross flow over an infinite cylinder.

Option (2) is the Axisymmetric approximation, which works in the X-Radial (Cylindrical) coordinates. I say radial, but in some cases, such as XY Plots, the Radial dimension is still called the 'Y' dimension. In this case, the assumption is that the geometry is constantly revolved 360degrees about the X-Axis (i.e. d/dtheta=0, no change in the theta direction). The equations are therefore solved in a Cylindrical coordinate system where d/dtheta=0.

As far as choosing from the three options, that depends heavily on what you're doing.

Option (3) is for "2D" flow. Like a rectangular jet, assuming that the depth of the jet (the dimenion into/out of your screen) is much larger than the height of the jet. This can also be used if the radius of curvature is very large compared to the geometry being modeled, like I've seen this used to model lubrication heating in a very large bearing... the diameter of the bearing was MUCH larger than the thickness of the film being modeled, making the curvature effects negligible.

Option (2) is the axisymmetric model and it's used for "revolved" geometry, such as a pipe or an annulus. There's also an "axisymmetric with swirl" option which allows for swirl velocities (changes in velocities in the theta direction are still 0 though).

Once again, Option (1) is just the 2D approximation (option (3)) with a symmetry BC used. Symmetry BCs aren't dependent on the modeling though, and it can be used in conjunction with Option (2) or Option (3), just be careful that your implementation makes sense. In an axisymmetric domain (option (2)) it doesn't make sense for the symmetry condition to be used if it's not perpendicular to the axis of rotation... The numerical assumptions behind the model will allow you to use a Symmetry BC just about anywhere, but it's up to you to make sure you are careful not to use it in places that don't make sense.

Hope this helps, and good luck, Jason
  Reply With Quote


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
Quenching simulation - wall boiling model Michael.J CFX 10 August 27, 2013 17:02
geometry "fluid volume' setup for simulation Easyflow8 FLUENT 0 February 3, 2011 21:42
GUI crash and simulation engine still running RPJones FLOW-3D 2 November 9, 2010 09:18
velocity profile export from a simulation onto another sudhirlv STAR-CCM+ 1 September 12, 2010 18:57
Simulation doesn't meet reality Hans FloEFD, FloWorks & FloTHERM 1 June 9, 2010 08:59

All times are GMT -4. The time now is 11:36.