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

Why: Point velocity always monitored as 0.0?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 4, 2007, 19:01
Default Why: Point velocity always monitored as 0.0?
  #1
Tanhn
Guest
 
Posts: n/a
I want to monitor the point velocity at my axisymmetry 2D model; however, the axial velocity is always plotted as ZERO. In fact, when I checked the axial velocity value at 0.5m. It has a non-zero value.

What is the problem? Please advise. Thanks in advance.

----------------------------------------------- The steps taken are:

(1) Surface->Point(x0=0.5,y0=0.0)-> name: p0.5m

(2) Solve-> monitors-> surface->monitor 1/every time step/define...:

Report type: mass-weighted average

Report of: Velocity/axial velocity

Surface: p0.5m

(3) then, seclect OK

(4) iterate...

  Reply With Quote

Old   February 5, 2007, 10:07
Default Re: Why: Point velocity always monitored as 0.0?
  #2
Jason
Guest
 
Posts: n/a
If I had to guess, I'd think it's the mass-weighted average (mass flow through a point is 0 even if the velocity has a value because the area of a point is 0)... you're looking at a point, so use the vertex average.

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

Old   February 5, 2007, 10:39
Default Re: Why: Point velocity always monitored as 0.0?
  #3
Tanhn
Guest
 
Posts: n/a
Hi,Jason,

It works when using the vertex average.Thanks.

Although this problem is solved. However, I stilll do not understand how to choose the REPORT TYPE for different variables concerned(such as temperature, pressure,volume fraction,velocity,...).

Afterall, there are a number of options under the REPORT TYPE item. So, could you give me a general indication for performing a choice properly?

  Reply With Quote

Old   February 6, 2007, 10:47
Default Re: Why: Point velocity always monitored as 0.0?
  #4
Jason
Guest
 
Posts: n/a
It depends on what you're looking for. For a point, there is only one vertex, so max, min and average are the same. Both a point and a line have zero area, therefore any of the report types having to do with area will be zero (mass report types, because mdot=rho*A*v, if A=0, mdot=0).

If you're looking at the average across a surface, then you have to pick from vertex, facet, area, and mass flow report types.

Vertex averaging interpolates the flow field solution to each vertex on the surface you're interested in, then sums all of the values for the vertices you're interested in and divides by the number of vertices:

<indent>Vertex_avg = sum(Value)/(number of vertices)

Facet averaging is the same thing, but interpolates and sums across the facet centers instead. (I don't think Facet averaging works along a line, but it may interpolate to the edge centers. If someone's tried it, can you comment?)

Area weighted averaging goes a step further from facet averaging and takes into account the area of the facet:

Area_weight_avg = sum(Facet_Area * Value)/sum(Facet_Area)

This is helpful because typically your cell faces aren't of a constant area and you don't want tiny cells counting the same as large cells. Example is flow through a pipe with a BL mesh. You don't want the cell next to the wall which is extremely tiny and has a velocity of close to zero to count as much as the large cell at the centerline. This also explains why it doesn't work for a point or a line, because when it multiplies Facet_Area by Value it always gets zero.

Flow weighted averaging is similar, but uses the flow through a facet instead of the area of the facet:

Flow_weight_avg = sum(Facet_Flow * Value)/sum(Facet_Flow)

Choosing between the different averaging techniques depends on what you're looking for and what you're comparing it to. If you're comparing it to area averaged data, then you should be using area averaged calculations. If you're comparing it to mass flow weighted values, then you should be comparing it to mass flow weighted calculations.

Hope this helps, and good luck, Jason
  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
Results of CFX Simulations Sof_70_Usthb CFX 3 July 9, 2011 06:15
Dynamic Mesh- Parallel UDF DE HEART Fluent UDF and Scheme Programming 14 August 11, 2010 01:29
Gmsh and samplesurface touf Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 December 10, 2007 03:27
STONE'S STRONGLY IMPLICIT SOLVER anybody Main CFD Forum 8 August 18, 2006 10:01
chemical reaction - decompostition La S. Hyuck CFX 1 May 23, 2001 00:07


All times are GMT -4. The time now is 16:54.