CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

Does the variable 'nbl' have an upper limit?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 29, 2010, 11:50
Default Does the variable 'nbl' have an upper limit?
  #1
Member
 
Yang Yue
Join Date: Feb 2010
Location: Birmingham, UK
Posts: 36
Rep Power: 7
therockyy is on a distinguished road
Hi fellas,

I think the variable 'nbl' is used to define the number or sequence of the mesh blocks in Flow-3D. But I cannot find the definition of it in the help file. I used more than 5 mesh blocks in my simulation, but the nbl only has a rage from 1 to 5 in the output. I didn't give it a limit in my code. Does it have an upper limit defined in Flow-3D orginal code?

Thanks a lot!

Yang
therockyy is offline   Reply With Quote

Old   September 2, 2010, 22:55
Default
  #2
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
The limit for the number of mesh blocks is 500, and it is only set in the post-processor; the solver does not have that limit.

Are you customizing the solver?
MuxaB is offline   Reply With Quote

Old   September 3, 2010, 05:35
Default
  #3
Member
 
Yang Yue
Join Date: Feb 2010
Location: Birmingham, UK
Posts: 36
Rep Power: 7
therockyy is on a distinguished road
Yes, currently I'm using a customised code to tracking the surface entraiment during fill of casting mould. There are still some variables that I cannot understand in the customisation.

Can Flow-3D calculate the six different velocities of the face centres in one element (mesh cell)? or it only has one value, i.e. one velocity in the body centre of the element?

Thank you!

Yang
therockyy is offline   Reply With Quote

Old   September 4, 2010, 11:53
Default
  #4
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by therockyy View Post
Yes, currently I'm using a customised code to tracking the surface entraiment during fill of casting mould. There are still some variables that I cannot understand in the customisation.

Can Flow-3D calculate the six different velocities of the face centres in one element (mesh cell)? or it only has one value, i.e. one velocity in the body centre of the element?

Thank you!

Yang
Velocity components are computed at call faces. For a cell ijk, (i,j,k), u(ijk) is the x-component at the high-x face, u(imjk) (i-1,j,k) is at low-x face and so on. The manual's chapter 9 has more details.
MuxaB is offline   Reply With Quote

Old   September 6, 2010, 05:47
Default
  #5
Member
 
Yang Yue
Join Date: Feb 2010
Location: Birmingham, UK
Posts: 36
Rep Power: 7
therockyy is on a distinguished road
Thanks, Michael.

I just checked the manual. It mentions that the u(ijk), v(ijk) and w(ijk) is the velocities at right, back and top faces respectively, that means the velocity at the left face of cell (ijk) is represented by the velocity at right face of cell (imjk). But how about the velocity at the left face of the far left cell? Is that the reason why Flow-3D using real cells and boundary cells around them?

By the way, when I asked a question about the calculated free surface in Flow-3D by VOF method, Jeff Burnham relpied that "the way FLOW-3D calculates the fluid free surface in sharp-interface problems uses special algorithms (TruVOF and FAVOR) so that the location of the free surface is accurately calculated independent of the mesh size". Does that mean the calculated free surface in Flow-3D is insensitive to mesh size? Since the definition of entrainment through NF values in the customization which I'm using is sensitive to the mesh size, I'm thinking if I can use another method to tracking the entrainment location.

Thanks a lot!

Yang
therockyy is offline   Reply With Quote

Old   September 10, 2010, 21:58
Default
  #6
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by therockyy View Post
Thanks, Michael.

I just checked the manual. It mentions that the u(ijk), v(ijk) and w(ijk) is the velocities at right, back and top faces respectively, that means the velocity at the left face of cell (ijk) is represented by the velocity at right face of cell (imjk). But how about the velocity at the left face of the far left cell? Is that the reason why Flow-3D using real cells and boundary cells around them?

A: Yes, this is one of the reasons. The boundary cells are also used to set other BC variables like pressure and temperature.

By the way, when I asked a question about the calculated free surface in Flow-3D by VOF method, Jeff Burnham relpied that "the way FLOW-3D calculates the fluid free surface in sharp-interface problems uses special algorithms (TruVOF and FAVOR) so that the location of the free surface is accurately calculated independent of the mesh size". Does that mean the calculated free surface in Flow-3D is insensitive to mesh size? Since the definition of entrainment through NF values in the customization which I'm using is sensitive to the mesh size, I'm thinking if I can use another method to tracking the entrainment location.

A: What Jeff meant is that the interface is always kept sharp, that is, contained within one cell, as opposed to spread over several cells. Also the FAVOR method for processing geometry is independent of mesh to a degree in that one can change the mesh without changing geometry and vice versa, in contrast to body-fitted grids.

The solution in general, of course, depends on the resolution. For example, flow features that generally affect the free surface dynamics can be resolved only to the smallest mesh size, etc.

There is a class of relatively simple problems where mesh dependency of the free surface solution in FLOW-3D is minimal, but they are not representative of real world flows.

Thanks a lot!

Yang
ghjfghjsfgfsssssssssssssssssssssssssssssssssssssss sssssssssss
gfssssss
MuxaB is offline   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
How to limit a variable ash OpenFOAM Running, Solving & CFD 1 June 26, 2008 20:32
error in COMSOL:'ERROR:6164 Duplicate Variable' bhushas Main CFD Forum 1 May 30, 2008 04:35
limit for a variable Luis CFX 5 February 12, 2008 06:55
Temperature went outside of its upper limit Atit Koonsrisuk CFX 0 January 8, 2004 12:43
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 21:09


All times are GMT -4. The time now is 22:29.