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

problems in natural convection

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 16, 2004, 00:39
Default problems in natural convection
  #1
nabeel
Guest
 
Posts: n/a
hi, i am simulating quenching of heated cylinder in oil with natural convection. i want to ask four question 1.what is effect of g and operating density in opersting condition.what density and temperature should i use to get sonverged solution. 2.mr Ra is < 10e8 suold i use turbulence model 1equ or two equ. 3.in manuual it is mentioned that u use pressure p' in ur simulation.what this p' means. 4.during my simulation my monitors show on heated cylinder wall temp 325 this is temp on which i initialised my simualtion.but actually my temeprature is 1473 and it should fall with time in transient anlysis rather that it increase. can anbody help in this regard. nabeel
  Reply With Quote

Old   July 16, 2004, 12:20
Default Re: problems in natural convection
  #2
Evan Rosenbaum
Guest
 
Posts: n/a
1. The operating density won't matter too much as long as you have defined temperature dependent density in the materials panel. 2. For a viscous material like oil, use a two equation model. 3. p' = p + rho x g x h 4. After initializing the problem, set the initial temperature of your cylinder to 1473 using the patch command.
  Reply With Quote

Old   July 22, 2004, 00:44
Default Re: problems in natural convection
  #3
nabeel
Guest
 
Posts: n/a
hi, u have said that patch velocity to cylinder but in my modeling rectanlge simulating fluid and a small area having thickness of cylinser area is subtracted from large area.i have given temperature 1473 to small area inner wall and given thickness of wall and outer wall having same temperaure but no thickness.is am on right path.patching rectangle is considering the fluid is at 1473!. second solution is not converging how i can judge that solution is going right.can any method.using segregated solver and presto for pressure second order for other. nabeel
  Reply With Quote

Old   July 22, 2004, 12:06
Default Re: problems in natural convection
  #4
Evan Rosenbaum
Guest
 
Posts: n/a
You cannot use a wall to model this transient. A wall in FLUENT can have a thermal resistance, but had no thermal capacity (i.e., density and specific heat capacity = 0). You need to model the cylinder as a solid, so it will have a thermal capacity.
  Reply With Quote

Old   July 23, 2004, 00:22
Default Re: problems in natural convection
  #5
nabeel
Guest
 
Posts: n/a
hi, but in defining solid i have shadow BC what should i do then.how can i handle this shadow condition nabeel
  Reply With Quote

Old   July 23, 2004, 12:16
Default Re: problems in natural convection
  #6
Evan Rosenbaum
Guest
 
Posts: n/a
If you leave the default BCs for the walls at the solid/fluid interface, they just track the temperature of the underlying solid.
  Reply With Quote

Old   July 25, 2004, 10:21
Default Re: problems in natural convection
  #7
nabeel
Guest
 
Posts: n/a
hi, i have modeled solid region and fluid region.i meshed them both separately.i intialised solution at 313k.then i patched 1473 to solid zone.but a after solution i have found no gradien all fluid is at 313 and solid zone is at 1473.i think no interaction is taking place.second is neccesary to give wall 1473 temperature. nabeel
  Reply With Quote

Old   July 26, 2004, 12:17
Default Re: problems in natural convection
  #8
Evan Rosenbaum
Guest
 
Posts: n/a
Go back into GAMBIT and merge coincident edges. I think you have two, uncoupled sets of nodes along the common edges. This can happen if you create your solid and fluid areas using booleans.
  Reply With Quote

Old   July 28, 2004, 02:06
Default Re: problems in natural convection
  #9
nabeel
Guest
 
Posts: n/a
hi, i am very grateful that u are guiding me in this problem.sir can i use split faces command instead of subtract command.merge command is not working and giving error that egdes are not connected.secong can i merge faces. nabeel
  Reply With Quote

Old   July 28, 2004, 11:55
Default Re: problems in natural convection
  #10
Evan Rosenbaum
Guest
 
Posts: n/a
Yes, I think split faces should work.
  Reply With Quote

Old   July 29, 2004, 01:28
Default Re: problems in natural convection
  #11
nabeel
Guest
 
Posts: n/a
hi, i want to ask that then i use link edges command of fluid faces and solid faces.to transfer temperature data. nabeel
  Reply With Quote

Old   July 29, 2004, 01:28
Default Re: problems in natural convection
  #12
nabeel
Guest
 
Posts: n/a
hi, i want to ask that then i use link edges command of fluid faces and solid faces.to transfer temperature data.or i should use connect edge command nabeel
  Reply With Quote

Old   July 29, 2004, 04:02
Default Re: problems in natural convection
  #13
nabeel
Guest
 
Posts: n/a
hi, when i use subtract comd it does not merge edges b/c they do not coincide.what should i do. nabeel
  Reply With Quote

Old   July 29, 2004, 17:14
Default Re: problems in natural convection
  #14
Evan Rosenbaum
Guest
 
Posts: n/a
Don't use booleans. I think tou have a right-circular cylinder in a square tank. Create the surfaces directly from the vertices to the lines to the surfaces to the volumes. This will ensure everything is connected.
  Reply With Quote

Old   August 2, 2004, 01:54
Default Re: problems in natural convection
  #15
nabeel
Guest
 
Posts: n/a
hi, after merging edges i meshed domain.but they are not exporting mesh b/c it is not considering continuum type b/c of virtual face . second i am doing analysis in 2d and having rectangle showing oil and cylinder geometry profile . sir can u guide me nabeel
  Reply With Quote

Old   August 2, 2004, 12:48
Default Re: problems in natural convection
  #16
Evan Rosenbaum
Guest
 
Posts: n/a
You should still be able to mesh this directly. Create four vertices for the corners of your tank and four more for the corners of your cylinder. Create lines between the vertices and then create faces from the lines. See figure.

x-----------x |\ /| | \ / | | x-----x | | | | | | | | | | | | | | x-----x | | / \ | |/ \| x-----------x

x = Vertex | and - = Faces

This will have all connected geometry.
  Reply With Quote

Old   August 3, 2004, 07:00
Default Re: problems in natural convection
  #17
nabeel
Guest
 
Posts: n/a
hi, i have splitted my domain as u said.when i use rampant solver it export mesh and boundary condition and continum type are quite accurately defined.can u tell me that is my solver type is correct and what effect it has on problem. nabeel
  Reply With Quote

Old   August 3, 2004, 12:08
Default Re: problems in natural convection
  #18
Evan Rosenbaum
Guest
 
Posts: n/a
Unfortunately, I don't know anything about RAMPANT. We only use FLUENT.
  Reply With Quote

Old   August 4, 2004, 00:14
Default Re: problems in natural convection
  #19
nabeel
Guest
 
Posts: n/a
hi, sir ihave got solution and how i judge that my solution is accurate if it is not converging.my residuals are less than one nabeel
  Reply With Quote

Old   August 6, 2004, 00:52
Default Re: problems in natural convection
  #20
nabeel
Guest
 
Posts: n/a
hi, rampant is solver density based code used for unstructured mesh in fvm.sir it is used in before exporting mesh file in gambit.bc are dependent on solver type. sir how i judge the solution is right nabeel
  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
Very simple natural convection problem Naseem FLUENT 17 December 15, 2015 11:12
Natural Convection Problem - Helium marzoa STAR-CCM+ 0 April 18, 2011 14:12
CFX Natural Convection, please help. dbecker CFX 5 October 13, 2010 19:07
CFdesign and Natural Convection Javifonte Autodesk Simulation CFD 1 November 17, 2009 14:59
Natural Convection with heat generation krishnachandranr Main CFD Forum 0 July 28, 2009 04:22


All times are GMT -4. The time now is 23:58.