# conduction between 2 different solids

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 6, 2006, 11:19 conduction between 2 different solids #1 matt Guest   Posts: n/a I have a gas in a steel pipe surrounded by heat insulator. There is forced convection between gas and pipe, conduction in steel pipe, conduction between steel and heat insulator, conduction in heat insulator, and then free convection between heat insulator and ambiant air. The inlet temperature is given by an udf. It change for each step time. I don't know how it's possible to simulate the conduction between steel and heat insulator with Fluent. My boundaries conditions are a wall at the limit of the steel zone and an other one at the begining of the heat insulator zone. I thought about using an udf method to get temperatures values at the limit of the steel zone and put them as boundary condition for the heat insulator zone. Is that a good way? If yes, can you give me the udf program. thanks

 November 9, 2006, 07:04 Re: conduction between 2 different solids #2 RoM Guest   Posts: n/a Is there any need to model the pipe wall? The conductivity of the steel pipe is about 100 times higher than a normal insulator so it play no (or very little) role in the heat transfer to the outside. The limiting factors are the insulator and the free convection. You can model only the fluid zone and set the boundary condition at the wall to "convection". RoM

 November 9, 2006, 09:13 Re: conduction between 2 different solids #3 matt Guest   Posts: n/a Thanks for your idea but i absolutly need to model all the elements. The aim of my study is to know the temperature value at the steel/heat insulator interface, on heat insulator side. I have to compare the adiabatic case (without heat insulator but no heat flux on steel pipe boundary with outside) and the real one. So I have to make an UDF to get steel pipe limit temperature value and an other one to calculate heat flux between steel and heat insulator. thanks for your help.

 November 9, 2006, 09:36 Re: conduction between 2 different solids #4 RoM Guest   Posts: n/a You dont need an udf to model the solid zones. You can run the Gambit journal below to see the basic geometry setup. If you mesh the 3 volumes and export the mesh to Fluent, Fluent will create some interface zones between the different fuid/sold zones. Dont change those interfaces. Assign the porper materials to the steel and insulator solid zones, define a convection bc for the wall (wall material is not important, thickness = 0.) and set up the gas flow. If everything works right Fluent will calculate a heat flow through both solid zones. Good luck, RoM default set "GRAPHICS.GENERAL.CONNECTIVITY_BASED_COLORING" numeric 1 volume create height 100 radius1 5 radius3 5 offset 0 0 50 zaxis frustum volume create height 100 radius1 6 radius3 6 offset 0 0 50 zaxis frustum volume create height 100 radius1 7 radius3 7 offset 0 0 50 zaxis frustum volume split "volume.3" volumes "volume.2" connected bientity volume split "volume.2" volumes "volume.1" connected bientity physics create "gas" ctype "FLUID" volume "volume.1" physics create "steel" ctype "SOLID" volume "volume.2" physics create "insulator" ctype "SOLID" volume "volume.3" physics create "wall" btype "WALL" face "face.8" physics create "inlet" btype "WALL" face "face.12" physics create "outlet" btype "WALL" face "face.13"

 November 9, 2006, 09:57 Re: conduction between 2 different solids #6 RoM Guest   Posts: n/a If your problem is not multiphase you should always use Get_Domain(1). But as i said in my previous post, there is no need for an udf in this case. Fluent can calculate heat transfer between different solid zones. All you have to do is set up the geometry right (make shure everything is connected). RoM

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post jlefevre76 FLUENT 2 February 5, 2013 10:53 chingyinh ANSYS Meshing & Geometry 6 December 21, 2012 01:52 bawfuls FLUENT 3 August 11, 2011 21:50 srinidhi4u FLUENT 0 September 15, 2009 07:30 Fluent FLUENT 2 July 22, 2005 06:08

All times are GMT -4. The time now is 09:47.

 Contact Us - CFD Online - Top