[numberone]

hello,

im new at fluent/ gambit. i have a problem with heat generation in fluid.

i drawed a pipe in 2D in gambit and meshed.

here is the pic.




Source terms only works with fluid, not solid part. how can i fix it ?


Thanks.

[ComputerGuy]

While it looks like you have the energy equation enabled (assuming the picture you've shown is of temperature contours), the source term for the solid can only be enabled if the energy equation is being solved.

Have you defined the region as a solid (Define--->Boundary Conditions--->Solid_Zone-->Solid)?

ComputerGuy

[numberone]

energy equation is checked..
face1 (inside of pipe) is selected as fluid and given source temrs.
face2 (pipe) is selected as solid.

face2 didnt effected from face1's source terms.. it seems pure blue . what should i do ?

[ComputerGuy]

Perhaps you didn't create the geometry appropriately, such that the two zones are connected? This is necessary for conjugate heat transfer. While there are many ways of creating your geometry in Gambit, a simple command list might be:

face create width 20 height 10 xyplane rectangle
face create width 20 height 8 xyplane rectangle
face split "face.1" connected faces "face.2"

This will create an 8x20 flow channel, and two, 1x20 walls on either side. When you load the model into Fluent, assuming you've defined an inlet and an outlet on the fluid, you should be left with a solid-fluid wall and a solid-fluid wall "shadow." This means that you have a thermally coupled boundary between a fluid and a solid. If you don't see "shadow" in the list of boundary conditions, you likely have an uncoupled system.

Have a look, and if you can't get it, send me your Gambit journal.

[ComputerGuy]

numberone,

First, if this is a symmetric problem, you should define the "eksen" boundary in your journal file as a symmetry condition, not an axis.

Second, I've made a fictitious case with no modification to the default values in fluent (aluminum and air for the solid and fluid, respectively). I've also imposed a heat generation rate of 1e5 W/m^3 in the air. Have a look at contours of wall flux-->total surface heat flux in your solution. You'll see that the solid and the fluid are coupled by default (heat flux in = heat flux out). Note that the temperature variation within the solid is quite low because its thermal conductivity is quite high. As such,if you try and view contours over the whole range of temperatures, you won't see any variation within the solid. Try unselecting the "auto range" button on the contours tab and choosing the coldest temperature for the Min, and 1 degree warmer than the coldest temperature for the Max. This will show you that there is temperature variation within the solid

Lower the thermal conductivity of your solid to be close to that of your fluid and you'll see a more striking difference.

ComputerGuy