Hi, all,

Just read the Fluent user's menu, it seems Fluent can also simulate heat transfer in solid regions. I tried but failed to get the temperature distributions inside a solid region. Would you pls tell me how to do such simulation ?

Thanks,

T. T.

Correct... Fluent can simulate heat transfer in solid regions. Two options I am aware of: Option 1) -- mesh the "solid" volume along with your fluid volume, with wall boundaries separating the two volumes. You can then speicty the solid as a "solid" material, give material properties (same as you would for a fluid). The surfaces bounding the solid volume can then be specified boundary conditions, as appropriate. When the mesh is read into FLUENT, surfaces between the fluid and solid volumes will be automatically identified and a "[surf name] and [sufrace name}-shadow boundary will be created. Option 2) -- if your solid volume corresponds to a bounding surface in the mesh and is of uniform thickness and composition, you don't have to mesh the solid volume. Instead, you can activate the "shell conduction" option. this will create shell elements (not visible or plottable), where you can similarly specify material conposition and BCs. (Note: if two "shell conduction" sones are adjacent to each other, then are treated as totally disassociated from each other. They will NOT conduct energy from one to the other). I have used both options often and compared FLUENTs results to stand alone analysis (ANSYS) with same thermal BCs and have always obtained equivalent results....I threfore have good confidence in FLUENTs abilities to accurately perform this analysis.

Thanks Glenn! Acturally I tried the first option, but failed to see the variation of temperature inside the solid region, so, confusing... Maybe something is wrong.

I would suggest checking units of conductivity for the material solid. Also, suggest creating a post-processing surface which traverses through the solid material only and then plotting temperature (auto-scaled) on the traversing surface. You should see something....note the auto-scaled range of magnitudes. Check results (approximately) with a rough hand-calculation so you know what to expect. Just some suggetions....

how obuut 2D? i have to simulate one heat source it the soil from one pipe.....source of heat about 50^C......thickness ch4 pipe negligible for example dim about 14mx10m....thanks

i have been solve for 2d as Glenn suggestion.... have one more queston: how to set boundary condition for wall as linear temperature not constant temperature conduction?....for example we have 4 node: node1=12^C, node 2=14^C, node3=16^C, Node4=18^C?....thanks

You can read in a *.prof file which specifies a variable (wall temperature, in this case) as a function of X,Y,Z (or radius) cordinates. See the FLUENT documentation for the format of a *.prof file. Once read in, go to the wall boundary condition window and you can now hook to the variable from there. Please note: FLUENT does a zero-order interpolation of the variable onto the boundary, so if a linear variation is required, you need to specify many points in the *.prof file...or you can create a UDF and apply the BC as a UDF.

thanks, a have been done it for my case. thank you.

my conclusion: the same as modeling sine, cosine, ... functions like finite difference methods..one should be make the value in table form as fluent tutorial..