Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Transient Heat Transfer [Acusolve]

Hi everyone.
I have a question regarding the initial temperature boundary condition in acusolve transient heat transfer.
Initial temperatures of body and fluid are known.

I used Nodal initial condition to provide initial temperature. How to assign initial tempreatures of the volume and surfaces?

Thanks in advance for help.

Find more posts tagged with

AcuSolve

English

Accepted answers

All comments

acupro

In AcuConsole, you can do this with 'Temperature initial condition type' set to 'Script'. Then select 'Open Text' for 'Temperature script' and use functions like 'if inVolume' to set the values for the different Volumes (element sets). You can also do this in the input file itself:

 NODAL_INITIAL_CONDITION( 'temperature - body' ) {     selection_type             = element_set    element_set                = 'body'     variable                   = temperature     type                       = constant    constant_value             = 273.0    satisfy_boundary_condition = off    precedence                 = 1 }

Mateusz L

Thank you for instructions, I will try this /emoticons/default_biggrin.png' srcset='/emoticons/biggrin@2x.png 2x' title=':D' width='20' />

Vignesh Lakshmanan

Hi,

I would like to define a zone Boundary condition that my body is maintained at a particular temperature, rather than initial condition. How can I do this in HW CFD

Thanks in Advance,

Vignesh

acupro

Hi,

I would like to define a zone Boundary condition that my body is maintained at a particular temperature, rather than initial condition. How can I do this in HW CFD

Thanks in Advance,

Vignesh

It looks like HWCFD doesn't yet have the ability to select nodes/volumes and apply Nodal BCs.

If this is a solid volume in which you want to maintain a constant temperature - it's fine just to remove that meshed volume, and apply a constant temperature boundary condition on the surfaces where it would be in contact with the rest of the meshed model. It would then have the same effect overall for the rest of the model.

Vignesh Lakshmanan

It looks like HWCFD doesn't yet have the ability to select nodes/volumes and apply Nodal BCs.

If this is a solid volume in which you want to maintain a constant temperature - it's fine just to remove that meshed volume, and apply a constant temperature boundary condition on the surfaces where it would be in contact with the rest of the meshed model. It would then have the same effect overall for the rest of the model.

Thanks for your reply.

My requirement is this: I am simulating Nat convection (and next will be forced convection with fan) heat dissipation from a heat sink attached to a heat source. Both the heat sink and source are placed in a room at ambient temperature (here it is my computational domain). I cannot remove the domain right. Is there a possibility to define ambient temperature on my domain?

Regards

Vignesh

acupro

Thanks for your reply.

My requirement is this: I am simulating Nat convection (and next will be forced convection with fan) heat dissipation from a heat sink attached to a heat source. Both the heat sink and source are placed in a room at ambient temperature (here it is my computational domain). I cannot remove the domain right. Is there a possibility to define ambient temperature on my domain?

Regards

Vignesh

The energy added from the heat source will go from the heat source into the heat sink and into the surrounding air domain - thus raising its temperature. It seems it would not be appropriate to define a constant temperature (through Nodal Boundary Condition) to that surrounding air domain. It would be appropriate to define an initial condition - as the surrounding room temperature. I would suggest you put a boundary condition on the outer surfaces of that air domain and define the constant temperature on those surfaces, some distance from the object(s) of interest so they don't really affect what is happening near those bodies. The air near the source and heat sink will get hotter and rise (with Boussinesq density model) as expected.