Defining the rate of heat flux

You can use the Heat Flux command to define the rate of heat energy that is transferred through a given area. When you specify the magnitude for the heat flux:

• A positive value indicates a movement of heat energy into the area.

• A negative value indicates a movement of heat energy out of the area.

Defining a heat flux in the Nastran environment

In the Nastran environment, the Type options in the Heat Flux dialog box control which bulk data entry the software creates when you export or solve your model.

• Uniform element and Uniform element—spatial apply a heat flux to surface elements and correspond to the QBDY3 bulk data entry. With these options, you can also specify a node as an optional control point. Nastran uses the temperature at that node to multiply the heat flux terms.

• Variable element and Variable element—spatial apply a heat flux to grid points (nodes) on surface elements and correspond to the QBDY2 bulk data entry.

• Grid and Grid—spatial apply a heat flux to an area defined by grid points (nodes) and correspond to the QHBDY bulk data entry.

For more information, see the Simcenter Nastran Thermal Analysis User’s Guide.

Defining a heat flux in the Abaqus environment

In the Abaqus environment, the options in the Heat Flux dialog box correspond to the Abaqus *DFLUX, *DSFLUX, and *CFLUX keywords.

• You can select DFLUX to apply distributed fluxes to polygon faces or element faces in a fully coupled thermal-stress analysis.

• You can select DSFLUX to apply distributed fluxes to surface regions in a fully coupled thermal-stress analysis.

• You can select CFLUX to apply a concentrated heat flux to any node or set of nodes in a fully-coupled thermal-stress analysis.Note: In the Abaqus input file, a nodal heat flux magnitude must be specified per node number (units of energy per time, for example J/s where J is joule and s is seconds). The units of the Heat Flux value in the Heat Flux dialog box are Power per Length2 (for example, W/mm2), where Power is the amount of energy consumed per unit of time. In the SI system, the unit of power is a watt, W, which is equivalent to J/s. The software calculates the nodal area for each node as thickness x average distance between nodes or t*d/2. It then multiplies the associated nodal area by the Heat Flux value to compute the concentrated nodal heat flux for each node. The software writes the concentrated nodal heat flux in consistent units:(Power/Length2)*Length2= Power, such as J/s

For more information, see *DFLUX, *DSFLUX, *CFLUX in the Abaqus Keywords Reference Guide.

Defining a heat flux in the ANSYS environment

In the ANSYS environment, the options in the Heat Flux dialog box correspond to the ANSYS SF and SFE commands. When you export or solve your model:

• If you select Nodal or Nodal-Spatial from the Type list, the software includes the SF,,HFLUX command in your input file. With these options, you select

• If you select Element, Elemental, Element-Spatial, or Elemental-Spatial from the Type list, the software includes the SFE,,HFLUX command in your input file.

In ANSYS, sometimes you may need to apply a heat flux that your element type does not accept. In those cases, you can use surface effect elements to overlay the current mesh. When you solve your model, the surface effect elements serve as a conduit to apply the heat flux. In the Heat Flux dialog box, you can use the SURF151 or SURF152 options to create surface effect elements.

• SURF151 elements can be overlaid on 2D thermal solid elements, such as PLANE77 elements.

• SURF152 elements can be overlaid on 3D thermal solid elements, such as SOLID87 elements.

If you use surface effect elements to apply the heat flux, you can also use the FLUID116 options to connect the SURF151 or SURF152 elements to FLUID116 elements. In ANSYS, a FLUID116 element is a 3D element that can conduct heat and transmit fluid between its primary nodes. FLUID116 elements:

• Are used in coupled-thermal fluid analyses.

• Have two primary nodes and can have two additional optional nodes.

Where do I find it?

Application	Pre/Post
Prerequisite	An active Simulation file with Nastran, Abaqus, or ANSYS as the specified solver and Thermal as the specified Analysis Type
Command Finder	Heat Flux
Simulation Navigator	Right-click Loads→New Load→Heat Flux

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Defining the rate of heat flux, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });