Defining convection constraints

Convection is an exchange of thermal energy that is proportional to the difference between the surface temperature on the geometry and the temperature of the surroundings.

Defining convection in the Nastran environment

You can use the Convection command to specify a free convection boundary condition for a heat transfer analysis. Free convection allows thermal communication between a surface and an ambient environment through a heat transfer coefficient and a surface element (CHBDYE, CHBDYG, or CHBDYP).

In the Nastran environment, the options in the Convection dialog box generally correspond to the fields on the CONV bulk data entry. However, Nastran requires a number of different bulk data entries, such as CONV, PCONV, and MAT4, to fully define free convection. The software automatically creates these necessary bulk data entries when you export or solve your model. Specifically, it creates:

• A CONV and PCONV bulk data entry.

• An SPOINT and SPC entryWhen you define the Ambient Temperature value in the Convection dialog box, the software automatically creates an SPOINT entry. The software assigns the ID field on the SPOINT ID entry to the TA field in the CONV entry. The software then uses an SPC entry to constrain the temperature value at that location.

• MAT4 or MATT4 entries which contain the Convection Coefficient value you specify in the Convection dialog box.

Additionally, in Nastran, surface elements (CHBDYE, CHBDYG, or CHBDYP) provide the geometric connection between the structural elements in the mesh and the applied convection. Because you cannot create Nastran surface elements directly in Pre/Post, Pre/Post automatically creates them for you when you export or solve. In a SOL 153 or 159 analysis, you can use the Geometric Surface Element Form option on the General tab of the Solution dialog box to control the type of surface elements that the software automatically creates.

Defining convection in the Abaqus environment

In the Abaqus environment, the options in the Convection dialog box correspond to the parameters for the *CFILM or *FILM keywords depending on the options you select. In Abaqus, film conditions define heating or cooling due to convection by surrounding fluids.

• Element-based film conditions define convection from element faces in the model (*FILM).

• Concentrated film conditions define convection from nodes or vertices (CFILM).When shell elements are formatted, the nodal area is equal to td/2.0, where t is shell thickness and d is the distance between the node and its neighbor nodes. The software calculates the nodal area automatically so you do not need to enter it in the Convection dialog box (Abaqus).

In Abaqus, you use the *FILM and *CFILM keywords to define film coefficients and sink temperatures for heat transfer and fully coupled thermal-stress analyses.

For more information, see:

• *FILM and *CFILM in the Abaqus Keywords Reference Manual

• Thermal Loads in the Abaqus Analysis User’s Manual

Defining convection in the ANSYS environment

In the ANSYS environment, the options in the Convection dialog box correspond to the SFE,,CONV command. Convections are surface loads that you can apply to the exterior surfaces of your model to account for heat lost to (or gained from) a surrounding fluid medium. In ANSYS, you can only define a convection load on solid and shell elements.

You can use the surface effect elements (SURF151 or SURF152) to analyze heat transfer for convection/radiation effects. The surface effect elements allow you to generate film coefficient calculations and bulk temperatures from FLUID116 elements and to model radiation to a point.

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	Convection
Simulation Navigator	Right-click Constraints→New Constraint→Convection

How do I

Define convection constraints

Define convection constraints (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Defining convection constraints, 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 } });