Define a spatial pressure load in parameter space

When you use either the spatial distribution method or a spatial boundary condition, you can map the boundary condition to parameter space using U, UV, or UVW locations.

The following example shows how to map a spatial boundary condition to a location defined by a parameter curve (U).

1. Choose Home tab→Loads and Conditions group→Pressure .

2. In the Pressure dialog box, from the Type list, select Normal pressure on 2D elements or 3D element faces.

3. Select the geometry or FE entity to which the pressure will be applied.

4. Click and select from New Field→Formula .

5. In the Formula Field dialog box, from the Independent list, select Parameter.The u variable is listed in the Independent table.Note: The domain list is filtered to include only spatial domain types. Parametric types include Parameter, Parameter Plane, and Parameter Space).You do not need to assign a dependent variable, because the software automatically assigns the dependent domain to be unitless and dimensionless.

6. Expand the Spatial Map group. From the Type list, select Parametric Space.

7. From the Bounding Box list, select Opposite Corner.

8. With the first Specify Point highlighted, select a point in the model to define one corner of the bounding box.

9. With the second Specify Point highlighted, select the second corner of the bounding box.

10. With Specify CSYS highlighted, select the coordinate system to use to map the field.See CSYS dialog box for more information.

11. In the Expressions box, enter the ramp function:if (ug_var("u") <0 || ug_var("u") >1)(0) else (1*(ug_var("u")))Tip: Double-click the expression u in the Filters list to add it to the new expression.

12. Click Accept Edit . The expression is added to the Expressions list.

13. Click OK to create the field.The field is mapped to the location identified by the bounding box and coordinate system.

14. In the Scale Factor box, type 1.0.

15. Click OK.The graphic shows the resulting pressure defined for the spatial field.Tip: Change the boundary condition style to Expanded to view a more detailed display of the pressure load. To do this, right-click the pressure and choose Style.

How do I

Define a time-varying force with a formula field

Define a spatially-distributed force with a formula field

Define a spatial normal pressure load

Breakout modeling workflow

Learn more

Using fields and expressions to define boundary conditions

Breakout modeling

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Define a spatial pressure load in parameter space, 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 } });