Creating 1D Properties

This task shows you how to:

Add 1D physical properties to a shape design by selecting a meshed wireframe geometry
Create local 1D properties (on the condition a 1D property was previously applied to the geometry).

A 1D property is a physical property assigned to a section of a part. You can also associate a local 1D property to a piece of the geometry.
To know more about this property, refer to Beam Property in the Finite Element Reference Guide.

Open the sample52.CATAnalysis document from the sample directory.

Make sure a material was applied to the geometry and a linear 1D mesh part was assigned to the beam (it is already done in this particular case).
To know more about linear 1D mesh part, refer to Creating 1D Mesh Parts in this guide.
You cannot apply 1D properties and 1D mesh parts on geometry included in a sketch.

Adding 1D Physical Properties

You can add 1D physical properties to a shape design by selecting a meshed wireframe geometry.

Click 1D Property in the Model Manager toolbar.

The 1D Property dialog box appears.

Name: lets you modify the name of the property.
Supports: lets you select a support.
Select Mesh Parts: this button is only available if you have selected a support.
For more details, refer to Selecting Mesh Parts.

Material: indicates you that a material has been applied.

If you do not specify a user material, the material taken into account will be the first one found, if any, on the way up from the selected geometry in the specification tree.

User-defined material: lets you select an isotropic material that you have created.
For more details, refer to Creating an User Material.
Type: lets you choose the type of section (and symbol) and define the parameters using the Component Edition button .
For more details about the Type options, refer to 1D Property Section Type.

If you select a geometry option, all the data of the user-defined beam are computed.

Orientation Geometry: you can select several geometrical elements to orient the section of a beam.

point: the orientation point gives the orientation of the Y direction for any wire frame at any point: X is fixed tangent to the wire frame and in the direction of the oriented wire frame. After computation is performed, to visualize particular axis on each element, right-click on the property set and select the Generate Image called Local axis symbol (see further below for more details).

Avoid creating an orientation point that is tangent to the line or the curve. If so, you may have some problems when computing the case.

line: when referencing a straight line the system will tend to make this line be the Y axis of the beam with the following algorithm: The X axis is always chosen as being along the element in the direction of its generation (which is the direction of the geometry). A vector direction w is extracted from the line. The cross product X*w is the Z axis and the cross product Z*X is the Y axis.

Note that, following the algorithm detailed, if the line selected is perpendicular in the right direction to the beam element, it is then the Y axis.
Note also that curved lines will not be accepted for selection because it would not make sense to extract a direction from a curved line.

direction of an axis system: you can reference one of the three directions of a design axis. The behavior is then the same as the behavior described for the line
surface: when referencing a surface the system will tend to make the Y axis of the beam perpendicular to the surface with the following algorithm: the center of gravity of the beam element will be projected on the surface on a point P. The normal to the surface at point P will be computed and will be taken as the vector direction w on which the operation described in the Lines paragraph will be computed.

Additional options available with the ELFINI Structural Analysis (EST) product:

Offset: lets you define or not offset values at each end of the beam.
- None: no offset will be defined.
- Customized: lets you customize the offset values by clicking the Component Edition button.
Released DOF: lets you release or not the degrees of freedom.
- None: no degree of freedom will be released.
- Customized: lets you choose the degrees of freedom you want to release by clicking the Component Edition button.

Variable beam factors: lets you create a linear approximation of variable cross section beams.

This option is not authorized:

with the following section types: User-defined beam, Beam from surface and Variable beam.
for discontinuous supports (e.g. a join constituted of two different lines).

If you activate this option, two new fields appear in the Beam Property dialog box.

The Multiplication Factors on Extremities frame lets you give a scaling factor on each side of the section. The beam is modeled as a sequence of constant section beams. For each beam elements, the cross sectional area is computed at the center of elements (and not at the node of elements):

symbolizes the node of elements and symbolizes the center of elements.

A₁ = A x f₁ and A₂ = A x f₂ where:

A is the specified cross-sectional area
f₁ is the Starting factor
f₂ is the Ending factor.

Select the support geometry to be applied a 1D property.

The 1D Property dialog box is updated as shown here:
Select Rectangular beam as Section option.
Click the Component Edition button in the 1D Property dialog box to define dimensions.

The Beam Definition dialog box appears.
Enter 10 mm in the Length (Y) field and 10 mm in the Height (Z) field.
Click OK in the Beam Definition dialog box.

Symbols appear on the geometry to simulate the section of the beam.
Activate the Orientation Geometry field and select a point.

The 1D Property dialog box appears as shown here:

Click OK in the 1D Property dialog box.

The 1D Property is added. In this case, 1D Prorperty.1 feature appears in the specification tree.

Creating Local 1D Property

You can associate a local section to a piece of the geometry on the condition a 1D property was previously applied to the geometry.

Only available with the ELFINI Structural Analysis (EST) product.

Right-click the 1D Property.1 property previously created in the specification tree and select Local 1D Property .

The Local 1D Property dialog box appears.

For details about the dialog box options, refer to Adding 1D Properties.

Name: lets you modify the name of the property.
Supports: lets you select a support.
Select Mesh Parts: this button is only available if you have selected a support.
For more details, refer to Selecting Mesh Parts.
Material: indicates you that a material has been applied.
User Defined Material: lets you select an user isotropic material on condition that it has been previously created.
For more details, refer to Creating an User Material.
Type: lets you choose the type of section (and symbol) and define the parameters.
For more details, refer to 1D Property Section Type.
Orientation geometry: you can select point, line or surface to orient the section of a beam.
Offset: lets you define or not offset values at each end of the beam.
Released DOF: lets you release or not the degrees of freedom.
Variable beam factors: lets you create a linear approximation of variable cross section beams.

Select the part of the geometry on which you want to apply a local 1D property.

The Local 1D Property is updated as shown here:
Change the Type option. In this particular case, select the Thin box beam option.

The geometry appears as shown here:
Click the Component Edition button in the Local 1D Property dialog box to define the dimensions of the section.

The Beam Definition dialog box appears.
Enter the following values in the different fields of the Beam Definition dialog box.
Click OK in the Beam Definition dialog box.
Select a point as Orientation Geometry.
Click OK in the Local 1D Property dialog box.

A Local 1D Property.1 property appears in the specification tree (under 1D Property.1).

Note that you can manually edit or delete 1D properties.