SpaceClaim Online Help

Bend deduction table

Bend deduction tables are used to calculate flat pattern layouts. The tables are based on the Bend Deduction (BD) formula, which calculates the flat line length to produce a specific bend angle.

BD = 2 X OSSB - BA

Where:

• BD is Bend Deduction
• BA is the Bend Allowance that equals the arc length of the bend along the neutral line. The neutral line is the radius where the material transitions from compressive stress (inside) to tensile stress (outside)
• OSSB is the Outside Set Back. Depending on the bend angle, SpaceClaim uses two different definitions of OSSB as explained below.

For bend angles less than 90-degrees, OSSB is measured from the beginning of the bend to the Outside Mold LineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the Pull tool, lines become edges., which is the intersection of the planar faces. See the image below.

 

OSSB = Tan(A/2) X (BR + T) Hence BD = 2 X Tan(A/2) X (BR + T) - BA   Where: BR = Bend Radius T = Thickness A = Angle measured from flat (radians)

 

For bend angles greater than, or equal to, 90-degrees, the OSSB is measured from the beginning of the bend to a plane tangent to the outside bend face. This means that the OSSB is the same as the outside radius of the bend. See the image below.

 

OSSB = BR + T Hence BD = 2 X (BR + T) - BA   Where: BR = Inside Bend Radius T = Thickness A = Angle measured from flat (radians)

 NOTE:

• If a bend table is not assigned to a part, the Bend Allowance is calculated from the default K-factor found in the Sheet Metal options.
• If a bend table is assigned to a part, the Bend Allowance is obtained from the table and the assigned bend table file must specify tables for all possible combinations of part thickness and Vee Die width.
• If some bends in the part use Vee Die and other bends in the part do Not, the assigned bend table file must specify a table with no Vee Die Width entry.
• If you enter values in the Properties panelArea of the user interface that displays editable details about the selected object(s). This panel is initially displayed on the lower left side of the screen, but can be moved. for a Bend Allowance or Bend Deduction, it will override the values obtained from the bend table or computed using K-factorParameter of bends in a sheet metal part used to calculate the bend radius. K-factor is a percentage of the metal thickness and depends on factors such as the material and type of bending operation. Relates to the depth of the neutral axis; a line within the sheet where the length does not change when the sheet is bent. The inside of the bend is under compression, the outside is under tension, and the neutral axis occurs somewhere between the midpoint of the material (K-factor=0.50) and a point closer to the inside of the bend (K-factor=0.25)..
• You can set the bend deduction to a negative value to correctly represent the corresponding bend allowance.

To use a sheet metal bend table to calculate unfolded lengths

1. Copy a CSV file to the SpaceClaim LibraryYou can select from the Materials Library in the Properties panel and add them to your Local Materials./Bends folder or into a SpaceClaim Support File directory.

2. Set the bend table for a sheet metal component by selecting the component in the Structure treeDisplay in the Structure panel that shows you each of the objects in your design. You can expand or collapse the nodes of the tree to view the objects. You can rename objects, create, modify, replace, and delete objects, as well as work with components. and selecting the bend table from the Bend Table property.

All values may then be obtained from the bend table instead of being calculated. Any values not obtained from the bend table may result in an error when you unfold the design. You can clear the sheet metal bend table assignment from a component by selecting the blank value from the Bend Table property drop-down.

The table below shows a simple bend table as it would appear in a spreadsheet editor. Keywords are shown in bold. Angle Values are measured from the flat.

When you unfold a sheet metal design, the thickness, inner bend radius, and angle from the design are used to determine the value in the selected table.

Once you select a bend table, you can edit the Vee Die Width property in the Properties panelArea of the user interface that displays editable details about the selected object(s). This panel is initially displayed on the lower left side of the screen, but can be moved.. Vee die width sets the width of the tooling that produces the bend.

Comma-separated value file

Bend table files are stored as comma-separated value (CSV) files, which can be edited. The file below shows the same data as in the previous table, but as it appears when stored in the comma-separated value file.

Tables can have two types of data. In the example above, the data type is DataTypeCompensation, which is the default. The table below is an example where data type is set to DataTypeRadius.

In this table, each combination of Thickness and VeeDieWidth represents a table that provides the actual radius based on tool radius and angle. In the example above the green cells are the tool radius, blue cells are the angle, and pink cells are the actual radius applied to the geometry.

The radius table only affects bend creation. Once the bend is created the actual (table lookup) radius is stored in the bend. You can change the value later or disconnect the table without affecting the bend.

When a radius table is applied, Bend creation changes slightly. In the Sheet Metal Options panel, Die width is a dropdown list. The Bend radius text box label is changed to Tool radius and the input dynamically changes to a dropdown list if the following conditions are met.

• One or more edges of a sheet metal part are selected
• The selected edge is in a part that references a bend table file
• The bend table file contains a table that matches the part's thickness and selected vee die width

Keyword description parameters for bend tables