ECAD > Working With ECAD Assemblies > Creating and Modifying Board Segments > Creating Board Segments > Creating Attached Flat, Flange, and Twist Segments > About the Flange Segment User Interface
  
About the Flange Segment User Interface
The Flange user interface consists of commands, tabs, and shortcut menus. To access the Flange tab, click Model > Flange.
Use the following configuration options to control the default values and behavior of selected tool settings:
board_drive_tools_by_parameters—Uses parameter values as the default values of selected tool settings and to automatically update features when parameter values change.
board_drive_bend_by_parameters—Uses parameter values to control the default value of bend angle and bend dimension location settings and to automatically update features when parameter values change.
 
* If you want to enable board_drive_bend_by_parameters, you must also set board_drive_tools_by_parameters to yes.
In the following descriptions, [<Parameter Value>] indicates that tool settings are controlled by parameters.
Commands
Shape list—Includes standard flange shapes and a user-defined option.
 
* You can use the flange_shape_sketches_directory configuration option to specify the directory path to your library of predefined flange shapes to appear on the list.
Flange End Location buttons—Determines the location of each end of the flange segment:
—Sets the segment end at the chain end.
—Trims or extends the segment end from the chain end by a specified value.
—Trims or extends the segment end to a selected point, curve, plane, or surface.
The following additional options are available only for extruded flange segments:
—Extrudes the segment in the first direction from the sketch plane by a specified value.
—Extrudes the segment symmetrically in both directions.
—Does not extrude the segment in this direction.
—Flips the material thickness direction.
—Adds a bend at the attachment edge. Default values are as follows:
Thickness—Uses a default radius equal to the thickness of the segment.
2.0 * Thickness—Uses a default radius equal to twice the thickness of the segment.
[<Parameter Value>]—Adds a bend defined by the BOARD_BEND_RADIUS parameter.
Dimension Location buttons:
—Dimensions the radius according to the outside surface of the segment.
—Dimensions the radius according to the inside surface of the segment.
—Dimensions the radius according to the location controlled by the BOARD_RADIUS_SIDE parameter.
Tabs
Placement—Displays the selected edge type in the collector.
Shape—Displays the following options:
Sketch—Opens Sketcher to edit the sketch.
Open—Opens the Open dialog box and displays .sec files.
Save As—Opens the Save a Copy dialog box to save the segment sketch as an .sec file.
Shape attachment—Determines how the segment is dimensioned:
Height dimension includes thickness—Includes segment thickness when calculating the height.
Height dimension does not include thickness—Does not include segment thickness when calculating the height.
Sketch window—Displays a window to preview and edit the sketch dimensions.
Add bends on sharp edges—Adds bends on any sharp edges.
Flip profile—Flips the segment profile to the other segment edge.
Length—Specifies how the segment length is determined:
Chain End—Sets the flange end at the chain end.
Blind—Trims or extends the flange end from the chain end by a specified value.
To Selected—Trims or extends the flange end to a selected point, curve, plane, or surface.
The following additional options are available only for extruded flange segments:
Symmetric—Extrudes the segment symmetrically in both directions.
None—Does not extrude the flange segment in this direction.
Blind—Extrudes the segment in the first direction from the sketching plane by a specified value.
Offset—Sets the offset of the segment from the attachment edge.
 
* Available only when a bend is added to the attachment edge.
Click the Offset segment with respect to attachment edge check box to activate the following options:
Add to part edge—Adds the segment to the attachment edge without trimming the height of the attachment segment.
Automatic—Offsets the new segment, maintaining the original height of the attachment segment.
By value—Offsets the segment by a specified value.
Positive value—Adds to the attachment segment by the specified value.
Negative value—Trims the attachment segment by the specified value.
Relief—Sets the type of relief.
Click the Define each side separately check box to set separately the relief for each segment end.
Side 1—Sets the relief for the start point of the attachment edge.
Side 2—Sets the relief for the endpoint of the attachment edge.
Type—Lists the types of relief available. Depending on the type of relief, other selections become available:
No Relief—Adds no relief.
Slit
—Adds a slit relief.
Rectangular—Adds a rectangular relief.
Obround—Adds an obround relief.
[<Parameter Value>]—Adds a relief whose type is controlled by the BOARD_BEND_REL_TYPE parameter.
When the Bend Relief type is set to Rectangular or Obround, you can set values for the following options:
Relief depth:
Blind—Creates a the bend reliefs with a depth set in the box below.
Up to Bend—Creates the bend reliefs up to the bend line.
[<Parameter Value>]—Uses the BOARD_BEND_REL_DEPTH_TYPE parameter value.
Relief length:
Blind—Creates the bend reliefs with a length of the specified value.
To Next—Creates the bend reliefs with a length to the next surface.
Through All—Creates the bend reliefs through all surfaces.
[<Parameter Value>]—Uses the BOARD_BEND_REL_LENGTH_TYPE parameter value.
Relief width:
Thickness—Use a default width that is equal to the thickness of the sheet metal wall.
Thickness * 2—Use a default width that is twice the thickness of the sheet metal wall.
[<Parameter Value>]—Uses the BOARD_BEND_REL_WIDTH parameter value.
Type a value—Use the absolute value that you type in the box.
Bend Allowance—Sets the bend allowance.
Select an option from the Developed length calculation list:
Use part settings—Uses the part's bend allowance settings to calculate the developed length for the feature.
Use feature settings—Uses the feature bend allowance settings to calculate the developed length for the feature.
By K factor—Calculates the developed length using the K factor.
By Y factor—Calculates the developed length using the Y factor.
Factor Value Input list.
Use bend table—Calculates develop length for arcs using a bend table from the list.
Properties—Displays the feature information:
Name—Shows a default name for the segment.
—Shows feature information in a browser.
Shortcut Menus
Right-click the selected segment to access the following commands:
Clear—Removes the reference in the active collector.
Add Bend—Adds a bend at the attachment edge.
Flip Profile—Flips the profile to the other edge.
Flip Thickness—Flips the material thickness direction.
Add Offset—Adds the new segment offset to the attachment edge according to the value specified.
Right-click the Offset handle to access the following commands:
Add to part edge—Adds the segment to the attachment edge without trimming the height of the attachment segment.
Automatic Offset—Offsets the new segment, maintaining the original height of the attachment segment.
By Value—Offsets the segment by specified value.
Right-click a handle on the flange end to access the following commands:
Chain End—Creates the segment up to the end of the attachment segment.
Blind—Trims or extends the swept segment in either direction from the chain end by a specified value.
To Selected—Trims or extends the swept segment in either direction to a selected point, curve, plane, surface, axis, or edge.
Symmetric—Extrudes the segment symmetrically in both directions.
None—Does not extrude the segment in this direction.
Right-click the Relief handle and choose Edit Relief to access the following commands:
No Relief—Adds no bend relief.
Slit—Adds a slit relief to the bend.
Rectangular—Adds a rectangular relief to the bend.
Obround—Adds an obround relief to the bend.
Define each side separately—Sets the type of relief for each end separately.
Exit Edit Relief—Makes the change and exits the Edit Relief menu.
Right-click the Dimension Location handle to open the shortcut menu:
Inside Radius—Dimensions the radius according to the inside radius of the segment.
Outside Radius—Dimensions the radius according to the outside radius of the segment.
[<Parameter Value>]—Dimensions the bend radius according to the dimension location controlled by the BOARD_RADIUS_SIDE parameter.