About the Flange Wall User Interface
The Flange user interface consists of commands, tabs, and shortcut menus. To access the Flange tab, click > 
Flange.
Flange.Use the following configuration options to control the default values and behavior of selected tool settings:
• smt_drive_tools_by_parameters—Uses parameter values as the default values of selected tool settings and to automatically update features when parameter values change.
• smt_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 smt_drive_bend_by_parameters, you must also set smt_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 walls shapes to appear on the list. |
• Flange Length buttons—Determines the location of each end of the flange wall:
◦ 
—Sets the wall end at the chain end.
—Sets the wall end at the chain end.◦ 
and 
—Trims or extends the wall end from the chain end by a specified value.
and —Trims or extends the wall end from the chain end by a specified value.◦ 
—Trims or extends the wall end to a selected point, curve, plane, or surface.
—Trims or extends the wall end to a selected point, curve, plane, or surface.• The following additional options are available only for extruded flange walls:
◦ 
—Extrudes the wall symmetrically in both directions.
—Extrudes the wall symmetrically in both directions.◦ 
—Does not extrude the wall in this direction.
—Does not extrude the wall in this direction.• Settings options:
◦ 
Thickness Side—Changes the thickness to the other side of the profile.
Thickness Side—Changes the thickness to the other side of the profile.• Bend Dimensions options:
◦ 
—Adds a bend at the attachment edge. Default values are as follows:
—Adds a bend at the attachment edge. Default values are as follows:▪ Thickness—Uses a default radius equal to the thickness of the sheet metal wall.
▪ 2.0 * Thickness—Uses a default radius equal to twice the thickness of the sheet metal wall.
▪ [<Parameter Value>]—Adds a bend defined by the SMT_DFLT_BEND_RADIUS parameter.
◦ When you add a bend the Dimension Location buttons are available:
▪ 
—Dimensions the radius according to the inside surface of the wall.
—Dimensions the radius according to the inside surface of the wall.▪ 
—Dimensions the radius according to the outside surface of the wall.
—Dimensions the radius according to the outside surface of the wall.▪ 
—Dimensions the radius according to the location controlled by the SMT_DFLT_RADIUS_SIDE parameter.
—Dimensions the radius according to the location controlled by the SMT_DFLT_RADIUS_SIDE parameter.Tabs
• Placement—Displays the selected edge type in the collector.
◦ Details—Opens the Chain dialog box that displays the selected edge reference.
| | For more information on chains, search the Help Center. |
◦ Allow automatic segment exclusion—Select this check box to create a corner instead of an excluded segment. This prevents a failure of wall regeneration when the fillet of the wall removes a small segment of the referenced chain.
• 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 wall sketch as an .sec file.
◦ Shape attachment—Determines how the wall is dimensioned:
Height dimension includes thickness—Includes sheet metal thickness when calculating wall height.
Height dimension does not include thickness—Does not include sheet metal thickness when calculating wall height.
Section Preview—Click to open the Sketch window to preview and edit the sketch dimensions.
◦ Add bends on sharp edges—Adds bends on any sharp edges.
◦ Flip profile—Flips the wall orientation along the attachment edge.
| | To make the command available on the Flange wall Shape tab and shortcut menu, set the smt_allow_flip_sketch configuration option to yes. |
• Length—Specifies how the wall length is determined:
◦ 
Chain end—Sets the flange end at the chain end.
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.
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.
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 walls:
◦ Symmetric—Extrudes the wall symmetrically in both directions.
Symmetric—Extrudes the wall symmetrically in both directions.◦ None—Does not extrude the flange wall in this direction.
None—Does not extrude the flange wall in this direction.• Bend Position—Opens a list of offset types.
| | Available only when a bend is added to the attachment edge. |
◦ Type—Sets the type of offset.
▪ 
Profile on Edge—Adds bend geometry while keeping the wall profile on the original attachment edge.
Profile on Edge—Adds bend geometry while keeping the wall profile on the original attachment edge.▪ 
Bend Outside—Adds bend geometry with the bend line tangent to the attachment edge.
Bend Outside—Adds bend geometry with the bend line tangent to the attachment edge.▪ 
Offset from Bend Start—Measures the offset from the attachment edge to the Bend Start:
Offset from Bend Start—Measures the offset from the attachment edge to the Bend Start:Value—Type an offset value in the box or choose from a list of previously used values. Use a positive value to add to the attachment segment by the specified value. Use a negative value to trim the attachment segment by the specified value.
▪ 
Offset from Bend Apex—Measures the offset from the attachment edge to the Bend Apex:
Offset from Bend Apex—Measures the offset from the attachment edge to the Bend Apex:Value—Type an offset value in the box or choose from a list of previously used values. Use a positive value to add to the attachment segment by the specified value. Use a negative value to trim the attachment segment by the specified value.
▪ 
Constrained—Keeps the attached wall geometry within the boundary of the attached edge.
Constrained—Keeps the attached wall geometry within the boundary of the attached edge.• Corner Treatment—Specifies the type of edge rip and the dimensions for a pair of adjacent wall segments. The edge rip is created with reference to the offset wall and not the attachment edge. Where available, set any dimensions. Select one of the following options:
◦ Open—Creates a standard open edge rip.
| | An open type of edge rip is applicable only for a concave vertex. |
You can select the Narrow the corner check box to completely close the corner.
◦ Gap—Creates a gap along the edge rip according to a specified dimension.
◦ Blind—Creates a blind edge rip according to a specified dimension.
◦ Overlap—Creates a standard overlapping edge rip.
Flip—Reverses the overlap direction.
Add Gap—Adds a space between the edges by a specified value.
◦ [<Parameter Value>]—Creates a rip whose type is controlled by the SMT_DFLT_EDGE_TREA_TYPE parameter.
| | You can set the seam type and any required dimensions for Gap, Blind, and Overlap in the Seam area of the Sheetmetal Preferences dialog box or in the Parameters dialog box. |
• Miter Cuts—Adds miter cuts between a pair of wall segments with overlapping geometry.
Click the Add miter cuts check box to set the following options:
◦ Offset Value—Offsets the miter cut between the two adjacent edges.
◦ Cut Width—Sets the width of the miter cut.
◦ Keep all deformation areas—Maintains all the deform areas created by the bends.
| | You can set the miter cut type and any required dimensions in the Miter Cuts area of the Sheetmetal Preferences dialog box or in the Parameters dialog box. |
• Relief—Sets the type of wall relief.
◦ When Relief Category is set to Bend Relief, the following options are available:
Click the Define each side separately check box to set the bend relief for each wall end separately.
▪ Side 1—Sets the bend relief for the start point of the attachment edge.
▪ Side 2—Sets the bend relief for the end point of the attachment edge.
Type—Lists the types of bend relief available. Depending on the type of relief, other selections become available.
No Relief | Adds no relief. |
Rip | Adds a rip relief. |
Stretch | Adds a stretch relief. |
Rectangular | Adds a rectangular relief. |
Obround | Adds an obround relief. |
[<Parameter Value>] | Adds a relief whose type is controlled by the SMT_DFLT_BEND_REL_TYPE parameter. |
When the Bend Relief type is set to Rectangular or Obround, you can set values for the following options:
▪ Bend 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.
Tangent to Bend—Creates the bend reliefs tangent to the bend.
[<Parameter Value>]—Uses the SMT_DFLT_BEND_REL_DEPTH_TYPE parameter value.
▪ Bend 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 SMT_DFLT_BEND_REL_LENGTH_TYPE parameter value.
▪ Bend width:
Thickness—Use a default width that is equal to the thickness of the sheet metal wall.
2.0 * Thickness—Use a default width that is twice the thickness of the sheet metal wall.
[<Parameter Value>]—Uses the SMT_DFLT_BEND_REL_WIDTH parameter value.
Type a value—Use the absolute value that you type in the box.
◦ When Relief Category is set to Corner Relief and the Define corner relief check box is selected, the following options are available to define corner relief:
▪ Create relief geometry—Creates the corner relief geometry in the feature. The reliefs can be referenced. When you clear the Create relief geometry check box, the relief is created only during the unbend and flat pattern operations.
▪ Type—Lists available types of corner relief.
No Relief | Adds no corner relief. |
V Notch | Retains the default V notch characteristic of the corner. |
Normal | Adds a relief from the corner up to and normal to the bend end. |
Circular | Adds a circular-shaped relief. |
Square | Adds a square-shaped relief. |
Rectangular | Adds a rectangular-shaped relief. |
Obround | Adds an obround-shaped relief. |
[<Parameter Value>] | Adds corner relief as set by the SMT_DFLT_CRNR_REL_TYPE parameter. |
▪ Origin—Defines the attachment point of the relief:
Corner point—Places the relief at the point where the bend attachment edges intersect.
Bend lines intersection—Places the relief at the point where the bend lines intersect.
▪ Orientation—Defines the orientation reference of the corner relief.
Bisector—Aligns the corner relief with the bisector of the angle between the two bend edges.
Diagonal—Aligns the corner relief with the diagonal line connecting the intersection points of the bend edges and the bend lines.
▪ Additional dimensioning and placement options are available for Circular, Square, Rectangular, and Obround relief:
| | You can set any required dimensions in the Relief area of the Preferences dialog box or using sheet metal parameters. |
Corner Relief Dimension options—Sets the width and depth of the corner relief.
Rotate about origin—Rotates the corner relief about the origin by a specified value. The following table details the point of rotation for the different types of relief:
Relief Type | Rotation Point |
|---|---|
Circular | Center of circle |
Square | Center of square |
Rectangular | Midpoint of rectangle width |
Obround | Center of circle |
[<Parameter Value>] | Coordinate system defined for the SMT_DFLT_CRNR_REL_TYPE parameter |
Offset perpendicular to orientation—Offsets the corner relief perpendicular to the bisector by a specified distance.
• Bend Allowance
Use this tab to set a feature-specific bend allowance to calculate the developed length of the bend.
◦ Use part settings—Uses the developed length calculation set for the part.
◦ Use feature settings—Uses the developed length calculation defined below.
▪ By K factor—Calculates the developed length according to the K factor. To change the value for K factor, type a new factor value or select a value from the list.
▪ By Y factor—Calculates the developed length according to the Y factor. To change the value for Y factor, type a new factor value or select a value from the list.
▪ By bend table—Calculates the developed length using a bend table. To choose a different bend table, select one from the list.
• Properties—Displays the feature information:
◦ Name—Shows a default name for the wall.
◦ 
—Shows feature information in a browser.
—Shows feature information in a browser.Shortcut Menus
Right-click in the graphics window to open the mini toolbar and shortcut menu:
• Profile on Edge—Adds bend geometry while keeping the wall profile on the original attachment edge.
Profile on Edge—Adds bend geometry while keeping the wall profile on the original attachment edge.• Bend Outside—Adds bend geometry with the bend line tangent to the attachment edge.
Bend Outside—Adds bend geometry with the bend line tangent to the attachment edge.• Offset from Bend Start—Measures the offset from the attachment edge to the Bend Start:
Offset from Bend Start—Measures the offset from the attachment edge to the Bend Start:Value—Type an offset value in the box or choose from a list of previously used values. Use a positive value to add to the attachment segment by the specified value. Use a negative value to trim the attachment segment by the specified value.
• Offset from Bend Apex—Measures the offset from the attachment edge to the Bend Apex:
Offset from Bend Apex—Measures the offset from the attachment edge to the Bend Apex:Value—Type an offset value in the box or choose from a list of previously used values. Use a positive value to add to the attachment segment by the specified value. Use a negative value to trim the attachment segment by the specified value.
• Constrained—Keeps the attached wall geometry within the boundary of the attached edge.
Constrained—Keeps the attached wall geometry within the boundary of the attached edge.• 
Edit Seam—Click and then click again to display corner seam options. arrow and choose an different option from the list. Click to exit corner seam edit mode.
Edit Seam—Click and then click again to display corner seam options. arrow and choose an different option from the list. Click to exit corner seam edit mode.• 
Edit Corner Relief—Click and then click again to display corner relief edit options. Click the arrow and choose an different option from the list. Click to exit corner relief edit mode.
Edit Corner Relief—Click and then click again to display corner relief edit options. Click the arrow and choose an different option from the list. Click to exit corner relief edit mode.• 
Edit Bend Relief—Click and then click again to display bend relief edit options. Click the arrow and choose an different option from the list. Click 
to edit each side separately. Click to exit corner relief edit mode.
Edit Bend Relief—Click and then click again to display bend relief edit options. Click the arrow and choose an different option from the list. Click to edit each side separately. Click to exit corner relief edit mode.• Clear—Clears the selected references.
• Add Bend check box—Clear the check box to remove the bend.
• Flip Thickness—Flips the thickness to the other side of the sketch plane.