Sheetmetal > Designing in Sheetmetal Design > Creating and Modifying Walls > Attached Walls > Flange Walls > About the Flange Wall User Interface
  
About the Flange Wall 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:
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 End Location buttons—Determines the location of each end of the flange wall:
—Sets the wall end at the chain end.
—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.
The following additional options are available only for extruded flange walls:
—Extrudes the wall symmetrically in both directions.
—Does not extrude the wall 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 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.
Dimension Location buttons:
—Dimensions the radius according to the outside surface of the wall.
—Dimensions the radius according to the inside surface of the wall.
—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.
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.
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 wall profile to the other wall edge.
Length—Specifies how the wall 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 walls:
Symmetric—Extrudes the wall symmetrically in both directions.
None—Does not extrude the flange wall in this direction.
Blind—Extrudes the wall in the first direction from the sketching plane by a specified value.
Offset—Sets the offset of the wall from the attachment edge.
 
* Available only when a bend is added to the attachment edge.
Click the Offset wall with respect to attachment edge check box to activate the following options:
Add to part edge—Adds the wall to the attachment edge without trimming the height of the attachment wall.
Automatic—Offsets the new wall, maintaining the original height of the attachment wall.
By value—Offsets the wall by a specified value.
Positive value—Adds to the attachment wall by the specified value.
Negative value—Trims the attachment wall by the specified value.
Edge 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 Close 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 edge treatment type and any required dimensions for Gap, Blind, and Overlap in the Edge Treatment 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:
Cut Width box—Sets the width of the miter cut.
Offset—Offsets the miter cut between the two adjacent edges.
Keep all deform 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.
Thickness * 2—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.
Circular
Adds a circular-shaped relief.
Rectangular
Adds a rectangular-shaped relief.
Obround
Adds an obround-shaped relief.
Square
Adds a square-shaped relief
Normal
Adds a relief from the corner up to and normal to the bend end.
[<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, Rectangular, Obround and, Square relief:
 
* You can set the 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—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
Rectangular
Midpoint of rectangle width
Obround
Center of circle
Square
Center of square
[<Parameter Value>]
Coordinate system defined for the SMT_DFLT_CRNR_REL_TYPE parameter
Offset—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.
Shortcut Menus
Right-click the selected wall 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 sheet metal wall 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 wall to the attachment edge without trimming the height of the attachment wall.
Automatic Offset—Offsets the new wall, maintaining the original height of the attachment wall.
By Value—Offsets the wall by specified value.
Right-click a handle on the flange end to access the following commands:
Chain End—Creates the wall up to the end of the attachment wall.
Blind—Trims or extends the swept wall in either direction from the chain end by a specified value.
To Selected—Trims or extends the swept wall in either direction to a selected point, curve, plane, surface, axis, or edge.
Symmetric—Extrudes the wall symmetrically in both directions.
None—Does not extrude the wall in this direction.
Right-click the Relief handle and choose Edit Relief to access the following commands:
No Relief—Adds no bend relief.
Rip—Adds a rip relief.
Stretch—Adds a stretch 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 wall relief for each wall 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 wall.
Outside Radius—Dimensions the radius according to the outside radius of the wall.
[<Parameter Value>]—Dimensions the bend radius according to the dimension location controlled by the SMT_DFLT_RADIUS_SIDE parameter.