About the Attached Flat Wall User Interface

Sheetmetal > Sheetmetal > Designing in Sheetmetal Design > Creating and Modifying Walls > Attached Walls > Attached Flat Walls > About the Attached Flat Wall User Interface

The Flat user interface consists of commands, tabs, and shortcut menus. To access the Flat tab, click Sheetmetal >

Flat.

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—Lists wall shapes:

◦ Standard wall shapes:

▪ Rectangle—Rectangular wall

▪ Trapezoid—Trapezoidal wall

▪ L—L-shaped wall

▪ T—T-shaped wall

◦ User Defined—Select to create a new wall shape using the Shape tab.

◦ Predefined wall shapes—Saved wall sketches appear on the list when they have been accessed during the current session.

You can use the Flat_shape_sketches_directory configuration option to specify the directory path to your library of predefined flat walls shapes to appear on the list.

•

Wall Angle list—Lists predefined values, user-defined values, a flat wall option, and [<Parameter Value>] for the wall attachment angle.

—Flips the angle direction to the other side of the attachment wall.

• [<Parameter Value>] uses an angle set by the SMT_DFLT_BEND_ANGLE parameter.

• The angle between the attachment edge and surface cannot exceed 180 degrees. When you need a larger angle, use the opposite side of the sheet metal as the attachment edge.

•

—Flips the

material thickness direction.

•

—Adds a bend to the attachment edge according to a specified value. Default values are as follows:

◦ Thickness—Uses a radius equal to the thickness of the sheet metal wall.

◦ 2.0 * Thickness—Uses a radius equal to twice the thickness of the sheet metal wall.

◦ [<Parameter Value>]—Uses a radius as set 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 as set by the SMT_DFLT_RADIUS_SIDE parameter.

Tabs

• Placement—Displays the selected edge type in the collector.

• Shape—Displays the following options:

◦ Sketch—Opens the sketch in Sketcher for editing.

To change sketch references or orientation or both, click Sketch > Sketch Setup in Sketcher.

◦ Open—Opens the Open dialog box to select a saved .sec file.

◦ Save As—Opens the Save a Copy dialog box, to save the wall sketch as an .sec file in the specified directory.

◦ 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.

• Bend Position—Opens a list of offset types.

◦ Type—Sets the type of offset.

▪

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.

▪

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:

▪

Constrained—Keeps the attached wall geometry within the boundary of the attached edge.

• Relief—Sets the type of wall relief.

◦ Click the Define each side separately check box to set separately the relief for each wall 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.

▪ 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:

▪ 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.

Tangent to Bend—Creates the bend reliefs tangent to the bend.

[<Parameter Value>]—Uses the SMT_DFLT_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 SMT_DFLT_BEND_REL_LENGTH_TYPE parameter value.

▪ Relief 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.

• 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 graphics window to access the shortcut commands:

• Clear—Removes the reference from the active collector.

• Add Bend—Adds a bend at the attachment edge.

• Flip Thickness—Flips the material thickness direction.

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.

Right-click the offset handle to open the shortcut menu:

• 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.

• Offset from Bend Start—Measures the offset from the attachment edge to the Bend Start:

• Offset from Bend Apex—Measures the offset from the attachment edge to the Bend Apex:

• Constrained—Keeps the attached wall geometry within the boundary of the attached edge.

Right-click the relief handle and choose Corner Relief. Select the Define corner relief check box to open the shortcut menus:

• 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—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—Offsets the corner relief perpendicular to the bisector by a specified distance.