Document Properties - Sheet Metal

Lets you specify sheet metal options. Available for all document types. Options vary depending on whether you are working with a part, assembly, or drawing.

To open this dialog box:

With a part, assembly, or drawing open, click Tools > Options > Document Properties > Sheet Metal.

To show bend lines in flat patterns, do one of the following:

  • Click View > Hide/Show > Sketches.
  • In the FeatureManager design tree, expand Flat-Pattern and Flat-Pattern(n) . Right-click Bend-Lines and click Show .

Options for Parts and Assemblies

Simplify bends
Straightens curved edges in the flat pattern. When this option is not selected, complex edges remain in the flat pattern.
Simplify bends selected
Simplify bends cleared
Corner treatment Applies smooth edges in the flat pattern.
Create multiple flat patterns whenever a feature creates multiple sheet metal bodies If you use a feature to create additional bodies in a sheet metal part, each new body gets a sheet metal and flat pattern feature.

This option applies to parts created prior to SOLIDWORKS 2013. Otherwise, each body in a multibody sheet metal part has its own flat pattern.
Show form tool punches when flattened Displays the forming tool and its placement sketch in a flat pattern.

Show form tool profiles when flattened Displays the forming tool's placement sketch in a flat pattern.

Show form tool centers when flattened Displays the forming tool's center mark where the forming tool is located in a flat pattern.

Show sheet metal gusset profiles when flattened Displays gusset profiles when you flatten a sheet metal part.

Show sheet metal gusset centers when flattened Displays gusset center marks when you flatten a sheet metal part.

Options for Drawings

Flat pattern colors Lets you select colors for entities in flat patterns. You can select colors for:
  • Bend Lines - Up Direction
  • Bend Lines - Down Direction
  • Form Feature
  • Bend Lines - Hems
  • Model Edges
  • Flat Pattern Sketch Color
  • Bounding box
Display sheet metal bend notes Displays bend notes in the drawing. In Style, select the location for the bend notes. You can also right-click a flat pattern view and click Properties, and select or clear Display sheet metal bend notes.
If you select above or below the bend lines, you can also add note leaders individually or simultaneously while in the drawing document.
Leader style
  • Select: a Leader Style .
  • Select: a Leader Thickness or select Custom Size and enter a thickness.
Text
  • Font. Click to modify the font.
  • Text alignment. Select:
    • Center
    • Left
    • Right
Leader anchor Select a default anchor position:
  • Closest
  • Left
  • Right
Leader display
  • Straight
  • Bent. Inserts a horizontal bend in the leader that is aligned with the text. Select either:
    • Use document leader length. Derives Leader length from the Annotations page settings.
    • Leader length. Lets you enter the length of the unbent portion of the leader.
  • Underlined
  • Leader justification snapping. Allows the leader to snap to one side of the text.
Layer
Select a Layer .
You must first create layers for the drawing before you can select them for document properties.
Border
  • Style. Select None to display the text with no border, or select a border style.
  • Size. Select a size from the list (a specified number of characters), Tight Fit (which adjusts automatically to the text), or Custom Size (where you can set the size).
Format Lets you change the format or language for flat pattern bend notes in drawings.

For example, if you create a flat pattern view in English, the bend line notes are in English. To change the format or language of the bend line notes, set Format to Exchange, then in Tools > Options > System Options > File Locations, set Show folders for to Sheet Metal Bend Line Note File, and set the file location to the desired format or language.

To keep the same format or language for flat pattern bend notes, set Format to Keep.
Show fixed face Displays the fixed face that is defined in the flat pattern feature of the sheet metal part.
To view the fixed face, the flat pattern view must include a bend table.
Show grain direction Displays the grain direction that is defined in the flat pattern feature of the sheet metal part.
To view the grain direction, the flat pattern view must include a bend table.

New Sheet Metal Bodies

You can define the default behavior that controls whether sheet metal bodies follow the parameters defined in the Sheet-Metal folder in the FeatureManager design tree.

The following options let you control the default behavior for newly created sheet metal bodies - whether sheet metal definitions follow the Sheet-Metal folder settings or not:
  • Override default parameters
  • Override bend allowance parameters
  • Override auto relief parameters
  • Use sheet metal parameters from material. When you assign a custom material to a sheet metal part, you can link the sheet metal parameters to the material. This option uses sheet metal parameters attached to the selected material. When selected, the parameters assigned to the material apply to everything in the Sheet-Metal folder in the FeatureManager design tree.

When selected, these options override the Sheet-Metal folder parameters. In the individual sheet metal body PropertyManagers, the corresponding Override default parameters check boxes are selected. When all options are cleared, all individual body sheet metal parameters are driven by the settings in the Sheet-Metal folder.

Edge Flange Options

Automatically add Flange Length dimension to flange profiles Adds length dimensions to all edge flange profiles. The sketch dimension (not the feature dimension) controls the flange length.