GuiCommand: Name: SheetMetal AddWall MenuLocation: SheetMetal , Make Wall Workbenches: SheetMetal Workbench Shortcut: W

SheetMetal AddWall

Description

The SheetMetal AddWall command creates flanges on selected edges of a base plate. By changing the angle property a flange it can be turned into a hem.

A flange consists of a 90° cylindrical bend and a planar strip (wall).

Resetting the angle property to about 180° in a second step will create a hem instead.

Usage

1. Select one or more edge(s) of a base plate.
2. There are several ways to invoke the command:
   • Press the Make Wall button.
   • Select the Sheet Metal → Make Wall option from the menu.
   • Right-click in the Tree view or the 3D view and select the Sheet Metal → Make Wall option from the context menu.
   • Use the keyboard shortcut: W.
3. The Flange Parameters Task panel opens (introduced in version 0.5.00).
4. Optionally press the Select button to add more edges.
   • Press the Preview button to finish the selection and display the changes.
5. Optionally adjust the parameters in the Task panel.
6. Press the OK button to finish the command and close the Task panel.
7. A Bend object will be created consisting of one new flange at each selected edge.
8. Optionally adjust the parameters in the Property editor.

Notes

To create a base plate use a closed 2D outline - preferably a Sketch - with the Make Base Wall command.

Alternatively a base plate (blank) can be created with commands from the Part Workbench or PartDesign Workbench.

To create a blank with the Part Workbench:

1. Create a solid using either:
   • [Part Box](wiki-test2.php?gitpage=Part_Box).
   • [Part Extrude](wiki-test2.php?gitpage=Part_Extrude) from: - A [Draft Rectangle](wiki-test2.php?gitpage=Draft_Rectangle). - A [Draft Wire](wiki-test2.php?gitpage=Draft_Wire). - A [Sketch](wiki-test2.php?gitpage=Sketcher_NewSketch).
2. Make sure one the dimensions of the Box or the extrusion distance equals the sheet metal thickness.

To create a blank with the PartDesign Workbench:

1. Create a solid using either:
   • [Additive Box](wiki-test2.php?gitpage=PartDesign_AdditiveBox).
   • [PartDesign Pad](wiki-test2.php?gitpage=PartDesign_Pad) from a [Sketch](wiki-test2.php?gitpage=Sketcher_NewSketch).
2. Make sure one the dimensions of the Box or the Length property of the Pad equals the sheet metal thickness.

If you start with a PartDesign Body, you can mix SheetMetal features with PartDesign features such as PartDesign Pocket or PartDesign Hole.

Properties

See also: Property editor.

A SheetMetal Bend object is derived from a Part Feature object or, if it is inside a PartDesign Body, from a PartDesign Feature object, and inherits all its properties. It also has the following additional properties:

Data

{{Properties_Title|Parameters}}

• Bend Type|Enumeration: \"Bend Type\". {{value|Material Outside}} (default), {{value|Material Inside}}, {{value|Thickness Outside}}, {{value|Offset}}.

• Length Spec|Enumeration: \"Type of Length Specification\". {{value|Leg}} (default), {{value|Outer Sharp}}, {{value|Inner Sharp}}, {{value|Tangential}}. (v0.21)

• angle|Angle: \"Bend Angle\". Default angle: {{value|90,00°}}.

• base Object|LinkSub: \"Base Object\". Link to the planar face to receive a bend.

• extend1|Distance: \"Extend from Left Side\". Default: {{value|0,00 mm}}.

• extend2|Distance: \"Extend from Right Side\". Default: {{value|0,00 mm}}.

• gap1|Distance: \"Gap from Left side\". Default: {{value|0,00 mm}}.

• gap2|Distance: \"Gap from Right side\". Default: {{value|0,00 mm}}.

• invert|Bool: \"Invert Bend Direction\". Default: False.

• length|Length: \"Length of Wall\". Default: {{value|10,00 mm}}.

• radius|Length: \"Bend Radius\", the default value depends on the radius property of the parent feature:

• That property is not existent: This property is set to {{value|1,00 mm}}.

• That property contains a numeric value: An expression linking that property is inserted into this property.

• That property contains an expression: The expression is copied into this property.

{{Properties_Title|Parameters Ex}}

• Auto Miter|Bool: \"Enable Auto Miter\". Default: True.

• kfactor|FloatConstraint: \"Location of Neutral Line. Caution: Using ANSI standards, not DIN.\". Default: {{value|0,50}}. K factor (also known as neutral factor) for the bend. Used to calculate bend allowance when unfolding.

• max Extend Dist|Length: \"Auto Miter maximum Extend Distance\". Default: {{value|5,00 mm}}.

• min Gap|Length: \"Auto Miter Minimum Gap\". Default: {{value|0,20 mm}}.

• min Relief Gap|Length: \"Minimum Gap to Relief Cut\". Default: {{value|1,00 mm}}.

• offset|Distance: \"Offset Bend\". Default: {{value|0,00 mm}}.

• unfold|Bool: \"Shows Unfold View of Current Bend\". Default: True unfolds the bend.

{{Properties_Title|Parameters Ex2}}

• Sketch|Link: \"Sketch Object\".

• sketchflip|Bool: \"Flip Sketch Direction\". Default: False.

• sketchinvert|Bool: \"Invert Sketch Start\". Default: False.

{{Properties_Title|Parameters Ex3}}

• Length List|FloatList: \"Length of Wall List\". Default: {{value|[10.00]}}.

• bend AList|FloatList: \"Bend Angle List\". Default: {{value|[90.00]}}.

{{Properties_Title|Parameters Miterangle}}

• miterangle1|Angle: \"Bend Miter Angle from Left Side\". Default angle: {{value|0,00°}}.

• miterangle2|Angle: \"Bend Miter Angle from Right Side\". Default angle: {{value|0,00°}}.

{{Properties_Title|Parameters Perforation}}

• Nonperforation Max Length|Length: \"Non-Perforation Max Length\". Default: {{value|5 mm}}.

• Perforate|Bool: \"Enable perforation\". Default: False.

• Perforation Angle|Angle: \"Perforation Angle\". Default: {{value|0 °}}.

• Perforation initial Length|Length: \"Initial Perforation Length\". Default: {{value|5 mm}}.

• Perforation Max Length|Length: \"Perforation Max Length\". Default: {{value|5 mm}}.

{{Properties_Title|Parameters Relief}}

• Relief Factor|Float: \"Relief Factor\". Default: {{value|0,70}}.

• Use Relief Factor|Bool: \"Use Relief Factor\". Default: False.

• relief Type|Enumeration: \"Relief Type\". {{value|Rectangle}} (default), {{value|Round}}. Enabled only when a gap value is set.

• reliefd|Length: \"Relief Depth\". Default: {{value|1,00 mm}}. Enabled only when a gap value is set.

• reliefw|Length: \"Relief Width\". Default: {{value|0,80 mm}}. Enabled only when a gap value is set.

Example

Preparation

This tray is made of a rectangular blank with walls added to its outline edges. And so one outline sketch for the blank has to be prepared in advance.

*Just a rectangular outline*

Workflow

1. Create a blank
   1. Select the outline sketch
   2. Press the or use the keyboard shortcut: (The blank is padded in z direction
2. Add walls to the outline edges
   1. Select the blank\'s outline edges
   2. Press the or use the keyboard shortcut:
   3. If the fold is 90° down set the value of invert property to true to reverse the direction (and length to a lower value for smaller walls)
3. Add some more walls
   1. Select the tray\'s upper outside edges
   2. Press the or use the keyboard shortcut:
   3. The walls are a bit too long (but nicely trimmed) and so the length property has to be set to a lower value
   4. If you like the folds swing outward set the invert value to true

Done!

⏵ documentation index > SheetMetal > Addons > External Command Reference > SheetMetal AddWall

This page is retrieved from https://github.com/FreeCAD/FreeCAD-documentation/blob/main/wiki/SheetMetal_AddWall.md