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This page is a translated version of the page SheetMetal Extrude and the translation is 3% complete.

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SheetMetal Extrude.svg SheetMetal Extrude

Menu location
SheetMetal → Extend Face
Workbenches
SheetMetal
Default shortcut
E
Introduced in version
-
See also
None

Description

The SheetMetal Extrude.svg SheetMetal Extrude command extends a sheet metal plate at a selected edge face.

It creates a simple extension along the face normal of the selected edge face:

SheetMetal Extrude-01.png Button right.svg SheetMetal Extrude-02.png


If an outline sketch is added it creates interlocking geometry to close a profile:

SheetMetal Extrude-05.png Button right.svg SheetMetal Extrude-04.png

Three profiles with outline sketches to add → three results

Usage

Simple Extension

  1. Select one or more edge face(s) to be extended.
  2. Activate the SheetMetal Extrude.svg SheetMetal Extrude command using one of the following:
    • The SheetMetal Extrude.svg Extend Face button.
    • The SheetMetal → SheetMetal Extrude.svg Extend Face menu option.
    • The keyboard shortcut: E.
  3. Change the value of the property DANElength to adjust the length of the extension.

Interlocking Extension

  1. Select one edge face to be extended.
  2. Activate the SheetMetal Extrude.svg SheetMetal Extrude command (see above).
  3. Add a coplanar outline sketch to the property DANESketch.
  4. Set the property DANEUse Subtraction to true to create cut-outs to make room for the extensions.
  5. Set the property DANEOffset to adjust the clearance around the extension.

SheetMetal Extrude-03.png Button right.svg SheetMetal Extrude-05.png Button right.svg SheetMetal Extrude-06.png Button right.svg SheetMetal Extrude-04.png

Three profiles → position of the sketches → results without cut-outs → final results

Notes

  • A sketch can contain more than one outline.
After inserting a sketch, at least one of its outlines must at least touch one opposite face or the tool will fail to create any extension or cut-out.
Just one outline touching an opposite face is enough to create extension geometry from all outlines of the sketch.
  • Each cut-out will have a cuboid shape, no matter what shape the corresponding outline sketch is.
  • Shapes other than rectangles may behave little bit strange and even though the object can be unfolded, the result will not turn out as expected.

SheetMetal Extrude-07.png Button right.svg SheetMetal Extrude-08.png

Three outline sketches and their resulting extensions: separate triangle plate with a rectangular cut-out, circle without clearance → unfold solid is split at an unexpected position

  • In an extension operation it is recommended to leave the property DANERefine set to true (default).

Properties

See also: Property editor.

A SheetMetal Extend object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

Base

  • DANELabel (String): Default value: Extend (+ a sequential number for second and following items).
    The user editable name of this object, it may be any arbitrary UTF8 string.
  • DANE (hidden)Base Feature (Link): Base Feature. Link to the parent feature.
  • DANE (hidden)_Body (LinkHidden): Hidden link to the parent body.

Parameters

  • DANEbase Object (LinkSub): "Base object". Link to the planar face to be extended.
  • DANEgap1 (Distance): "Gap from the left side". Default: 0,00 mm.
  • DANEgap2 (Distance): "Gap from the right side". Default: 0,00 mm.
  • DANElength (Length): "Length of Wall". Default: 10,00 mm.

Parameters Ext.

  • DANEOffset (Distance): "Offset for subtraction". Default: 20,00 µm.
  • DANERefine (Bool): "Use Refine". Default: true.
  • DANESketch (Link): "Wall Sketch".
  • DANEUse Subtraction (Bool): "Use Subtraction". Default: false