PartDesign Thickness

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Revision as of 14:54, 20 May 2022 by FBXL5 (talk | contribs) (enhanced description)
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PartDesign Thickness

Menu location
Part Design → Apply a dress-up feature → Thickness
Workbenches
PartDesign
Default shortcut
None
Introduced in version
0.17
See also
Part Thickness

Description

The text-top=Thickness PartDesign Thickness command works on a solid body and transforms it into a hollow object with at least one open face, giving to each of its remaining faces a uniform thickness. It adds a Thickness object to the document with its corresponding representation in the Tree view.

Base solid (A) → Solid with selected face to be opened (B) → Resulting hollow object (C)

Usage

Add a Thickness

  1. Optionally activate the Body to apply Thickness to (by double clicking the Tree view item).
  2. Select one or more face(s) of the active Body.
  3. There are several ways to invoke the Thickness tool:
    • Press the text-top=Thickness Thickness button.
    • Select the Part Design → Apply a dress-up feature → Thickness option from the menu.
  4. The Thickness parameters dialog will open in the Task panel and allows to set several options.
  5. Click OK to validate.


Remember:
  • Since there must be at least one face for the feature, the last remaining face in the list cannot be removed.

Edit a Thickness

  1. There are two ways to reopen the Thickness parameters dialog to edit a Thickness:
    • Double-click on the Thickness item in the Tree view
    • Right-click on the Thickness item in the Tree view and select Edit Thickness from the context menu.
  2. The Thickness parameters dialog will open in the Task panel and allows to set several options.
  3. Click OK to validate.

Options

  • Thickness: Set the desired wall thickness of the resulting object either by editing the value or by clicking on the up/down arrows.
  • Mode:
    • Skin: Select this option if you want to get an item like a vase, headless but with the bottom
    • Pipe: Select this option if you want to get an object like a pipe, headless and bottomless.
    • Recto Verso:
(In case you wonder: Pipe and Recto Verso functionality hasn't been implemented since version 0.13, see 2013 topic and 2021 follow-up)
  • Join Type:
    • Arc: Removes the outer edges and creates a fillet with a radius equal to the defined thickness.
    • Intersection: When faces are offset outward, sharp edges are kept between faces.
  • Make thickness inwards: When checked, faces are offset inward.

Properties

See also: Property editor.

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

Data

Base

  • DataBase (LinkSub): Base. Sub-link to the parent feature's list of selected edges and faces.
  • DataSupportTransform (Bool): Support Transform. "Include the base additive/subtractive shape when used in pattern features.
If disabled, only the dressed part of the shape is used for patterning. Default: false.
  • Data (hidden)AddSubShape (PartShape): Add Sub Shape.
  • Data (hidden)BaseFeature (Link): Base Feature. Link to the parent feature.
  • Data (hidden)_Body (LinkHidden): _Body. Hidden link to the parent body.

Part Design

  • DataRefine (Bool): "Refine shape (clean up redundant edges) after adding/subtracting". Default: true.

Thickness

  • DataValue (Length): Value. "Thickness value". Default: 1,00 mm.
  • DataMode (Enumeration): Mode. Skin (default), Pipe (seems to be useless).
("Recto verso" isn't even listed here...)
  • DataJoin (Enumeration): Join. "Join type".Arc (default).
  • DataReversed (Bool): Reversed. "Apply the thickness towards the solids interior". Default: false.
  • DataIntersection (Bool): Intersection. "Enable intersection-handling". Default: false.

Limitations

  • At least one face to be opened must be selected.
  • If thickness goes inwards, the value must be smaller than the smallest height of the Body.
  • The command may fail with complex shapes. In this context the surface of e.g. a cone has already to be regarded as complex.

Example

  1. Create a Pad from the sketch
  2. Create a second sketch on the XY plane
  3. Create a second Pad from the second sketch

As in the following pictures:

File:Braga-primoPad.png

File:Braga-secondoschizzo.png

File:Braga-secondo Pad.png

Then

  1. Select a circular face
  2. Select Thickness
  3. Add the other circular faces to the selection

Result:

Known Errors

  • BRep_API: command not done
  • BRep_Tool: no parameter on edge
  • Silently Fails


PartDesign
User documentation
Retrieved from "http://wiki.freecad.org/index.php?title=PartDesign_Thickness&oldid=1140339"