PartDesign Draft: Difference between revisions

From FreeCAD Documentation
(a more recent approach on displaying the usage section, but too shy to remove images or special cases paragraph)
(enhanced description)
Line 22: Line 22:


<!--T:2-->
<!--T:2-->
This tool creates angular draft on the selected faces of an object. A new separate Draft entry (followed by a sequential number if there are already existing drafts in the document) is created in the Project tree.
The [[Image:PartDesign_Draft.svg|16px|text-top=Draft|link=PartDesign_Draft]] [[PartDesign_Draft|PartDesign Draft]] command creates angular draft on the selected faces of an object. It adds a '''Draft''' object to the document with its corresponding representation in the [[Tree_view|Tree view]].


<!--T:9-->
<!--T:9-->

Revision as of 14:54, 20 May 2022

Other languages:

PartDesign Draft

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

Description

The text-top=Draft PartDesign Draft command creates angular draft on the selected faces of an object. It adds a Draft object to the document with its corresponding representation in the Tree view.

Select one or more faces on the object before starting the tool. Here, 2 faces have been selected.
Showing Draft Parameter in TaskPanel.
2 faces have been added, and a 10 deg. draft applied. The bottom plane has remained dimensionally stable, while the draft has made the top plane smaller.
The Neutral Plane has been changed to the Top Surface. Now, the top plane has stayed dimensionally stable, while the draft has made the bottom plane larger.
Pull direction is set to the lower right edge, resulting in the draft pulling to the left.
Checking the Reverse Direction box has applied an inward draft rather than outward.

Usage

Add a Draft

  1. Optionally activate the Body to draft (by double clicking the Tree view item).
  2. Select one or more face(s) on the active Body.
  3. There are several ways to invoke the Draft tool:
    • Press the text-top=Draft Draft button.
    • Select the Part Design → Apply a dress-up feature → Draft option from the menu.
  4. The Draft 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 Draft

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

Options

  • Draft angle: Set the Draft angle either by entering a value or by clicking on the up/down arrows. The applied draft angle is shown in real time.
  • Add: Add faces to the selection by pressing the Add button and selecting more faces.
  • Remove: Choose a way to remove faces from the selection:
    • Select each face in the list of the dialog and press the DEL key or right-click in the list and select Remove from the context menu.
    • Press the Remove button. All faces being previously selected are highlighted in purple. Select each face to be removed.
  • Neutral plane: Set the the neutral plane by pressing the Neutral plane button and selecting the plane that must not change dimensionally. The change is made in real time.
  • Pull direction: Set the the pull direction by pressing the Pull direction button, then select an edge. Pull Direction is only effective if the Neutral Plane has been set. Results can be unpredictable.
  • Reverse pull direction: invert the pull direction by checking the Reverse pull direction checkbox. This will toggle the draft between positive and negative angles.

Special Cases

The Draft tool will only function on faces that are normal to each other. If there are any tangential faces attached to the face you wish to apply draft to, it will fail. A common cause of failure is attempting to apply draft to a face that already has a fillet or chamfer applied to it. In this case, remove the tangential surface, apply the draft as need, then re-apply the fillet or chamfer.

Properties

See also: Property editor.

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

Data

Base

  • DataAngle (Angle): Angle. Default: 1,50 °.
  • DataReversed (Bool): Reversed. Default: false.
  • 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.

Draft

  • DataNeutralPlane (LinkSub): Neutral Plane. Sub-link to the parent feature's list containing the neutral plane.
  • DataPullDirection (LinkSub): Pull Direction.

Part Design

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


PartDesign
User documentation
Retrieved from "http://wiki.freecad.org/index.php?title=PartDesign_Draft&oldid=1140338"