Base ExampleCommandModel.png Tutorial

Topic
ShapeString (Draft workbench)
Level
Beginner
Time to complete
30 minutes
Author
r-frank
FreeCAD version
0.16.6704
Example File(s)


Introduction

In this tutorial we will discuss how to

  • insert a text with the Draft ShapeString.png ShapeString tool
  • extrude it to be a solid
  • position it in 3D space using placement and Draft Move with sketches as helper elements
  • doing an engraving by applying a boolean cut

It is recommended to have completed the sketcher tutorial first.

Creating the basic shape

  • Start FreeCAD and create a new document
  • Switch to part workbench
  • Insert a cube by clicking on Part Box.png
  • Make sure the cube is selected in the tree view
  • Change width to be 31 mm by using the data-tab in the property view
  • Click on View-axometric.png to change to axometric view
  • Click on View-zoom-all.png to zoom to fit all
  • Select upper edge on the front face of the cube in 3D view
  • Apply a chamfer (to Edge6) of 5 mm by clicking on Part Chamfer.png
  • Make sure object "chamfer" is selected in the tree view and press <Space> to toggle visibility

TutorialDraftShapeString BasicShape.jpg

Inserting text with the Draft ShapeString tool

  • Switch to Draft workbench
  • make sure nothing is selected in the tree view
  • Toggle working plane to XY (Top) by clicking on Draft SelectPlane.png Auto and choosing XY
  • Insert text "FreeCAD" by
    • Click on Draft ShapeString.png
    • Highlight the text in the "Global X"-field and type "0" on the keyboard and press Return
    • Highlight the text in the "Global Y" field
    • Type "0" on the keyboard and press Return
    • Highlight the text in the "Global Z" field
    • Type "0" on the keyboard and press Return
    • Enter "FreeCAD" in the string field (without brackets) and press Return
    • Choose a height of 5mm
    • Choose a tracking of 0 mm
    • now point FreeCAD to a "TTF"-Text-Font to use (for example the ARIAL-TTF)
    • After pressing Return one last time, the Draft-Shapestring object is created in the tree view

Create 3D text

  • Switch to part workbench
  • Make sure the Draft Shapestring object view is selected in the tree view
  • Use Part Extrude-Tool Part Extrude.png with the parameters:
    • extude Z=1 mm
    • make sure to tick "create solid"
  • Make sure object "Extrude" is selected in the tree view and press <Space> to toggle its visibility

TutorialDraftShapeString DraftShapestring.jpg

Insert sketch for positioning

  • Switch to sketcher workbench
  • Make sure object "chamfer" is selected in the tree view and press <Space> to toggle its visibility
  • Choose sloped face created by chamfer operation
  • Click on Sketcher NewSketch.png to insert new sketch
  • Draw a line (may be horizintal or vertical, length is not of importance ...)
  • Constrain one of the endpoints to be +2,5 mm vertical distance and +2 mm horizontal distance away from the origin
  • Close the sketch

TutorialDraftShapeString Sketch.jpg

Positioning 3D text in 3D space

  • Make sure object "Extrude" is selected in the tree view and press <Space> to toggle visibility
  • Make sure, object "Extrude" is selected in the tree view
  • Apply incremental placement, axis of rotation Z=90°
  • Apply incremental placement, axis of rotation Y=45°
  • Switch to draft workbench
  • Switch to wireframe mode
  • Make sure, only "snap to endpoint" is activated
  • Select "extrude"-object
  • Click on Draft Move.png
  • In 3D view click on the most upper left corner point of "extrude"-object (1) and then click on the constrained point in the sketch (2)

TutorialDraftShapeString Position.jpg

Creating engraved text

  • Switch to part workbench
  • Switch to "As is"-view mode
  • Select the 3D text ("extrude") and then the base object ("chamfer") in the tree view
  • Apply a boolean cut by clicking on Part Cut.png
  • Make sure object "Sketch" is selected in the tree view
  • Press <Space> to toggle visibilty
  • Click on View-axometric.png to change to axometric view
  • Click on View-zoom-all.png to zoom to fit all
  • Finished

TutorialDraftShapeString Complete.jpg

Notes

  • for creating curved text you can use the macro Circular Text
  • for importing text from inkscape look at the Importing text from inkscape tutorial
  • Extrusion of the Shapestring-Text can also be done with the PartDesign-Pad-Tool
  • Remember that the DraftShapestring-Object cannot be attached to a face (so no pocket-command possible)
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