Draft ShapeString tutorial

Introduction
In this tutorial we will discuss how to
 * insert a text with the Draft 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 [[Image:Part_Box.png|32px]]
 * 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 [[Image:View-axometric.svg|32px]] to change to axometric view
 * Click on [[Image:View-zoom-all.svg|32px]] 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 [[Image:Part_Chamfer.png|32px]]
 * Make sure object "chamfer" is selected in the tree view and press  to toggle visibility

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 and choosing
 * Insert text "FreeCAD" by
 * Click on [[Image:Draft_ShapeString.png|32px]]
 * Highlight the text in the "Global X"-field and type "0" on the keyboard and press
 * The text in the "Global Y" field is highlighted
 * Type "0" on the keyboard and press
 * The text in the "Global Z" field is highlighted
 * Type "0" on the keyboard and press
 * Enter "FreeCAD" in the string field (without brackets) and press
 * 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 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
 * Use Part Extrude-Tool [[Image:Part_Extrude.png|32px]] 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  to toggle visibility

Insert sketch for positioning

 * Switch to sketcher workbench
 * Make sure object "chamfer" is selected in the tree view and press  to toggle visibility
 * Choose sloped face created by chamfer operation
 * Click on [[Image: Sketcher_NewSketch.png|32px]] 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 sketch

Positioning 3D text in 3D space

 * Make sure object "Extrude" is selected in the tree view and press  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 [[Image: Draft_Move.png|32px]]
 * 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)

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 [[Image:Part_Cut.png|32px]]
 * Make sure object "Sketch" is selected in the tree view
 * Press  to toggle visibilty
 * Click on [[Image:View-axometric.svg|32px]] to change to axometric view
 * Click on [[Image:View-zoom-all.svg|32px]] to zoom to fit all
 * Finished