Draft ShapeString tutorial/ru

Introduction

In this tutorial we will discuss how to

• insert a text with the 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
• 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 to change to axometric view
• Click on 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
• Make sure object "chamfer" is selected in the tree view and press <Space> 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 Auto and choosing XY
• Insert text "FreeCAD" by
  • Click on
  • 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 object "Shapestring" is selected in the tree view
• Use Part Extrude-Tool with the parameters:
  • extrude Z=1 mm
  • make sure to tick "create solid"
  • use "OK" to finish part extrude operation
• Make sure object "Extrude" is selected in the tree view and press <Space> to toggle its visibility to be visible

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 to visible
• Choose sloped face created by chamfer operation
• Click on to insert new sketch
• Draw a line (may be horizontal or vertical, length is not of importance ...)
• Constrain one of the endpoints to be +2,5 mm vertical distance and +2,5 mm horizontal distance away from the origin
• Close the sketch

Positioning 3D text in 3D space

• Make sure object "Extrude" is selected in the tree view and press <Space> to toggle visibility to visible
• Make sure, object "Extrude" is selected in the tree view
• Open Placement task Edit->Placement...
• 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 Draft->Snapping->Snap to endpoint
• Select "extrude"-object
• Click on
• 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
• Make sure object "Sketch" is selected in the tree view
• Press <Space> to toggle visibilty
• Click on to change to axometric view
• Click on to zoom to fit all
• Finished

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)