Draft ShapeString tutorial

From FreeCAD Documentation
Revision as of 08:06, 23 November 2019 by Vocx (talk | contribs) (Partial rewrite of the tutorial. Will be finished later.)
Tutorial
Topic
Product design
Level
Beginner
Time to complete
30 minutes
Authors
r-frank
FreeCAD version
0.17 and above
Example files
Draft_Shapestring_Text
See also
None

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 understand the basics of the Sketcher Workbench as well.

Setup

1. Open FreeCAD, create a new empty document with File → New, and switch to the Part Workbench.

1.1. Press the View isometric button, or press 0 in the numerical pad of your keyboard, to change the view to isometric to visualize the 3D solids better.
1.2. Press the View fit all button whenever you add objects in order to pan and zoom the 3D view so that all elements are seen in the view.
1.3. Hold Ctrl while you click to select multiple items. If you selected something wrong or want to de-select everything, just click on empty space in the 3D view.

Create the basic shape

2. Insert a primitive cube by clicking on Box.

2.1. Select Cube in the tree view.
2.2. Change the dimensions in the Data tab of the property editor.
2.3. Change Width to 31 mm.

3. Create a chamfer.

3.1. Select the upper edge (Edge6) on the front face of the Cube in the 3D view.
3.2. Press Chamfer.
3.3. In the Chamfer edges task panel go to Selection, choose Select edges. As Fillet type choose Constant length, then set Length to 5 mm.
3.4. Press OK. This will create a Chamfer object.
3.5. In the tree view, select Chafmer, in the View tab change the value of Line Width to 2.0.

Base figure created from a cube object and a chamfer.

Insert the ShapeString

4. Switch to the Draft Workbench.

4.1. Make sure nothing is selected in the tree view.
4.2. Establish the working plane to XY (Top) by clicking on SelectPlane and pressing Top (XY).

5. Insert the text "FreeCAD".

5.1. Press on ShapeString.
5.2. Change X to 0 mm.
5.3. Change Y to 0 mm.
5.4. Change Z to 0 mm.
5.5. Or press Reset point.
5.6. Change String to FreeCAD; change Height to 5 mm; change Tracking to 0 mm.
5.7. Make sure Font file points to a valid font, for example, /usr/share/fonts/truetype/dejavu/DejaVuSans.ttf. Press the ellipsis ... to open the operating system's dialog to find a font.
5.8. Press OK. This will create a ShapeString object.
5.9. Recompute the document by pressing Refresh.
5.10. In the tree view, select Chamfer, then press Space. This will hide the object, so you can see the ShapeString better.

Text created as a ShapeString, that is, as a collection of edges in a plane.

Create the 3D text

6. Switch back to the Part Workbench.

6.1. In the tree view, select ShapeString, then press Extrude.
6.2. In the Extrude task panel go to Direction, choose Along normal; in Length, set Along to 1 mm; also tick the Create solid option.
6.3. Press OK. This will create an Extrude object.

Text created as a ShapeString, and turned into a solid by extrusion.

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)