Draft ShapeString tutorial/ro

This tutorial has been re-worked for FreeCAD v1.1, but it should be possible to follow the steps for v1.0 as well.

This tutorial describes a method to create 3D text and use it with solid objects in the Part Workbench. We will discuss how to:

• insert outlined text with the Draft ShapeString tool,
• position it on geometry using Part EditAttachment,
• extrude it to be a 3D solid with Part Extrude, then finally
• engrave the text by applying a boolean Part Cut.

To use ShapeStrings inside the PartDesign Workbench, the process is essentially the same as with the Part Workbench, but the ShapeString must be placed inside the PartDesign Body. Go to the end of this tutorial for more information.

Final model of the engraved text.

Setup

1. Open FreeCAD and create a new empty document with File → New Document.

1.1. Switch to the Part Workbench either with View → Workbench → Part Workbench, or with the Workbench Selector .

1.2. Press the Isometric button, or press 0 in the numerical pad of your keyboard, to change the view to isometric to visualize the 3D solids better.

1.3. Whenever you add objects, press the Fit All button, or its hotkey V, F. This will pan and zoom the 3D View so that all elements are visible in the view.

1.4. Hold Ctrl while you click to select multiple items. If you make a wrong selected or want to de-select everything, just click in an empty area in the 3D View.

2. Create a rectangular box:

2.1. Insert a primitive cube by clicking on Cube.

2.2. Select the created Cube in the Tree View.

2.3. On the Data tab of the Property View:

2.3.1. Change Width to 31 mm.

2.4. Re-center the view per step 1.3.

3. Create a chamfer:

3.1. Select the upper edge (Edge6) of the elongated face of the Cube in the 3D View.

3.2. Press Chamfer.

3.3. In the Chamfer Edges task panel:

3.3.1. Verify that Select edges is selected and that the Chamfer type is Equal distance.

3.3.2. Change Length to 5 mm.

3.3.3. Press OK. This will create a Chamfer object.

Base object created from an edited cube and a chamfer operation.

4. Create the ShapeString:

4.1. Switch to the Draft Workbench.

4.2. Click on Shape From Text.

4.3. In the ShapeString task panel:

4.3.1. Change Text to FreeCAD.

4.3.2. Change Height to 5 mm.

4.3.3. Make sure Font file points to a valid font, (e.g, /usr/share/fonts/truetype/dejavu/DejaVuSans.ttf or C:/Windows/Fonts/arial.ttf).

Note: for more details about working with fonts please refer to the Draft ShapeString page.

4.3.4. Reset its location to the origin by pressing Reset Point.

4.3.5. Press OK. This will create a ShapeString object.

4.4. In the Tree View, select Chamfer. On the View tab, change the value of Visibility to false, or press Space on the keyboard. This will hide the Chamfer object, so you can see the ShapeString better.

4.5. To see the ShapeString from above change the view by pressing Top, or 2 on the keyboard.

4.6. To restore the view to isometric, press Isometric, or 0 on the keyboard.

4.7. Reverse step 4.4 to make the Chamfer object visible again.

Text created as a ShapeString, that is, a filled compound shape on a plane

5. Move the ShapeString to the Chamfer:

5.1. Make sure both the Chamfer object and the ShapeString object are visible in the 3D View. If one is not, select it in the Tree View and press Space on the keyboard.

5.2. Switch to the Part Workbench.

5.3. In the Tree View, select ShapeString.

5.4. Select Part → Attachment.

5.5. In the 3D View, select the chamfered face of the Chamfer.

5.6. In the Attachment task panel:

5.6.1 Change the Attachment mode to Inertia 2-3.

5.6.2 Press OK.

5.8. Make sure Shapestring is selected in the Tree View.

5.9. On the Data tab of the Property View:

5.9.1. Change Justification to Middle-Center.

5.9.2. Expand the Attachment Offset property node and change Angle to 90.0 °.

The ShapeString centered on the chamfered face

6. Create a solid object from the ShapeString:

6.1. Make sure the Part Workbench is still active.

6.2. In the Tree View, select ShapeString, then press Extrude.

6.3. In the Extrude task panel:

6.3.1. In the Direction section select Along normal

6.3.2. In the Length section set Along to 0 mm and Against to 1 mm.

6.3.3. Check the Create solid option.

6.3.4. Press OK. This will create an Extrude object.

6.4. Since it has been extruded into the Chamfer object, the 3D View will look the same as before. Verify the creation of a solid 3D object by temporarily making the Chamfer object invisible:

6.4.1. In Tree View, select Chamfer.

6.4.2. Press Space to hide it. You should see a solid 3D object in the shape of the word "FreeCAD".

6.4.3. Press Space to make the Chamfer visible again.

The 3D text after making the Chamfer object invisible.

7. Engrave the text on the geometry:

7.1. In the Tree View select Chamfer first, and then Extrude.

Note: the order in which you select the objects is important for the cut operation. The base object must be selected first, then the object to be subtracted.

7.2. Press Cut. This will create a Cut object. This is the final object.

Final model: a chamfered cube, with engraved text created from ShapeString, Extrude, and boolean Cut operations.

Engraving 3D text with the PartDesign Workbench

A similar process as described above can be done with the PartDesign Workbench.

1. Create the Draft ShapeString first.
2. Create a PartDesign Body, make it active, and create a base solid by adding a primitive, or by extruding a sketch with PartDesign Pad.
3. Move the ShapeString object into the active body.
4. Attach the ShapeString object to one of the faces of the solid, or to an edge of the sketch, using Part EditAttachment.
5. Now create a PartDesign Pad or a PartDesign Pocket from the ShapeString, in order to produce an additive or a subtractive feature respectively.

See the forum thread How to use ShapeStrings in PartDesign.

• To create curved text you can use Macro FCCircularText.
• To import text from an SVG file look at the Import text and geometry from Inkscape tutorial.