Draft ShapeString tutorial/ro

This tutorial was originally written by Roland Frank (†2017, r-frank), and it was rewritten and re-illustrated by vocx.

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,
• extrude it to be a 3D solid with Part Extrude,
• position it in 3D space using placement, and Draft Move (it uses a sketch as auxiliary geometry), and
• 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 is placed inside the PartDesign Body to extrude it. Go to the end of this tutorial for more information.

Final model of the engraved text.

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.

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 Chamfer type choose Equal distance, then set Length to 5 mm.

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

3.5. In the tree view, select Chamfer, in the View tab change the value of Line Width to 2.0.

Base object created from a cube and a chamfer operation.

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. Click 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, (e.g, /usr/share/fonts/truetype/dejavu/DejaVuSans.ttf or C:/Windows/Fonts/arial.ttf). Press the ellipsis ... to open the operating system's dialog to find a font.

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

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 ShapeString, in the View tab change the value of Line Width to 2.0.

5.11. In the tree view, select Chamfer, in the View tab change the value of Visibility to false, or press Space in the keyboard. This will hide the object, so you can see the ShapeString better.

5.12. To see the ShapeString from above change the view by pressing Top (XY), or 2 in the keyboard.

5.13. To restore the view to isometric, press View isometric, or 0 in the keyboard.

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

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.

6.4. In the tree view, select Extrude, in the View tab change the value of Line Width to 2.0.

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

Now we will draw a simple sketch that will be used as auxiliary geometry to position the ShapeString extrusion.

7. In the tree view, select Extrude, and press Space in the keyboard to make it invisible.

8. Switch to the Sketcher Workbench.

9. In the tree view, select Chamfer, and press Space in the keyboard to make it visible.

9.1. Choose the sloped face created by the chamfer operation (Face3).

9.2. Click on NewSketch. In the Sketch attachment dialog, select FlatFace, and press OK.

9.3. The view should adjust automatically so that the camera is parallel to the selected face.

9.4. Draw a horizontal line in a general position on top of the face. The length is not important; we are just interested in its position.

9.5. Constrain the left endpoint to be 2.5 mm away from the local X axis and from the local Y axis, using ConstrainDistanceX and ConstrainDistanceY.

9.6. Since the sketch is just an auxiliary object, we don't need to have it fully constrained. You can do this if you wish by assigning a fixed distance, say, 20 mm, again with ConstrainDistanceX.

9.7. Close the sketch.

Line being created with the sketcher, with constraints.

Sketch line created on top of the solid face, to be used as reference guide for positioning the extruded text.

10. In the tree view, select Extrude, and press Space in the keyboard to make it visible.

11. With Extrude still selected, in the Data tab of the property editor, click on the Placement value so the ellipsis button ... appears on the right and click on that button.

11.1. Tick the option Apply incremental changes.

11.2. Change the Rotation to Rotation axis with angle; Axis to Z (by setting the X, Y and Z values of the axis inputboxes to 0, 0 and 1 respectively, Z is the third inputbox), and Angle to 90 deg, then click on Apply. This will apply a rotation around the Z-axis, and will reset the Angle field to zero.

11.3. Change the Rotation to Rotation axis with angle; Axis to Y (by setting the X, Y and Z values of the axis inputboxes to 0, 1 and 0 respectively), and Angle to 45 deg, then click on Apply. This will apply a rotation around the Y-axis, and will reset the Angle field to zero.

11.4. Click on OK to close the dialog.

12. Switch again to the Draft Workbench.

12.1. Switch to "Wireframe" draw style with View → Draw style → Wireframe, or press the Wireframe button in the view toolbar. This will allow you to see the objects behind other objects.

12.2. Make sure the Draft Snap "Snap to endpoint" method is active. This can be done from the menu Draft → Snapping → Toggle On/Off, and then → Endpoint, or by pressing the ToggleSnap and Snap endpoint buttons in the Snap toolbar.

13. In the tree view, select Extrude.

13.1. Click on Move.

13.2. In the 3D view click on the upper left corner point of the Extrude object (1), and then click on the leftmost point in the line drawn with the sketcher (2).

13.3. If Snap endpoint is active, as soon as you move the pointer close to a vertex, you should see that it attaches to it exactly.

Note: if you have problems snapping to vertices, make sure only the Snap endpoint method is enabled. Having multiple snapping methods active at the same time may make it difficult to select the right feature.

13.4. The extruded text should now be inside the body of the Chamfer object.

The extruded ShapeString should be moved to the position of the sketched line that lies on the face of the base body.

Extruded ShapeString positioned in the Chamfer.

14. Switch back to the Part Workbench.

14.1. Switch to "As is" draw style with View → Draw style → As is, or press the As is button in the view toolbar. This will show all objects with the normal shading and color.

14.2. In the tree view, select Sketch, and press Space in the keyboard to make it invisible.

15. In the tree view select Chamfer first, and then Extrude.

15.1. Then press Cut. This will create a Cut object. This is the final object.

Note: the order in which you select the objects is important for the cut operation. The base object is selected first, and the subtracting object comes at the end.

15.2. In the tree view, select Cut, in the View tab change the value of Line Width to 2.0.

Final model of a filleted cube, with carved text created from a 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 add a base solid by adding primitives, or using a Sketch and extruding it 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 a PartDesign Plane, 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 of the base body, 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.