Draft ShapeString tutorial/ru

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Тема Руководство ShapeString (Draft workbench) Beginner 30 minutes r-frank 0.16.6704 None

Introduction

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 tool,
• extrude it to be a 3D solid with ,
• position it in 3D space using placement, and (it uses a sketch as auxiliary geometry), and
• engrave the text by applying a boolean .

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.

The Sketcher Workbench is used briefly to draw an auxiliary line. More information about the tools of this workbench can be found in

Setup

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

1.1. Press the 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 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 .

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 .
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.

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 and pressing .

5.1. Click on .
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.
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 .
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 , or 2 in the keyboard.
5.13. To restore the view to isometric, press , or 0 in the keyboard.

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

Create the solid 3D text

6. Switch back to the Part Workbench.

6.1. In the tree view, select `ShapeString`, then press .
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.

Insert auxiliary sketch for positioning

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 . 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 and .
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 .
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.

Positioning the solid text in 3D space

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 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 and buttons in the Snap toolbar.

13. In the tree view, select `Extrude`.

13.1. Click on .
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 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 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 `Fillet` 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 `Fillet`.

Creating engraved text

14. Switch back to the Part Workbench.

14.1. Switch to "As is" draw style with View → Draw style As is, or press the 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 . 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 first.
2. Create a , make it active, and add a base solid by adding primitives, or using a Sketch and extruding it with .
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 , using .
5. Now create a or a 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.