Draft ShapeString tutorial/ru
|ShapeString (Draft workbench)|
|Время для завершения|
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.
The Sketcher Workbench is used briefly to draw an auxiliary line. More information about the tools of this workbench can be found in
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
Cubein the tree view.
- 2.2. Change the dimensions in the Data tab of the property editor.
- 2.3. Change Width to
3. Create a chamfer.
- 3.1. Select the upper edge (
Edge6) on the front face of the
Cubein 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
- 3.4. Press OK. This will create a
- 3.5. In the tree view, select
Chamfer, in the View tab change the value of Line Width to
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 SelectPlane and pressing Top (XY).
5. Insert the text "FreeCAD".
- 5.1. Click on ShapeString.
- 5.2. Change X to
- 5.3. Change Y to
- 5.4. Change Z to
- 5.5. Or press Reset point.
- 5.6. Change String to
FreeCAD; change Height to
5 mm; change Tracking to
- 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
- 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
- 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
- 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.
Create the solid 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
- 6.4. In the tree view, select
Extrude, in the View tab change the value of Line Width to
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 (
- 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 mmaway 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.
Positioning the solid text in 3D space
10. In the tree view, select
Extrude, and press Space in the keyboard to make it visible.
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
Zvalues of the axis inputboxes to
Zis 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
Zvalues of the axis inputboxes to
0respectively), 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
- 13.1. Click on Move.
- 13.2. In the 3D view click on the upper left corner point of the
Extrudeobject (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
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
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 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
- 15.1. Then press Cut. This will create a
Cutobject. 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
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.
- Create the Draft ShapeString first.
- 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.
- Move the
ShapeStringobject into the active body.
- Attach the
ShapeStringobject to one of the faces of the solid, or to a PartDesign Plane, using Part EditAttachment.
- 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.
- Примитивы: Куб(Параллелограмм), Конус, Цилиндр, Сфера, Тор, Полый цилиндр,Примитивы, Связующие формы
- Создание и правка: Выдавливание, Построение фигуры вращения, Отражение, Скругление, Фаска, Создать плоскость из граней, Ruled Surface, Профиль, Sweep, Section, Cross sections, 3D Offset, 2D Offset, Создать полый объект, Projection on surface, Прикрепление
- Булевы операции: Соединить, Разорвать связь, Compound Filter, Булевы операции, Cut, Fuse, Common, Connect, Embed, Cutout, Boolean fragments, Slice apart, Slice, XOR
- Измерительные: Measure Linear, Measure Angular, Measure Refresh, Clear All, Toggle All, Toggle 3D, Toggle Delta
- Инструменты структуры: Part, Group
- Вспомогательные инструменты: Create body, Create sketch, Edit sketch, Map sketch to face
- Инструменты моделирования
- Инструменты данных: Create a datum point, Create a datum line, Create a datum plane, Create a local coordinate system, Create a shape binder, Create a clone
- Аддитивные инструменты: Pad, Revolution, Additive loft, Additive pipe, Additive box, Additive cone, Additive cylinder, Additive ellipsoid, Additive prism, Additive sphere, Additive torus, Additive wedge
- Субстрактивные инструменты: Pocket, Hole, Groove, Subtractive loft, Subtractive pipe, Subtractive box, Subtractive cone, Subtractive cylinder, Subtractive ellipsoid, Subtractive prism, Subtractive sphere, Subtractive torus, Subtractive wedge
- Инструменты трансформации: Mirrored, Linear Pattern, Polar Pattern, Create MultiTransform
- Отделочные инструменты: Fillet, Chamfer, Draft, Thickness
- Бинарные: Boolean operation
- Дополнительно: Migrate, Shaft design wizard, Involute gear
- Инструменты контекстного меню: Set tip, Move object to other body, Move object after other object
- General: Create sketch, Edit sketch, Map sketch to face, Reorient sketch, Validate sketch, Merge sketches, Mirror sketch, Leave sketch, View sketch, View section, Toggle grid, Toggle snap, Configure rendering order, Stop operation
- Sketcher geometries: Point, Line, Arc, Arc by 3 points, Circle, Circle by 3 points, Ellipse, Ellipse by 3 points, Arc of ellipse, Arc of hyperbola, Arc of parabola, B-spline by control points, Periodic B-spline by control points, B-spline by knots, Periodic B-spline by knots, Polyline, Rectangle, Centered rectangle, Rounded rectangle, Triangle, Square, Pentagon, Hexagon, Heptagon, Octagon, Regular polygon, Slot, Fillet, Corner-preserving fillet, Trim, Extend, Split, External geometry, Carbon copy, Toggle construction geometry
- Sketcher constraints:
- Geometric constraints: Coincident, Point on object, Vertical, Horizontal, Parallel, Perpendicular, Tangent, Equal, Symmetric, Block
- Dimensional constraints: Lock, Horizontal distance, Vertical distance, Distance, Radius or weight, Diameter, Auto radius/diameter, Angle, Refraction (Snell's law)
- Constraint tools: Toggle driving/reference constraint, Activate/deactivate constraint
- Sketcher tools: Select unconstrained DoF, Select associated constraints, Select associated geometry, Select redundant constraints, Select conflicting constraints, Show/hide internal geometry, Select origin, Select horizontal axis, Select vertical axis, Symmetry, Clone, Copy, Move, Rectangular array, Remove axes alignment, Delete all geometry, Delete all constraints
- Sketcher B-spline tools: Show/hide B-spline degree, Show/hide B-spline control polygon, Show/hide B-spline curvature comb, Show/hide B-spline knot multiplicity, Show/hide B-spline control point weight, Convert geometry to B-spline, Increase B-spline degree, Decrease B-spline degree, Increase knot multiplicity, Decrease knot multiplicity, Insert knot, Join curves
- Sketcher virtual space: Switch virtual space
- Additional: Sketcher Dialog, Preferences, Sketcher scripting
- Установка: Загрузка, Windows, Linux, Mac, Дополнительных компонентов, Docker, AppImage, Ubuntu Snap
- Базовая: О FreeCAD, Интерфейс, Навигация мыши, Методы выделения, Имя объекта, Настройки, Верстаки, Структура документа, Свойства, Помоги FreeCAD, Пожертвования
- Помощь: Учебники, Видео учебники
- Верстаки: Std Base, Arch, Draft, FEM, Inspection, Mesh, OpenSCAD, Part, PartDesign, Path, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Start, Surface, TechDraw, Test Framework, Web