Tutorial Draft Forma da Testo
|
Argomento |
---|
Product design |
Livello di difficoltà |
Base |
Tempo di esecuzione |
30 minuti |
Autore |
r-frank e vocx |
Versione di FreeCAD |
0.17 o superiore |
File di esempio |
Draft_Shapestring_Text |
Contents
|
Introduzione
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.
Per disegnare una linea ausiliaria viene utilizzato l'ambiente Sketcher. Maggiori informazioni sugli strumenti di questo workbench sono disponibili in
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.
Creare la forma di base
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 theCube
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 to5 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 to2.0
.
Base object created from a cube and a chamfer operation.
Inserire il testo con lo strumento ShapeString di Draft
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 to5 mm
; change Tracking to0 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
ShapeString
, in the View tab change the value of Line Width to2.0
. - 5.11. In the tree view, select
Chamfer
, in the View tab change the value of Visibility tofalse
, or press Space in the keyboard. This will hide the object, so you can see theShapeString
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.
Creare il testo solido 3D
6. Switch back to the Part Workbench.
- 6.1. In the tree view, select
ShapeString
, then pressExtrude.
- 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 to2.0
.
Text created as a ShapeString, and turned into a solid by extrusion.
Inserire lo schizzo ausiliario per il posizionamento
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, usingConstrainDistanceX 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 withConstrainDistanceX.
- 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.
Posizionare il testo 3D nello spazio 3D
10. In the tree view, select Extrude
, and press Space in the keyboard to make it visible.
11. In the tree view, select Extrude
, in the Data tab of the property editor, click on the Placement value so the ellipsis button ... appears on the right.
- 11.1. Tick the option Apply incremental changes.
- 11.2. Change the Rotation to
Rotation axis with angle
; Axis toZ
, and Angle to90 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 toY
, and Angle to45 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
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
.
Creare il testo inciso
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 to2.0
.
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.
- 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
ShapeString
object into the active body. - Attach the
ShapeString
object to one of the faces of the solid, or to aPartDesign Plane, using
Part Attachment.
- 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.
Note
- To create curved text you can use the macro
Circular Text.
- To import text from an SVG file look at the Import text and geometry from Inkscape tutorial.
- General: Tutorial, Video tutorial
- Sketcher: Sketcher reference, Basic Sketcher tutorial
- PartDesign: Simple object, Simple object 2
- Part: Engraved text, Wiffle ball, Basic modeling, Screw threads, Placement
- TechDraw: Basic TechDraw tutorial, New template
- Path: Path for the impatient
- FEM: Cantilever analysis, Shear in a composite block, Postprocessing with Paraview, Reinforced concrete
- Rendering: Raytracing tutorial, POV-ray, Blender
- Primitives: Box, Cone, Cylinder, Sphere, Torus, CreatePrimitives, Shapebuilder
- Modifying objects: Booleans, Union, Common, Cut, Join features, Connect, Embed, Cutout
- Splitting tools: Boolean fragments, Slice a part, Slice, XOR, Part Defeaturing
- Compound: Make compound, Explode Compound, Compound Filter; Extrude, Fillet, Revolve, Section, Cross sections, Chamfer, Mirror, Ruled Surface, Sweep, Loft
- Offset tools: 3D Offset, 2D Offset, Thickness, Projection on surface
- Structure tools: Part, Group
- Helper tools: Create body, Create sketch, Edit sketch, Map sketch to face
- Modeling tools
- Datum tools: Create a datum point, Create a datum line, Create a datum plane, Create a local coordinate system, Create a shape binder, Create a clone
- Additive tools: Pad, Revolution, Additive loft, Additive pipe, Additive box, Additive cone, Additive cylinder, Additive ellipsoid, Additive prism, Additive sphere, Additive torus, Additive wedge
- Subtractive tools: Pocket, Hole, Groove, Subtractive loft, Subtractive pipe, Subtractive box, Subtractive cone, Subtractive cylinder, Subtractive ellipsoid, Subtractive prism, Subtractive sphere, Subtractive torus, Subtractive wedge
- Transformation tools: Mirrored, Linear Pattern, Polar Pattern, Create MultiTransform
- Dress-up tools: Fillet, Chamfer, Draft, Thickness
- Boolean: Boolean operation
- Extras: Migrate, Shaft design wizard, Involute gear
- Contextual Menu tools: Set tip, Move object to other body, Move object after other object
- The tools: New sketch, Edit sketch, Leave sketch, View sketch, View section, Map sketch to face, Reorient sketch, Validate sketch, Merge sketches, Mirror sketch
- Sketcher geometries: Point, Line by 2 point, Create an arc, Arc, Arc by 3 Point, Create a circle, Circle, Circle by 3 Point, Create a conic, Ellipse by center, Ellipse by 3 points, Arc of ellipse, Arc of hyperbola, Arc of parabola, Create a B-spline, Create B-spline, Create periodic B-pline, Polyline (multiple-point line), Rectangle, Create regular polygon, Triangle, Square, Pentagon, Hexagon, Heptagon, Octagon, Create Regular Polygon, Slot, Fillet, Trimming, Extend, External Geometry, CarbonCopy, Construction Mode
- Sketcher constraints
- Geometric constraints Coincident, Point On Object, Vertical, Horizontal, Parallel, Perpendicular, Tangent, Equal Length, Symmetric, Constrain Block
- Dimensional constraints Lock, Horizontal Distance, Vertical Distance, Distance, Radius, Internal Angle, Snell's Law, Internal Alignment, Toggle reference/driving constraint,
- Sketcher tools Select solver DOFs, Close Shape, Connect Edges, Select Constraints, Select Origin, Select Vertical Axis, Select Horizontal Axis, Select Redundant Constraints, Select Conflicting Constraints, Select Elements Associated with constraints, Show/Hide internal geometry, Symmetry, Clone, Copy, Move, Rectangular Array, 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, Convert Geometry to B-spline, Increase degree, Increase knot multiplicity, Decrease knot multiplicity
- Sketcher virtual space Switch Virtual Space

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