TechDraw General Examples/fr

Introduction
L' atelier TechDraw possède de nombreux outils, mais quels sont les éléments nécessaires pour transformer un morceau de papier en un véritable dessin ? Cette page a pour but de donner quelques explications et quelques exemples de ce que TechDraw est déjà capable de faire.

Dessins
Un dessin consiste en une ou plusieurs vues pour décrire géométriquement une pièce... Mais vous le savez déjà, n'est-ce pas ?

Examinons les éléments de base.



Dessins créés manuellement


La feuille de papier
Les formats de papier sont normalisés et, pour pouvoir imprimer sans être mis à l'échelle, le format de notre feuille doit correspondre au format d'impression souhaité.

Les cadres
Lorsque les dessins étaient réalisés à la main, ils devaient être épinglés ou collés sur une planche à dessin. Des trous de perforation étaient ajoutés au dessin fini pour attacher le dessin plié à un dossier ou à une chemise. Cette zone extérieure est séparée par un cadre rectangulaire. Un autre cadre rectangulaire situé à l'intérieur du premier définit la zone de dessin. Entre les deux cadres, il y a généralement un ensemble d'index et de séparateurs qui permettent de localiser certains éléments du dessin.



Le cartouche
Le cartouche contient des informations écrites sur la pièce et le dessin, telles que le numéro de la pièce, le titre, l'auteur, le propriétaire, etc.



La nomenclature
Les dessins d'assemblage peuvent éventuellement être accompagnés d'une nomenclature. La nomenclature peut également être placée sur une feuille de dessin séparée ou sur une feuille de calcul.



Changer le journal
Les modifications apportées à la pièce ou au dessin sont consignées dans un journal sur le dessin ou dans un document séparé et liées au dessin par des index correspondants.

Les vues
Les vues contiennent la description géométrique d'une pièce dans une certaine direction. La plupart des pièces nécessitent au moins deux vues pour être correctement décrites.

Les annotations
Des textes supplémentaires qui n'appartiennent pas aux éléments mentionnés ci-dessus.



Dessins réalisés avec TechDraw
Techdraw utilise un objet Page comme conteneur pour tous les éléments liés au dessin. Cet objet ne peut pas exister seul, mais doit contenir un modèle. C'est pourquoi il n'y a pas de commande Nouvelle page et un nouvel objet page est créé automatiquement chaque fois qu'un modèle est inséré.

Les modèles
Un objet Modèle est un fichier image SVG et son code contient toutes les informations nécessaires pour créer une feuille de papier virtuelle avec des cadres et un cartouche correspondants, et éventuellement une nomenclature.

Les images SVG ne sont pas paramétriques. Cela signifie que pour chaque format, un modèle distinct doit être créé, et qu'un tel ensemble de modèles est nécessaire pour toute variation d'objets de type cadre ou cartouche. C'est beaucoup à coder et à gérer, mais d'un autre côté, les modèles ne peuvent pas être modifiés accidentellement dans FreeCAD.

Il y a plusieurs façons de créer un modèle :
 * 1) Dessinez le avec Inkscape, voir Comment créer un modèle TechDraw personnalisé.
 * 2) Faites le manuellement, voir Template explained.
 * 3) Utiliser une macro, voir TechDraw Création de modèles et la macro TemplateHelper.







Le dessin jusqu'à présent
Jusqu'à présent, on peut dire que TechDraw, en relation avec des modèles SVG intégrés, peut fournir une feuille de dessin correcte avec un cadre et un cartouche. Certaines entrées peuvent être modifiées après la création grâce à des textes éditables et certains contenus peuvent être insérés automatiquement si des macros sont impliquées.

Les vues
Les vues contiennent la description géométrique en 2D d'un objet. Le contenu d'une vue TechDraw peut être dérivé de la géométrie 3D ou obtenu à partir d'un autre atelier comme des vues de Arch et des  vues de Draft.

Comme FreeCAD est une application de modélisation 3D, la fonction clé de TechDraw est de dériver des vues 2D à partir d'une géométrie 3D. Prenons un exemple simple, la pièce du Tutoriel d'introduction Part Design qui est également utilisée avec le TechDraw Tutoriel d'introduction :



Active View
An Active View is more or less a screen shot of the 3D view in its own kind of TechDraw view.



View
A View is TechDraw's basic view object to derive proper drawings. In contrast to an Active View it is not restricted to visible objects on the screen, but also displays selected objects outside the screen. The preferred scale depends on the available space and the level of detail that has to be displayed.



Projection Group
A Projection Group is a set of views. Each view direction is perpendicular to its neighbor and all depend on the 3D window's direction by default. TechDraw provides six views matching with the Navigation Cube sides, and four isometric views.



Section View
TechDraw provides tools to create a Simple Section View or a  Complex Section View. Both depend on a base view and on tools to define a section line and to derive the view direction. Have a look at TechDraw Section Examples for an overview.



Auxiliary View
If we need a view of a tilted plane to see its true lengths we would define the view direction in a base view and place the Auxiliary view accordingly, but TechDraw provides no tool for Auxiliary views yet.

Good news: It is quite easy to emulate using the Simple Section View tool:


 * 1) Select a base view.
 * 2) Create a [[Image:TechDraw_SectionView.svg|16px]] Simple Section View with default settings.
 * 3) Use [[Image:TechDraw_AngleDimension.svg|16px]] Insert Angle Dimension to measure the angle of the plane.
 * 4) Edit the section view angle in the Set View Direction area of its task panel.
 * 5) Edit the section view coordinates in the Section Plane Location area of its task panel. Use small steps to move the section line outside the object or FreeCAD may crash.
 * 6) Hide unwanted annotation elements such as section line, section arrows, and section name.
 * 7) Add needed items like view arrow, and view name.







Detail View
A Detail View is a copy of an area of a base view usually to magnify hardly visible geometry.



Imperfections

 * Detail views according to ISO standard do not have a frame/border (the upper part of the enclosing circle). Editor's note: what is meant here?? Frames are not printed...
 * The break line that cuts the detail off from the rest should be a thin freehand line or the cad equivalent, a thin zigzag line. FreeCAD/TechDraw do not provide freehand/zigzag lines (yet).
 * Hatched areas in the base view should be hatched in the detail view, too.

Arch View
An Arch View displays a view of an  Arch SectionPlane. Its content is rendered by the Arch workbench.

Draft View
A Draft View displays a view of a selected Part-based object or Group object. It is intended for 2D objects. Its content is rendered by the Draft workbench.



Spreadsheet View
A Spreadsheet View displays a view of a Spreadsheet Workbench sheet.



The views so far
TechDraw needs some additions like break lines, and a proper auxiliary view tool and also some improvement of the Detail View tool. But even in this state we can describe our objects visually quite well:



Dimensioning
Now that our item is described geometrically, dimensions will be added to further define the shape, and tolerances to define the allowed deviation. TechDraw supplies several tools to apply dimensions to the 2D representation of our item:
 * [[Image:TechDraw_LengthDimension.svg|16px]] Length Dimension
 * [[Image:TechDraw_HorizontalDimension.svg|16px]] Horizontal Dimension
 * [[Image:TechDraw_VerticalDimension.svg|16px]] Vertical Dimension
 * [[Image:TechDraw_RadiusDimension.svg|16px]] Radius Dimension
 * [[Image:TechDraw_DiameterDimension.svg|16px]] Diameter Dimension
 * [[Image:TechDraw_AngleDimension.svg|16px]] Angle Dimension
 * [[Image:TechDraw_3PtAngleDimension.svg|16px]] 3-Point Angle Dimension

They have in common that they measure the projected shape of the item. If you have learned drafting the manual way, you know how to use auxiliary views to turn the item into a position where projected lengths equal true lengths. For visualization other than this old school way, dimensions can be linked to 3D geometry using TechDraw imensionRepair to display "true dimensions".

Two other tools measure the overall length horizontally or vertically respectively: These cannot be linked with 3D geometry (yet).
 * [[Image:TechDraw_HorizontalExtentDimension.svg|16px]] Insert Horizontal Extent Dimension
 * [[Image:TechDraw_VerticalExtentDimension.svg|16px]] Insert Vertical Extent Dimension

See Dimension dialog (and the following properties section) for all settings that are not mentioned in this overview.

Simple dimensions
The dimension text depends mainly on these properties:
 * By default their defaults are
 * By default their defaults are
 * By default their defaults are
 * By default their defaults are

To "cheat" we can use these two properties:
 * Set to to use the content of the Format Spec to format the actual dimensional value.
 * Set to to use the content of the Format Spec to be displayed as text instead if the dimension value.
 * Set to to use the content of the Format Spec to be displayed as text instead if the dimension value.


 * : Like, but for the tolerance.

If we only need the dimension value there's nothing to do but to change the number of decimals if desired.
 * For example: →  to display 3 decimals, or  →  to display whole numbers.

Length dimension
There are three tools to add length dimensions: Length Dimension,  Horizontal Dimension, and  Vertical Dimension.



This shows that it is important to rotate a front view in the Projection Group dialog or otherwise the connected views will not follow. On the other hand that would restrict us to 90° turns.

If a dimension has to run parallel to an edge it needs another selectable line perpendicular to the edge and the Length Dimension tool, that can find the shortest (= perpendicular) distance between a point and a line. An edge will not be automatically extended by an imaginary line and so we need to create an auxiliary (cosmetic) line manually. (A cosmetic point could be used as well, but that requires even more work).


 * The black (point to line) [[Image:TechDraw_LengthDimension.svg|16px]] Length Dimension depends on a cosmetic line that doesn't rotate with the view. (A cosmetic point wouldn't be helpful either.)
 * The [[Image:TechDraw_HorizontalDimension.svg|16px]] Horizontal Dimension and [[Image:TechDraw_VerticalDimension.svg|16px]] Vertical Dimension (red and green) stay with the page orientation and change their values accordingly.
 * The blue is a point to line [[Image:TechDraw_LengthDimension.svg|16px]] Length Dimension, too but rotates with the view as there is no cosmetic geometry involved.

Angle dimension
TechDraw provides two tools to add angle dimensions: Angle Dimension and  3-Point Angle Dimension.




 * Blue: an [[Image:TechDraw_AngleDimension.svg|16px]] Angle Dimension between two edges.
 * Red: a [[Image:TechDraw_3PtAngleDimension.svg|16px]] 3-Point Angle Dimension using both end points and the center point of an arc.

Chamfer dimension
A chamfer dimension can be applied as a length dimension with a manually edited property or by using  Create Horizontal Chamfer Dimension and  Create Vertical Chamfer Dimension to create a size and angle dimension for a chamfer.



The chamfer tools work well for objects with horizontal and vertical sides as long as they are parallel to the view's = the page's X and Y axes, but many parts won't do us the favor of being perfectly aligned.

The angle values are not parametric! They do not change if the view is tilted. The last page shows the correct angles, but dimensions positioned like this are pointless.

To align the chamfer dimension along an edge we need an auxiliary (cosmetic) point where the unchamfered edges would meet and have to use Length Dimension; but cosmetic point won't follow the edges if the view is tilted. (also see Length dimension.)

Radius dimension
A Radius Dimension adds a radius dimension to a circle or circular arc, no more no less.



To change the arrowhead direction just set the property to ,

Diameter dimension
Diameter dimensions can be added as a Diameter Dimension or one of the length dimensions  Length Dimension,  Horizontal Dimension, and  Vertical Dimension. (Or in connection with a leader line pointing to a circle center or a center line - not displayed.)




 * Blue: a [[Image:TechDraw_VerticalDimension.svg|16px]] length dimension in the side view of the hole needs a "⌀" prefixed to distinguish this from a rectangular hole.
 * [[Image:TechDraw_ExtensionInsertDiameter.svg|16px]] Insert '⌀' Prefix is an easy way to do this, but the property can be edited manually as well.


 * Green: a simple [[Image:TechDraw_VerticalDimension.svg|16px]] length dimension.
 * It needs some auxiliary geometry (cosmetic points) as it cannot be applied to circles directly.


 * Red: a [[Image:TechDraw_DiameterDimension.svg|16px]] diameter dimension. In case you look along the hole axis and can see the circular shape of the hole the "⌀" may be omitted. To remove it edit the property manually.

Thread dimension
Thread dimensions can be applied just like diameter dimensions, but they require some auxiliary geometry created beforehand: Add Cosmetic Thread Hole Side View,  Add Cosmetic Thread Hole Bottom View,  Add Cosmetic Thread Bolt Side View, or  Add Cosmetic Thread Bolt Bottom View.



All Thread dimensions are applied to auxiliary (cosmetic) lines or circles (in connection with cosmetic points) and all properties need to be edited manually to prefix the "M" for metric threads.

Tolerances
Tolerances express how much a measured dimension may deviate from the dimension value on the drawing. To suffix a tolerance values to the dimension value simply set the property to a value other than, this results in a symmetric tolerance such as.

For an asymmetric tolerance set property to  and specify also a lower value for the  property.

The values can be set in the Dimension dialog or directly in the Property editor.

Hole/shaft fit
Fit tolerances can be added by suffixing tolerance classes to a dimension. A tolerance class consist of a tolerance field specifier (letter, upper case for holes, lower case for shafts) and a tolerance grade specifier (number) and can be suffixed in three ways:
 * 1) Set the  property to  and specify both tolerance classes in the  and  properties.
 * 2) Use the [[Image:TechDraw_HoleShaftFit.svg|16px]] Add hole or shaft fit tool. This suffixes only one tolerance class but adds the related values to the  and  properties.
 * 3) For a single tolerance simply suffix the tolerance class to the format specifier in the  property.

Thread fit
Thread fit tolerances can be suffixed like described above for hole/shaft fit tolerances, except method 2. The thread tolerance classes display the tolerance grade specifier (number) in front of the tolerance field specifier (letter, upper case for internal threads, lower case for external threads).

Inspection dimensions
Inspection dimensions are not yet implemented.

To fake an inspection dimension we set the property to " " (one space - no character at all and we would have no handle to grab the dimension line to move it) and then set the  property to ; this results in a dimension without value. The value can now be substituted with a balloon without leader line. This only works with horizontal dimensions since we cannot rotate balloons.



Geometric dimensioning and tolerancing
The system of geometric dimensioning and tolerancing (GD&T) aims at describing shapes more precisely than toleranced dimensions alone can do. It is built on datums, theoretically exact dimensions, and tolerance indicators.

Datums
Datums are virtual surfaces, planes, lines, and points used as references to describe geometrical features with theoretically exact dimensions and tolerance indicators. They can be used to built a theoretically exact virtual coordinate system.

Datum feature
A datum feature is a geometric feature of an object corresponding with a certain datum. Datum feature symbols are added using Balloon annotations.



The property has to be set to  for vertical leader lines, but this results in a portion of the line shown within the Frame.

Datum target
Datum targets are points or relatively small areas that denote where to derive a datum from. Most common use is to create a theoretically exact virtual coordinate system from a set of six datum targets.

Theoretically exact dimensions
Theoretically exact dimensions are added the same way as simple dimensions and the Theoretically exact checkbox makes the difference: It sets the property to  which adds a rectangular frame to the dimension value and deactivates tolerances and all tolerance settings.

Tolerance indicator
A tolerance indicator, also called "feature control frame", is a frame containing tolerance information about:
 * which geometric characteristic is tolerated
 * the shape and size of the tolerance field
 * the datums to be referenced
 * some more symbols to describe the features even more precisely.

Tolerance indicators are like datum feature symbols added using Balloon annotations.

In most cases tolerance indicators are aligned with a dimension line which is impossible in TechDraw except for horizontal dimensions since, as already mentioned, balloon annotations can not be rotated.