TechDraw Section Examples/de

Einleitung
Der Arbeitsbereicch TechDraw hat einen großen Schritt vorwärts gemacht, was die Erstellung von Schnittansichten angeht. Um die Referenzseite nicht zu überfrachten, ist die Absicht dieser Seite, Beispiele zu geben und die ausgeführten Aufgaben korrekt zu benennen.

Regionale Besonderheiten dürfen gerne ergänzt und Fehler verbessert werden.

Schnitte
Schnitte (Schnittansichten) werden verwendet, um in ein Objekt hineinzusehen und so Einzelheiten darzustellen, die sonst schlecht oder gar nicht zu erkennen sind. Normalerweise enthält eine Zeichnung Ansichten, die ein Objekt von mindestens 2 Seiten darstellt. Wird ein Schnitt eingesetzt, werden seine Lage und Ausrichtung mit einer Schnittlinie in einer der Ansichten dargestellt.

In FreeCAD ist es nicht möglich, einfach eine Schnittlinie zu zeichnen; FreeCAD benötigt stattdessen Eingaben im Aufgabenbereich (siehe Schnittansicht und KomplexerSchnitt).



Beispielobjekt
Dieses Objekt hat keinerlei Nutzen, außer dass es zur Beschreibung der unterschiedlichen Schnittdarstellungen dient.





Einfache Schnitte
Das Werkzeug Schnittansicht erstellt einen einfachen Schnitt, der nur eine Schnittebene verwendet, um ein Objekt zu durchschneiden. Das Werkzeug benötigt eine Basisansicht zum Positionieren der Schnittebene. Die vertikale Achse der Schnittebene entspricht immer der Normale der Basisansicht und die horizontale Achse der Schnittebene ist parallel zur Schnittlinie. Normalerweise wird auch die horizontale Achse der Schnittansicht parallel zur Schnittlinie ausgerichtet. Der Winkel zwischen Schnittlinie und horizontaler Achse der Basisansicht wird durch Widgets im Bereich gesteuert:



Die Combobox ermöglicht eine beliebigen Winkel einzustellen. Die vier Schaltflächen können zum Einstellen vorgegebener Winkel verwendet werden:

90° (nach oben), 270° (nach unten), 180° (nach links), 0° (nach rechts)



Horizontaler Schnitt
Schnitt A-A (nach oben)





Schnitt B-B (nach unten)





Vertical section
Section C-C (section left)





Section D-D (section right)





Arbitrary section
Section E-E (section at an arbitrary angle)





By default the section plane goes through the center of gravity of the object. To get an offset section we need to change the values in the area.



Auxiliary view
FreeCAD lacks a tool to derive auxiliary views from a base view, but Insert Section View can also handle that:

Using Section E-E from above and changing the mentioned values to X = and Y =  the section no longer cuts the object and becomes an auxiliary view instead. Note: be careful when changing the values, large steps can crash FreeCAD!

The label was edited. The section line and one arrow have to be hidden in following steps since a single arrow is enough to properly define an auxiliary view.

Single Section
If there is only one section view in the drawing, and it is plain to see that the object is cut along a center line, the section line, including the arrows, and the view title may be omitted.



Internal section
A section view may be integrated into the base view. This case doesn't require arrows and a title either.



Complex sections
The Insert Complex Section tool creates a complex section, such as an aligned section or an offset section, that uses more than one plane to cut an object.

The tool requires a base view ( property) to place several connected section planes to cut through the object, these are defined by a 3D polyline. (This tool can also handle curves, but curved sections are rather unusual.)

The vertical axes of the section planes are always parallel to the normal of the base view. Their horizontal axes are derived from the related segments of the 3D polyline. The orientation of the Section view depends on one of the 3D polyline's segments and is influenced by the widgets in the area of the tool's task panel:



This tool provides 3 options in the combobox to handle the section line segments:
 * : only segments perpendicular to the view direction are displayed (default).
 * : all segments are displayed in true length.
 * : all segments are projected along the same view direction. Depending on the angle between a segment and the view direction the projection may be shorter than the cut area. Segments parallel to the view direction result in a single line.

Offset section
An offset section starts with a base view plus a 3D polyline, a sketch in this case.

The view direction angle must be set to a matching value to avoid unexpected results.



Aligned section
An aligned section also starts with a base view and 3D polyline.

The view direction angle can be set with and  for a coarse orientation. It has to be guessed and set to a best matching value or the result may be unexpected.



If the view direction angle is set incorrectly the result may look like this:



Auxiliary view
The Insert Complex Section tool can, like the  Insert Section View tool, create auxiliary views from base views:

An auxiliary view starts with a base view and a single 3D line placed outside the object.

The value has to be extracted from the 3D line manually. The label was edited. The section line and one arrow have to be hidden in following steps since a single arrow is enough to properly define an auxiliary view.

NoParallel section
A NoParallel section is a mixture of aligned and offset sections.

The arrow direction should have been horizontal, but the tool did not work when the value of was set to. So the sketch was rotated by 5° and said angle was set to as well.

Comparison NoParallel vs. Offset and Aligned


For some reason if the value of of the aligned section is set to exactly  the result is faulty. Only after editing the section and accepting the strange value of that the angle is somehow set to, is the correct result displayed.



Complex one line sections
The length (width) of a complex section depends on the length of the used 3D line, but the results differ from offset section to NoParallel section:



Half section
A view showing a symmetric object cut on one side of a center line and uncut on the other. The depth is usually defined by another center line.