TechDraw Preferences

Introduction
The preferences of the TechDraw Workbench are found in the Preferences Editor,.

All preferences settings with italic labels are default values for new drawing objects. They have no effect on existing objects.

Drawing Update

 * Update With 3D: Whether or not pages are updated every time the 3D model is changed. This is a global policy setting.
 * Allow Page Override: Whether or not a page's Keep Update property can override the global Update With 3D parameter. This is a global policy setting.
 * Keep Page Up To Date: Keeps drawing pages in sync with changes of the 3D model in real time. This can slow down the response time.
 * Auto-distribute Secondary Views: Automatically distributes secondary views for projection groups.

Labels

 * Label Font: The name of the font for labels. The font is also used for new dimensions, changing it has no effect on existing dimensions.
 * Label Size: Default size for labels.

Conventions

 * Projection Group Angle: If projection groups will use either first-angle projection/European or third-angle projection/American. See multiview projection for an explanation.
 * Hidden Line Style: The style to be used for hidden lines.

Files

 * Default Template: Default template file for new pages.
 * Template Directory: Starting directory for toolbar button.
 * Hatch Pattern File: Default SVG or bitmap file for hatches.
 * Line Group File: Alternate file for personal line group definitions.
 * Welding Directory: Default directory for toolbar button.
 * PAT File: Default PAT pattern definition file for geometric hatches.
 * Pattern Name: Name of the default PAT pattern.

Scale

 * Page Scale: Default scale for new pages.
 * View Scale Type: Default scale for new views.
 * View Custom Scale: Default scale for views if View Scale Type is Custom.

Size Adjustments

 * Vertex Scale: Scale of vertex dots. Multiplier of line width.
 * Center Mark Scale: Size of center marks. Multiplier of vertex size.
 * Template Edit Mark: Size of template field click handles in mm (green dots).
 * Welding Symbol Scale: Multiplier for size of welding symbols.

Dimensions

 * Standard and Style: The standard to be used for dimensional values. The difference between the standards are shown in the image: TechDraw_Dimension_standardization.png
 * - drawn according to the standard ISO 129-1, text is rotated to be parallel with the dimension line tangent.
 * - drawn in compliance with ISO 129-1, text is always horizontal, above the shortest possible reference line.
 * - drawn according to the standard ASME Y14.5M, text is horizontal, inserted in a break within the dimension line or arc.
 * - drawn in compliance with ASME Y14.5M, text is horizontal, short reference line is attached to one side's vertical center.


 * Use Global Decimals: Use number of decimals from the general preferences.
 * Show Units: Appends the unit (mm, in, etc.) to dimension values.
 * Alternate Decimals: Number of decimals if Use Global Decimals is not used.
 * Default Format: Custom format for dimension text. Uses the printf format specifier.
 * Font Size: Font size for dimension text.
 * Tolerance Text Scale: Tolerance font size adjustment. Multiplier of dimension Font Size.
 * Diameter Symbol: Character used to indicate diameter dimensions.
 * Arrow Style: Arrowhead style for dimensions.
 * Arrow Size: Arrowhead size of dimensions.

Annotation



 * Section Line Standard: Standard to be used to draw section lines in section views.
 * Section Line Style: Style for section lines.
 * Section Cut Surface: Style for section cut surface. The options are:
 * Hide: There is no visible surface.
 * Solid Color: The surface gets the color set for Section Face
 * SVG Hatch: The surface is hatched.
 * PAT Hatch: The surface is geometrically hatched.
 * Line Width Group: A LineGroup to set the default line widths.
 * Detail View Outline Shape: Outline shape for detail views.
 * Detail Highlight Style: Line style of the outline shape for detail views.
 * Center Line Style: Default style for centerlines.
 * Balloon Shape: Shape of balloon annotations.
 * Balloon Leader End: Default style for balloon leader line ends.
 * Balloon Leader Kink Length: Length of balloon leader line kink.
 * Balloon Orthogonal Triangle: If Balloon Leader End is Filled Triangle, the triangle can only get a vertical or horizontal direction when the balloon is moved.
 * Leader Line Auto Horizontal: Forces last leader line segment to be horizontal.
 * Show Center Marks: Show arc center marks in views.
 * Print Center Marks: Show arc centers in printed output.

Colors


Setup of the default colors for new pages:


 * Normal: Normal line color.
 * Preselected: Preselection color. The color that is used to highlight objects when hovering with the mouse over them.
 * Selected: Color for selected objects.
 * Background: Background color around pages.
 * Dimension: Color of dimension lines and text.
 * Centerline: Color for centerlines.
 * Detail Highlight: Line color for the outline shape of detail views.
 * Transparent Faces: If checked, object faces will be transparent. Otherwise the set color will be used for faces.
 * Hidden Line: Hidden line color. This color will be used for all kinds of hidden lines.
 * Section Face: Color of the section view cut surface. Only used if the setting Section Cut Surface is set to Solid Color.
 * Section Line: Color of the section view cut line.
 * Hatch: Hatch image color.
 * Geometric Hatch: Geometric hatch pattern color.
 * Vertex: Color of the selectable vertices in views.
 * Leaderline: Color for new leaderlines.

HLR


In the English GUI, HLR stands for hidden line removal.


 * Use Polygon Approximation: Uses an approximation to find hidden lines. This is fast, but the result is a collection of short straight lines.
 * Show Hard Lines: Shows hard and outline edges (visible lines always shown)
 * Show Smooth Lines: Shows smooth lines. A smooth line is a line indicating a change between tangent surfaces, as in the transition from a flat surface to a fillet.
 * Show Seam Lines: Show seam lines. A seam line is a boundary between faces.
 * Show UV ISO Lines: Shows ISO lines. ISO stands for isoparametric. Here is a description what isoparametric lines (in fact curves) are.
 * ISO Count: The number of ISO lines per face edge.

Advanced



 * Detect Faces: If checked, TechDraw will attempt to build faces using the line segments returned by the hidden line removal algorithm. Faces must be detected in order to use hatching, but there can be a performance penalty in complex models.
 * Show Section Edges: Highlights the border of the section cut in section views.
 * Debug Section: Dumps intermediate results during a Section view processing
 * Debug Detail: Dumps intermediate results during a Detail view processing
 * Allow Crazy Edges: Includes edges with unexpected geometry in results, e.g. zero lengths
 * Fuse Before Section: Performs a fuse operation on the input shape(s) before Section view processing
 * Show Loose 2D Geom: Includes 2D Objects in projections, e.g. loose sketches
 * Edge Fuzz: Size of selection area around edges. The fuzz unit is approximately 0.1 mm, depending on your current zoom.
 * Mark Fuzz: Selection area around center marks. The fuzz unit is approximately 0.1 mm, depending on your current zoom.
 * Line End Cap Shape: Setting of the line end cap shape. Explanation of the options: https://doc.qt.io/qt-5/qt.html#PenCapStyle-enum
 * Max SVG Hatch Tiles: The limit of SVG tiles with a size of 64x64 pixels used to hatch a single face. For large scalings one might get an error about to many SVG tiles, then one needs to increase the tile limit.
 * Max PAT Hatch Segments: The maximum hatch line segments used when hatching a face with a PAT pattern.

Hidden Settings
Note:  Since FreeCAD 0.19, all settings are available in the Preferences dialogs. The following only applies for FreeCAD versions older than 0.19:

Some preference settings are only accessible through the Parameter editor,.

Preferences/Mod/TechDraw/Decorations

 * CenterMarkScale: default scale factor for CenterMarks
 * ShowCenterMarks: default /
 * PrintCenterMarks: / show CenterMarks when printing

Preferences/Mod/TechDraw/General

 * DefaultScale: initial setting of Page Scale
 * EdgeFuzz: pick radius for Edges
 * MarkFuzz: pick radius for CenterMarks
 * SectionFuseFirst: fuse Source objects before performing Section cut
 * EdgeEndCap: shape of Edge ends 0x00 FlatCap, 0x10 SquareCap, 0x20 RoundCap (Qt::PenCapStyle)

Preferences/Mod/TechDraw/Format

 * SectionFormat: section line style 0-ASME 1-ISO

Preferences/Mod/TechDraw/Standards

 * RadiusAligned: Radius dimension format 0-ISO(aligned) 1-ASME(uniform)