All preferences settings with italic labels are default values for new drawing objects. They have no effect on existing objects.
- 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.
- 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.
- Projection Group Angle: If projection groups will use either first-angle (European) projection or third-angle (American) projection. See multiview projection for an explanation.
- Hidden Line Style: The style to be used for hidden lines.
- 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 introduced in version 0.19 .
- PAT File: Default PAT pattern definition file for geometric hatches.
- Pattern Name: Name of the default PAT pattern.
- 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.
- 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. introduced in version 0.19
- Standard and Style: The standard to be used for dimensional values. The difference between the standards are shown in the image:
ISO Oriented- drawn according to the standard ISO 129-1, text is rotated to be parallel with the dimension line tangent.
ISO Referencing- drawn in compliance with ISO 129-1, text is always horizontal, above the shortest possible reference line.
ASME Inlined- drawn according to the standard ASME Y14.5M, text is horizontal, inserted in a break within the dimension line or arc.
ASME Referencing- 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.
- 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: introduced in version 0.19
- 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. introduced in version 0.19
- 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.
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. introduced in version 0.19
- Transparent Faces: If checked, object faces will be transparent. Otherwise the set color will be used for faces. introduced in version 0.19
- 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 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.
- 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: pen cap styles
- 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.
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, Tools → Edit parameters.
- CenterMarkScale: default scale factor for CenterMarks
- ShowCenterMarks: default
falseshow CenterMarks when printing introduced in version 0.19
- DefaultScale: initial setting of Page Scale introduced in version 0.19
- 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) introduced in version 0.19
- SectionFormat: section line style 0-ASME 1-ISO
- RadiusAligned: Radius dimension format 0-ISO(aligned) 1-ASME(uniform)