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TechDraw Dimension Length |
Системное название |
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TechDraw Dimension Length |
Расположение в меню |
Нет |
Верстаки |
TechDraw |
Быстрые клавиши |
Нет |
Представлено в версии |
- |
См. также |
TechDraw Dimension Horizontal, TechDraw Dimension Vertical |
Описание
The Length Dimension tool adds a linear dimension to a View. The dimension may be between the distance between two vertices, the length of one edge or the distance between 2 edges. The distance will initially be the projected distance (ie as shown on the drawing), but this may be changed to the actual 3D distance using the TechDraw LinkDimension tool.
Length dimension taken from two arbitrary nodes of the view
Применение
- Select the points or edge which define your measurement.
- Press the Length Dimension button.
- A dimension will be added to the View. The dimension may be dragged to the desired position.
- If needed, add tolerances as described in this page.
To change the properties of a dimension object either double-clicking it in the drawing or in the Tree view. This will open the dimension dialog:
Dimension dialog
The dimension dialog offers the following settings:
Tolerancing
- Theoretically Exact: If checked, is specifies the dimension as theoretically exact dimension. As such, it shall not bear any tolerances. The dimension will be displayed by a frame around the value:
- Equal Tolerance: If checked, the over- and undertolerance are equal and the negated value of the overtolerance is used as undertolerance. The display will be , otherwise it will be .
- Overtolerance: The amount by which the dimension may be larger.
- Undertolerance: The amount by which the dimension may be smaller.
Formatting
- Format Specifier: How the dimension value will be formatted. By default the specifier is %.xf whereby x is the number of decimals. For the formatting syntax see this Wikipedia page.
- Arbitrary Text: If checked, the dimension is replaced by the content of the Format Specifier field.
- OverTolerance Format Specifier: How the overtolerance value will be formatted. By default the specifier is %.xf whereby x is the number of decimals. For the formatting syntax see this Wikipedia page.
- UnderTolerance Format Specifier: How the undertolerance value will be formatted. By default the specifier is %.xf whereby x is the number of decimals. For the formatting syntax see this Wikipedia page.
- Arbitrary Tolerance Text: If checked, the tolerances are replaced by the content of the OverTolerance Format Specifier UnderTolerance Format Specifier fields.
Display Style
- Flip Arrowheads: Flips the direction in which the dimension line arrows are pointing. By default they are inside the dimension line/arc and pointing outwards.
- Color: The color for lines and text.
- Font Size: The dimension text size.
- Drawing Style: The standard (and its style) according to which the dimension is drawn. See the property Standard And Style for details.
Свойства
Data
Base
- ДанныеX: Horizontal position of the dimension text relative to the View.
- ДанныеY: Vertical position of the dimension text relative to the View.
- ДанныеType: Length,radius,diameter, etc. Not normally manipulated by the end user.
- ДанныеMeasure Type: How the measurement is performed. Not normally manipulated directly by the end user.
- True - based on 3D geometry or
- Projected - based on the drawing
- ДанныеTheoretical Exact: Specifies a theoretically exact (or basic) dimension.
- ДанныеEqual Tolerance: If over- and undertolerance are equal. Then the negated value of the overtolerance is used as undertolerance.
- ДанныеOver Tolerance: The amount by which the dimension may be larger.
- ДанныеUnder Tolerance: The amount by which the dimension may be smaller.
- ДанныеInverted: Marks whether the dimension represents a common or an inverted value.
false
- the ordinary value is used. For length it is a positive number, for angle the oblique value (0° - 180°).true
- the inverted value is used. For length a negative number, for angle the reflex value (180° - 360°).
Format
- ДанныеFormat Spec: How the dimension value will be formatted. By default the specifier is %.xf whereby x is the number of decimals. For the formatting syntax see this Wikipedia page.
- ДанныеFormat Spec Over Tolerance: Like ДанныеFormat Spec, but for overtolerances.
- ДанныеFormat Spec Under Tolerance: Like ДанныеFormat Spec, but for undertolerances.
- ДанныеArbitrary: Whether the dimension is replaced by the content of the Format Spec field.
false
- the content of the Format Spec is used to format the actual dimensional value.true
- the content of the Format Spec will be displayed as text instead if the dimension value.
- ДанныеArbitrary Tolerances: Like ДанныеArbitrary, but for the tolerance.
View
Base
- ВидVisibility: Sets whether the dimension is visible.
true
- visible,false
- hidden.
Dim Format
- ВидFont: The name of the font to use for the dimension text.
- ВидFont Size: Dimension text size.
- ВидLine Width: Dimension line weight.
- ВидColor: Color for lines and text.
- ВидStandard And Style: Specifies the standard (and its style) according to which the dimension is drawn:
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.
- ВидRendering Extent: Rather universal property specifying how much space the dimension drawing may take up:
None
- no lines or arrows are drawn, only the bare dimension value is displayed.Minimal
- for lengths and angles a single headed line connecting the dimensional value and the end point's virtual extension line is drawn. The extension line itself is not added.- Diameters are rendered following
Confined
extent, radii followingReduced
extent. Confined
- for lengths and angles a double headed line (or arc) connecting the start and end point's virtual extension lines is drawn, though the extension lines themselves are not added.- Diameters are drawn with a minimal single headed line from dimensional value to the closest point on circle, radii as with
Reduced
extent. Reduced
- for lengths and angles a single headed line connecting the dimensional value and the end point's extension line is drawn along with the extension line itself.- Diameters are drawn with a single headed line from the center to the closest point on circle, radii with a minimal single headed line from dimensional value to the closest arc point.
Normal
- the default value. For lengths and angles a double headed line (or arc) connecting the start and end point's extension lines is drawn, the extension lines themselves as well.- Diameters are drawn as double headed lines striking the center and connecting the closest and farthest points on the circle.
- Radii are drawn as a single headed line from center to the closest arc point.
Expanded
- Only diameters support this value, rendering them in a horizontal or vertical length-like way. Other dimension types are rendered as withNormal
extent.
- ВидFlip Arrowheads: By default the value inside the dimension line/arc means the arrows pointing outwards. If placed outside the dimension line/arc, the arrows point inwards the dimension line/arc.
false
- Let the direction of arrows to be selected automatically according to the rule above.true
- Override the automatically chosen direction and force the opposite one.
Ограничения
Dimension objects are vulnerable to the "topological naming problem". This means that if you modify the 3D geometry the faces and edges of the model may be renamed internally; if a dimension is attached to an edge that is then modified, the dimension may break. In general, it is not possible to keep the projected 2D dimensions synchronized with the actual 3D objects.
Therefore, it is recommended that dimensions be added when the 3D model is no longer being modified.
Workaround
If you want to keep a TechDraw view with dimensions that won't break, you need to dimension an object that won't change.
- Select the object that you want to project, then switch to the Part Workbench and use Part → Create simple copy. This will create a single object that is not parametric, that is, no longer editable.
- Select this copy, then use TechDraw View, and add the desired dimensions.
- If the original 3D model is modified, the modifications won't affect the simple copy, nor the dimensions in the TechDraw view.
See Landmark Dimensions for another approach to circumventing the topological naming issue.
Программирование
См. так же: TechDraw API и Основы составления скриптов FreeCAD.
The Length Dimension tool can be used in macros and from the Python console by using the following functions:
dim1 = FreeCAD.ActiveDocument.addObject('TechDraw::DrawViewDimension','Dimension')
dim1.Type = "Distance"
dim1.References2D=[(view1, 'Edge1')]
rc = page.addView(dim1)
Примечания
- Edge selection. Edges can be difficult to select. You can adjust the selection area for edges using the parameter "/Mod/TechDraw/General/EdgeFuzz" (see Std_DlgParameter). This is a dimension-less number. The default is 10.0. Values in the 20-30 range will make it noticeably easier to select edges. Large numbers will cause overlaps with other drawing elements.
- Decimal places. Dimensions use the global decimal places setting by default. This can be changed via preferences or by changing the FormatSpec property.
- Multiple objects. Views may contain multiple 3D objects as Source. Dimensions may be applied to geometry from any object(s) in the View (ex from Object1.Vertex0 to Object2.Vertex3).
- Pages: Insert Default Page, Insert Page using Template, Redraw Page, Print All Pages
- Views: Insert View, Insert Active View, Insert Projection Group, Insert Section View, Insert Complex Section View, Insert Detail View, Insert Draft Workbench Object, Insert Arch Workbench Object, Insert Spreadsheet View, Insert Clip Group, Share View, Project Shape
- Stacking: Move view to top of stack, Move view to bottom of stack, Move view up one level, Move view down one level
- Decorations: Hatch Face using Image File, Apply Geometric Hatch to Face, Insert SVG Symbol, Insert Bitmap Image, Turn View Frames On/Off
- Dimensions: Insert Length Dimension, Insert Horizontal Dimension, Insert Vertical Dimension, Insert Radius Dimension, Insert Diameter Dimension, Insert Angle Dimension, Insert 3-Point Angle Dimension, Insert Horizontal Extent Dimension, Insert Vertical Extent Dimension, Link Dimension to 3D Geometry, Insert Balloon Annotation, Insert Axonometric Length Dimension, Insert Landmark Dimension, Adjust Geometric References of Dimension
- Annotations: Insert Annotation, Add Leaderline to View, Insert Rich Text Annotation, Add Cosmetic Vertex, Add Midpoint Vertices, Add Quadrant Vertices, Add Centerline to Faces, Add Centerline between 2 Lines, Add Centerline between 2 Points, Add Cosmetic Line Through 2 points, Add Cosmetic Circle, Change Appearance of Lines, Show/Hide Invisible Edges, Add Welding Information to Leader, Add Surface Finish Symbol, Add Hole or Shaft Tolerances
- Extensions:
- Attributes and modifications: Select Line Attributes, Cascade Spacing and Delta Distance, Change Line Attributes, Extend Line, Shorten Line, Lock/Unlock View, Position Section View, Position Horizontal Chain Dimensions, Position Vertical Chain Dimensions, Position Oblique Chain Dimensions, Cascade Horizontal Dimensions, Cascade Vertical Dimensions, Cascade Oblique Dimensions, Calculate the area of selected faces, Calculate the arc length of selected edges, Customize format label
- Centerlines and threading: Add Circle Centerlines, Add Bolt Circle Centerlines, Add Cosmetic Thread Hole Side View, Add Cosmetic Thread Hole Bottom View, Add Cosmetic Thread Bolt Side View, Add Cosmetic Thread Bolt Bottom View, Add Cosmetic Intersection Vertex(es), Add an offset vertex, Add Cosmetic Circle, Add Cosmetic Arc, Add Cosmetic Circle 3 Points, Add Cosmetic Parallel Line, Add Cosmetic Perpendicular Line
- Dimensions: Create Horizontal Chain Dimensions, Create Vertical Chain Dimensions, Create Oblique Chain Dimensions, Create Horizontal Coordinate Dimensions, Create Vertical Coordinate Dimensions, Create Oblique Coordinate Dimensions, Create Horizontal Chamfer Dimension, Create Vertical Chamfer Dimension, Create Arc Length Dimension, Insert '⌀' Prefix, Insert '〼' Prefix, Remove Prefix, Increase Decimal Places, Decrease Decimal Places
- Export: Export Page as SVG, Export Page as DXF
- Additional: Line Groups, Templates, Hatching, Geometric dimensioning and tolerancing, Preferences
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