TechDraw Dimension Length

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TechDraw

Menu location
TechDraw Dimension Length
TechDraw → Dimension Length
Workbenches
TechDraw
Default shortcut
None
Introduced in version
-
See also
None

Descriere

Instrumentul pentru cote tip distanță adaugă o cotă distanță unei imagini. Cota poate fi între două vârfuri, lungimea unei muchii sau distanța dintre două margini. Distanța va fi inițial distanța proiectată(adică așa cum este reprezentată în desen), dar această distanță poate fi înlocuită prin distanța 3D reală utilizând instrumentul Link Dimension .

The TechDraw LengthDimension 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

Cum se folosește

Select the points or edge which define your measurement.
There are several ways to invoke the tool:
- Press the Insert Length Dimension button.
- Select the TechDraw → Dimensions → Insert Length Dimension option from the menu.
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. There is also an additional %w format that prints the specified number of digits after the decimal separator and removes trailing zeros. For example, %.2w means that at most 2 decimals will be printed and any trailing zeros will be cut off.

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.

Lines

Override Angles: If checked, the usual angles for the dimension line and extension lines will be overridden by the specified values.

Dimension line angle: Override value for angle of dimension line with view X axis (in degrees).

Use default: Set dimension line angle to the usual angle.

Use selection: Set dimension line angle to match the angle of the selected edge (or 2 vertices) in the view.

Extension line angle: Override value for angle of extension lines with view X axis (in degrees).

Use default: Set extension line angle to the usual angle.

Use selection: Set extension line angle to match the angle of the selected edge (or 2 vertices) in the view.

Proprietăți

DateX: Poziția orizontală a textului de dimensiune în mm față de View.
DateY: Poziția verticală a textului dimensional în mm față de vizualizare
DateFormatSpec: Adaugă text suplimentar la textul cotei. Valoarea distanței va înlocui %.2f (sau alt format specific valid).printf.
DateType: Lungimea, raza, diametrul etc. În mod normal, nu este manipulat de către utilizatorul final.
DateMeasureType: "True" -Bazat pe geometrie 3D sau "Projected" - bazat pe desen. În mod normal, nu este manipulat de către utilizatorul final.
DateArbitrary: "True" - ignoră valoarea reală și afișează FormatSpec ca valore. "False" - utilizează adevărata valoare.
VizualizareFont: Numele fontului folosit pentru afișarea textului cotei.
VizualizareFontsize: Fontul textului cotei exprimat în mm.
VizualizareLineWidth: Grosimea liniei de cotă.
VizualizareColor: Culoarea pentru linii și text.

Data

Base

DateX: Horizontal position of the dimension text relative to the View.
DateY: Vertical position of the dimension text relative to the View.
DateType: Length, radius, diameter, etc. Not normally manipulated by the end user.
DateMeasure 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

DateTheoretical Exact: Specifies a theoretically exact (or basic) dimension.

false - a common dimension by default, possibly with tolerances.

true - a theoretical value. As such, it shall not bear any tolerances. The dimension will be displayed by a frame around the value:

DateEqual Tolerance: If over- and undertolerance are equal. Then the negated value of the overtolerance is used as undertolerance.

true - the negated value of the DateOver Tolerance is used as DateUnder Tolerance. The display will be

false - the DateUnder Tolerance is taken into account. The display will be

DateOver Tolerance: The amount by which the dimension may be larger.
DateUnder Tolerance: The amount by which the dimension may be smaller.
DateInverted: 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

DateFormat Spec: How the dimension value will be formatted. See Formatting.
DateFormat Spec Over Tolerance: Like DateFormat Spec, but for overtolerances.
DateFormat Spec Under Tolerance: Like DateFormat Spec, but for undertolerances.
DateArbitrary: 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.

DateArbitrary Tolerances: Like DateArbitrary, but for the tolerance.

Override

DateAngleOverride: Whether the direction of dimension and extension lines is overridden.

false - the directions are computed as usual.

true - the directions are overridden by LineAngle and ExtensionAngle property values.

DateLineAngle: angle of dimension line with view X axis (in degrees).
DateExtensionAngle: angle of extension line(s) with view X axis (in degrees).

View

Base

VizualizareVisibility: Sets whether the dimension is visible. true - visible, false - hidden.

Dim Format

VizualizareFont: The name of the font to use for the dimension text.
VizualizareFont Size: Dimension text size.
VizualizareGap Factor ASME: Adjusts the gap between the dimension points and the start of the extension lines. The gap is this value times the line width. introduced in version 1.0
VizualizareGap Factor ISO: Adjusts the gap between the dimension points and the start of the extension lines. The gap is this value times the line width. introduced in version 1.0
VizualizareLine Width: Dimension line weight.
VizualizareColor: Color for lines and text.
VizualizareStandard 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.

VizualizareRendering 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 following Reduced 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 with Normal extent.

VizualizareFlip 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.

Note

Toate Cotele/Distanțele sunt extrem de vulnerabile la infama problemă a "topological naming". În acest moment nu este posibilă menținerea referințelor la obiectele geometrice 2D (proiectate) sau 3D (reale) în sincronizare cu modificările din model. Se recomandă adăugarea de Cote la sfârșitul procesului de creare a desenului.

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.

Script

Cotele tip distanță pot fi adăugate la Pages utilizând Python.

See also: TechDraw API and FreeCAD Scripting Basics.

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)

Notes

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).