# TechDraw LengthDimension

(Redirected from TechDraw Dimension Length)
Other languages:  ToggleFrame HorizontalDimension TechDraw Menu location TechDraw LengthDimension TechDraw → Dimensions → Insert Length Dimension TechDraw None - TechDraw HorizontalDimension, TechDraw VerticalDimension

## Description

The TechDraw LengthDimension tool adds a linear dimension to a View. The dimension may be the distance between two points, the length of a straight edge, the perpendicular distance between two edges, or the perpendicular distance between a point and an edge.

Length dimension taken from two points

## Usage

1. Select the points and/or edges which define your measurement. The geometry may be selected in the 3D view (first two options) or in the drawing (all options):
• Select two points.
• Select a single straight edge.
• Select two edges. If both edges are straight they must be parallel. This will produce a perpendicular dimension if an endpoint of one of the edges has a perpendicular projection on the other edge (the resultant point must lie on the actual edge). If multiple solutions are possible, the endpoint that is closest to its projected point is used. If there is no valid perpendicular projection, the dimension will be the distance between the nearest endpoints of the edges.
• Select a point and an edge. This will produce a perpendicular dimension. In version 0.21 and below the dimension will only be perpendicular if the point has a perpendicular projection on the actual edge. Else the dimension will be the distance between the point and the nearest endpoint of the edge.
2. If you have selected geometry in the 3D view: add the correct TechDraw View to the selection by selecting it in the Tree view.
3. There are several ways to invoke the tool:
4. A dimension is added to the View.
5. The dimension may be dragged to the desired position.

### Display 3D measurement

The dimension will initially display the projected measurement (i.e. as shown in the drawing). If required, and if the dimension is based on 3D references, it can be changed to the actual 3D measurement by changing its DataMeasure Type property to `True`. To base a dimension on 3D references select geometry from the 3D view at creation time, or use the TechDraw DimensionRepair tool to update existing dimensions.

### Change properties

To change the properties of a dimension object either double-click 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

• 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` where `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` where `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` where `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 of the dimension line arrows. By default they are inside the dimension line/arc and point 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.

## Limitations

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:

• Create a non-parametric copy of the object that you want to project with Part SimpleCopy.
• 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.