TechDraw Geometric dimensioning and tolerancing

Overview
The main purpose of a technical drawing is that others understand what the designer created with what tolerances and material and how to manufacture the design. To achieve this the system of Geometric Dimensioning and Tolerancing (GD&T) was developed for defining and communicating engineering tolerances.

TechDraws' capabilities to fulfill the common GD&T standards is still limited (as of FreeCAD 0.19) but you can achieve already many things. This Wiki page will explain what is implemented and what tricks are useful.

Dimensioning
TechDraw provides several tools to create different types of dimension. Please have a look at the different dimension on how to create and modify them.

Formatting
The default format for new dimension numbers depends on the preferences options Use Global Decimals and Alternate Decimals. This specifies the number of decimals, but in every case the dimension is a floating point number. For example if the setting is to have 2 decimals, the used format specifier is "%.2f" (floating point number with 2 decimals).

The number format can be changed:
 * 1) Select a dimension in the tree
 * 2) Go to the properties tab Data and there to the section
 * 3) The property  contains the format specifier, so change it to what you need

The syntax of the format specifier is explained here. You can also use this online tool to see what formatting specifier will format numbers.

Examples:
 * You use 2 decimals but for an angle you want to have only one decimal use the format specifier %.1f.
 * You use 2 decimals but don't like that trailing zeroes are printed (you prefer 4 instead of 4.00). Then use this format specifier: %g. The 'g' will use the shortest possible output and thus it omits trailing zeroes. Moreover it will automatically switch to scientific notation if necessary.

With the property you can make length dimensions negative and flip angles from the range 0 - 180° to the the reflex range 180° - 360°.

Setting the property to true will mark the dimension as theoretically exact by adding a frame around it.

You can use your own text instead of a formatted number by setting the property to true. Then the content of the property will be printed as dimension.

With the properties and  you can change the horizontal and vertical position of the dimension text relative to the view. Alternatively you can change the position by dragging the dimension number or text.

Tolerancing
TechDraw allows you to add tolerances to every dimension.

Creation

 * 1) Create a dimension in your drawing
 * 2) Select the dimension in the tree
 * 3) Go to the properties tab Data and there to the section
 * 4) Add to the property  the amount by which the dimension can be exceeded.
 * 5) Add to the property  the amount by which the dimension can be smaller.

Deletion
To get rid of a tolerance, change the the properties and  to each 0.00.

Formatting
The default format for new tolerances is %+g.??

The number format can be changed:
 * 1) Select a dimension in the tree
 * 2) Go to the properties tab Data and there to the section
 * 3) The property  contains the format specifier, so change it to what you need

You can also use your own text instead of a formatted number by setting the property to true. Then the content of the property will be printed as dimension.

Tolerances appear by default like this: In many cases you have equal over- and undertolerance, thus it should better be displayed like "7,87 ±0,1 mm" since this is the standard. The only way to achieve this at the moment, is to delete the tolerances as described in the section above. Then set to true an enter the the dimension as it should appear:  "7,87 ±0,1 mm".