Геометрические размеры и допуски в TechDraw

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This page is a translated version of the page TechDraw Geometric dimensioning and tolerancing and the translation is 21% complete.
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Важной целью технического чертежа является то, чтобы читающий его человек понимал, какими характеристиками должна обладать деталь, с какой точностью и как она должна быть изготовлена. Поскольку большинство деталей стыкуются друг с другом в процессе сборки, важны их геометрические размеры. Для достижения этой цели была разработана система геометрических размеров и допусков (англ. аббревиатура GD&T).

К примеру, рассмотрим эту деталь:

TechDraw Hole-Position-Example.png

При сборке ось должна быть продета через 2 отверстия детали. Это означает, что мы должны указать:

  • Диаметры отверстий и их расположение.
  • Что отверстия располагаются вдоль определенной оси, которая не перпендикулярна базовой плоскости XZ.
  • Что осевая часть должна обладать определенной прямолинейностью.

The straightness is important because a bent axis would not fit through the holes. The hole alignment is important because just drilling each hole at the given position without taking care of the axis, would lead to holes through which the axis will not fit. So just specifying the hole dimension and position is not sufficient. The first point is "classical" dimensioning while the 2 others are geometric information, thus GD&T comes into play. The example also makes clear that GD&T is essential to assure that parts fit well to assemblies.

If you are not familiar with the concept of GD&T, we highly recommend to learn about it now. For example a quick introduction is given in this video. For more like the concept of the "maximum material condition", have a look at this video. For details to all sorts of GD&T features, look around in the Internet. For example this YouTube channel provides some good explanations.

GD&T is defined in the standards ISO 1101 and ASME Y14.5.

TechDraws' capabilities to fulfill the common GD&T standards is limited (as of FreeCAD 0.20) but you can achieve already many things. This Wiki page explains what is implemented and what tricks can be used for non-implemented features. Note: this Wiki page is not about to teach GD&T!


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


The default font for new dimension is determined by the preferences setting Label Font. The default font size is specified by the preferences setting Font Size.
Note: It is recommended to use a font in which the minus sign has the same width as the plus sign because this assured that tolerances will be formatted as proposed by the GD&T norms. Such a font is for example osifont that is part of all FreeCAD installations.

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. Either double-click on the dimension in the drawing or onto the dimension object in the model tree
  2. In the appearing dimension dialog the field Format Specifier 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.


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

Setting the option Theoretically Exact in the dimension dialog 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 option Arbitrary Text in the dimension dialog. Then the content of the field Format Specifier will be printed as dimension.

With the properties ДанныеX and ДанныеY 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.



  1. Create a dimension in your drawing
  2. Either double-click on the dimension in the drawing or onto the dimension object in the model tree
  3. In the appearing dimension dialog specify as Overtolerance the amount by which the dimension can be exceeded.
    This will result in an equal tolerance like this: TechDraw equal-tolerance.png
  4. If you have unequal tolerances, specify as Undertolerance the amount by which the dimension can be smaller and uncheck the option Equal Tolerance.
    This will result in an unequal tolerance like this: TechDraw Non-equal-tolerance.png


To get rid of a tolerance, change Overtolerance and Undertolerance to each zero.


The default font for new tolerances is the same than for dimensions. The default font size is specified by the preferences setting Tolerance Text Scale. This scale is a factor of the font size used for the dimension.

The default number format for new tolerances is by default the same format than for the dimension. It can be changed in the dimension dialog.

You can also use your own text instead of a formatted number by checking the option Arbitrary Tolerance Text in the dimension dialog. Then the content of Tolerance Format Specifier will be used as tolerance text.

Geometrical Tolerancing

Tolerances are created by using the Balloon feature of TechDraw. Since for most features a frame is required, it is helpful to change in the TechDraw preferences the Balloon Shape to Rectangle.

Tolerance indicator

Example of a toleranced rod. (The run-out already defines the straightness, it is only there as example.)

The tolerance indicator of GD&T is a frame, also called "feature control frame". It can be created by using the Balloon feature of TechDraw:

  • after adding a Balloon and if its shape is not already a frame, double-click on it in the model tree and set in the appearing dialog the Shape to Rectangle.
  • add the corresponding Unicode character for the feature you need to the Balloon Text. (You can copy them from the reference tables below.)
  • by adding the character '|' to the Text, you start a new indicator field.

There is no rule that defines if or how the tolerance indicator must have a leader line or not, so you can either:

  • set the property Line Visible to False in the balloon dialog.
  • set End Symbol to Filled Arrow or Dot.

The example at the right side shows the two possible tolerance indicator layouts.

Опорные элементы

Datums in the GD&T sense of the meaning are surfaces your tolerance is relative to. They are created as Balloon:

  • after adding a Balloon, set End Symbol to Filled Triangle in the balloon dialog.
  • if the bubble shape is not already a frame, set Bubble Shape to Rectangle.
  • drag the bubble with the mouse so that the triangle points away from the datum surface.
  • since it is common to have a straight line for datums unless the datum surface is not perpendicular to X or Y, assure that either the properties ДанныеX and ДанныеOrigin X or ДанныеY and ДанныеOrigin Y are equal to get a straight Balloon line.
Example of a datum in a drawing

Symbol reference

To insert GD&T symbols TechDraw provides the Customize format label feature.

As reference, here are lists of characters to be used for geometric tolerancing:

Геометрических допуски на чертежах (В соответствии с таблицей №2 ISO 1101-2017 (См. также ГОСТ 53442))
Группа допусков Геометрическая характеристика Обозначение Unicode символ Необходимость указания базы Примечания
Допуски формы
GD&T Straightness.svg
GD&T Flatness.svg
GD&T Circularity.svg
In older norms also called circularity.
GD&T Cylindricity.svg
Суммарные допуски формы и расположения
Форма заданного профиля
GD&T Profileofaline.svg
No datum necessary when used for form purpose
Форма заданной поверхности
GD&T Profileofasurface.svg
No datum necessary when used for form purpose
Допуски ориентации
GD&T Parallelism.svg
GD&T Perpendicularity.svg
GD&T Angularity.svg
Допуски месторасположения
GD&T Position.svg
No datum necessary when working with norm ISO 5458.
Концентричность (для точек) / Соосность (для осей)
GD&T Concentricity.svg
Named concentricity when used for center points and coaxiality when used for median lines. In the norm ASME Y14.5 it was eliminated since the version from 2018.
GD&T Symmetry.svg
In the norm ASME Y14.5 from 2018, the symmetry was eliminated.
Допуски биения
GD&T Circular runout.svg
Полное биение
GD&T Totalrunout.svg
Symbols used in the feature control frame to specify a feature's description, tolerance, modifier and datum references
Symbol Unicode character Modifier Notes
Gd&t freestate.svg
Free state Applies only when part is otherwise restrained
Gd&t leastmaterialcondition.svg
Least material condition (LMC) Useful to maintain minimum wall thickness
Gd&t maximummaterialcondition.svg
Maximum material condition (MMC) Provides bonus tolerance only for a feature of size
Gd&t projectedtolerancezone.svg
Projected tolerance zone Useful on threaded holes for long studs
Gd&t regardlessoffeaturesize.svg
Regardless of feature size (RFS) Not part of the 1994 version. See para. A5, bullet 3. Also para. D3. Also, Figure 3-8.
Gd&t tangentplane.svg
Tangent plane Useful for interfaces where form is not required
Gd&t continuousfeature.svg
Continuous feature Identifies a group of features that should be treated geometrically as a single feature
Gd&t statisticaltolerance.svg
Statistical tolerance Appears in the 1994 version of the standard, assumes appropriate statistical process control.
Gd&t unilateral.svg
Unequal bilateral Added in the 2009 version of the standard, and refers to unequal profile distribution. Number after this symbol indicates tolerance in the "plus material" direction.