In the previous section 7.1 Part Drawing, the following points were explained to you by means of notes.
Drawings in general
- Since the sheet division, sheet size, scale and workpiece should be coordinated with each other, it is advisable to consider which sizes must be selected before creating the drawing.
- In technical drawings, care is taken to ensure that as many views as necessary and as few as possible are reproduced. The main view should be the one that shows most of the details.
- Never forget to insert the center axes of a drawing.
- Note lines and position numbers are entered into the drawing at any angle, but never horizontally or vertically. However, texts must always be aligned parallel to the lower or right side of the sheet so that they can be read from the main reading directions.
Dimensions
- Hidden edges are not to be dimensioned.
- Do not forget to enter the symbols and markings required for the respective workpiece in the drawing, such as the Ø symbol (diameter symbol), R (for a radius), etc.
- Double dimensions are not allowed. If an additional dimension is required for the understanding, an auxiliary dimension is entered in the drawing. Auxiliary dimensions are dimensions in which the dimensions are marked with round brackets. They can be calculated from the dimensions already entered.
- Collective entries (textual instructions) can be advantageous for the clarity of drawings, in addition to saving dimensions and corresponding work. Example: "All not dimensioned chamfers 1x45°".
- Do not rely on the accuracy of updated measurements after changes to the model. Check the correctness of all measurements after updating!
Dimension types
The following dimension types are distinguished for standard-compliant dimensioning:
| Parallel dimensioning | This is a reference dimension. It is often used when the components to be manufactured are machined with lathes and/or milling machines. Several dimension lines are entered parallel to each other for linear dimensions and concentric for angular dimensions. |
| Chain dimensioning | The individual dimensions are lined up directly next to each other. It should only be used if this is technically necessary for production. Otherwise, there is too great a risk that the tolerances of the individual sections or the tolerance of the total length cannot be adhered to. Reason: Each individual dimension has its own tolerance. The deviations add up in the unfavourable case, which results in a greater deviation of the total length. |
| Increasing dimensioning | The increasing dimensioning is a reference dimensioning, in which each form element is incrementally dimensioned from a reference element. As a rule, the dimension lines are arranged overlaid in a row from their origin. |
| Coordinate dimensioning | This is a reference dimension in a coordinate system. It is mostly used for the drawings of components that are machined with programmable machines (CNC machines). |
The different dimension types can also be used in combination if it increases the information content of the drawing.
Within the CAD course, you should preferably use parallel dimensioning (dimensioning over reference edges).
You can make the following settings in the Linear 
menu under Dimension Set:
| Icon | Function | Description |
|---|---|---|
 |
Chain dimensioning | Chain |
 |
Parallel dimensioning (dimensioning over reference edges) | Baseline |
Coordinate dimensioning and increasing dimensioning can be performed using the Ordinate 
function.
Manufacturing appropriate dimensioning
When creating and dimensioning the drawing, you should always consider how the part to be displayed will be manufactured later and dimension it accordingly. Therefore, make sure that your component is already in the manufacturing position.