Modern CNC machining systems can interpret the geometry of a part directly from the 3D CAD file. Technical drawings are not necessary to request a quote, but they are still very important and widely used in the industry, as they improve the communication of technical requirements between the designer/engineer and the machinist.
In this article, we will examine when and why should you include a technical drawing to your CNC order, we will break down the anatomy of a drawing and give you basic and advanced tips and guidelines for drawing one.
A well-designed, fully-dimensioned technical drawing is shown in the image below. By the end of this article, you will know how to read it and how to correctly prepare one yourself.
Why are technical drawings still important?
It is necessary to include a technical drawing to your order when your 3D CAD model includes:
- Threads (internal or external)
- Features with tolerances that exceed the standard
- Individual surfaces with specific finishing requirements (surface roughness etc)
These requirements cannot be conveyed in a 3D CAD file.
Even if your design does not include the above, it is generally a good practice to accompany your 3D CAD file with a drawing when placing a CNC order. Most CNC service providers can manufacture parts directly from a technical drawing and they often prefer them over 3D CAD files, because:
- They are trained to interpret quickly the geometry of a part from the 2D drawing
- It is easier to identify the main dimensions, functions and the critical features of a part
- It is easier to assess the cost of manufacturing the part
There a many different standards and best practices for drafting a technical drawing. It does not matter which techniques you use to draft your technical drawing, as long as all the technical requirements are communicated clearly.
Pro Tip: In the example drawing of this article, the model is fully-dimensioned. This is recommended but not necessary, as the basic dimensions of the part are conveyed in the 3D CAD file. To save time, you can annotate in your technical drawing only the most important features that you want to be measured and the threads.
The anatomy of a technical drawing
A typical technical drawing consists of the following parts:
- A title block
- An isometric/pictorial view of the part
- The main orthographic views of the part
- Section views or detail views
- Notes to the manufacturer
The title block
The title block contains basic information about the part, such as the part name, the material, the finishing and color requirements, the name of the designer and the company. It is important to fill in these basic information, as they inform the manufacturer about the function of the part.
The title block also contains other technical information, such as the scale of the drawing, the standard used for dimensioning and tolerancing.
Another element that is usually present in or near the title block in the angle projection. The angle projection determines the way the views are arranged in the drawing. Typically, drawings drafted using ASME standards (USA, Australia) use 3rd angle projection and ISO/DIN standards (Europe), like the drawing of this example, use 1st angle projection.
The pictorial (isometric) view
Adding one or more 3D pictorial view of the part to your drawing is recommended, as it makes the drawing easier to understand in a glance.
Isometric views are used for this purposes, as they combines the illusion of depth with the undistorted presentation of the parts geometry (vertical lines remain vertical and horizontal lines are drawn at 30o).
The main orthographic views
Most information about the geometry of the part is conveyed in the main orthographic views.
These are two-dimensional depictions of the three-dimensional object, representing the exact shape of the part, as seen from the outer side of a bounding box one side at a time. Only the edges of the parts are drawn this way to allow for the clearer communication of dimensions and features.
For most parts, two or three orthographic views are sufficient to accurately describe the whole geometry.
Section views can be used to show the internal details of a part. The cutting line in a main orthographic view shows where the part is cross-sectioned and the cross-hatch pattern of the section view indicates regions where material has been removed.
Technical drawings can have multiple section views with two letters linking each cutting line with each section view (for example A-A, B-B and so on). The arrows of the cutting line indicate the direction you are looking at.
Usually section views are placed in-line with an orthographic view, but they can also be placed elsewhere in the drawing if there is not enough space. The part can be sectioned along its whole width (like in the example above), along half its width or at an angle.
Note: The edges of hidden internal features can also be represented in an orthographic using dashed lines, but section views add more clarity.
Detail views are used to highlight complex or difficult to dimension areas of a main orthographic view.
They are typically circular in shape (placed offset to avoid confusion) and are annotated with a single letter that links the detail view with the main drawing (for example A, B and so on).
Detail views can be placed anywhere on the drawing and can use a different scale than the rest of the drawing, as long as this is clearly communicated (like in the example).
Notes to the manufacturer
Notes to the manufacturer can be added on the technical drawing to conveys additional information that was not included in the technical drawing.
For example, instructions to break (deburr) all sharp edges, specific overall surface finish requirements, and a reference to a CAD file or to an another component the part in the drawing interacts with can all be added to the notes of your technical drawing.
Sometime symbols are used instead of text. For example, surface roughness is commonly annotated with a symbol.
Note: If only one surface requires a specific surface roughness finish, then it should be annotated on the drawing and not on the notes. The standard surface roughness of the parts machined on 3D Hubs is Ra 3.2 μm (125 μinch). Finishes to a surface roughness of Ra 1.6 μm (64 μinch) and 0.8 μm (32 μinch) are also available.
Prepare a technical drawing in 7 steps
Here is a summary of the steps you should follow when drafting your technical drawing:
Step 1. Define the most important views and place the relevant orthographic in the center of the drawing, leaving enough space between them to add dimensions.
Step 2. If your part has internal features or complex and difficult to dimension areas, consider adding section views or detail view accordingly.
Step 3. Add construction lines to all views. Construction lines include centerlines (to define planes or axes of symmetry), center marks, and center mark patterns (to define the location of the center of holes or of circular patterns).
Step 4. Add dimensions to your drawing, starting with the most important dimensions first (more tips on this are given in the next section).
Step 5. Specify the location, size and length of all threads.
Step 6. Add tolerances to features that need higher accuracy than the standard tolerance (in 3D Hubs this is ±.125 mm or ±.005'').
Step 7. Fill in the title block and make sure that all relevant information and requirements that exceed the standard practices (surface finish, deburring etc.) are mentioned in the notes.
When your drawing is ready, export is as a PDF file and attach it to your order.
Now that you are familiar with the basic structure of a technical drawing, let's delve deeper into the specifics of adding dimensions, annotations and tolerances.
Tips for adding dimensions, tolerances & annotations
Adding critical dimensions
If your part is accompanied with a 3D CAD file, the dimensions that you add on the technical drawing are the dimensions that will be checked by the manufacturer. It is recommended to dimension all important features on your drawings though to avoid errors.
Here are some tips to help you dimension your models:
- Start by placing the overall dimensions of the part.
- Next, add the dimensions that are most critical for functional purposes. For example, the distance between the two holes in the example drawing are the most important.
- Then, add dimensions to other features. A good practice is to place all dimension starting from the same baseline (also known as datum), as shown in the example.
- The dimensions should be placed on the view that describes the feature most clearly. For example, the dimensions of the threaded holes are not included in this view, as they are more clearly described in the detail view A.
- For repeated features, add dimensions to only one of them, indicating the total number the feature is repeated on the current view. In the example, two identical holes with a counterbore are specified using a 2x in the callout.
More information on adding dimensions to your drawing can be found in this article by MIT.
Holes are common features in CNC machined parts. They are usually machined with a drill sot they have standardized dimensions.
They often also include secondary features, such as counterbores (⌴) and countersinks (⌵). Adding a callout instead of dimensioning each individual feature is recommended.
In the example below, the callout defines two identical though holes with a counterbore. The depth symbol (↧) can be used instead of adding an additional dimension to the drawing.
If your parts contain threads, then these must be clearly specified on the technical drawing. Threads can be defined by simply indicating a standard thread size (for example M4) instead of a diameter dimension.
The recommended way to define a thread though is by using a callout, as callouts add clarity to the drawing and allow the specification of pilot holes and threads with different length.
In this case, the first operation should define the dimensions of the pilot hole (the appropriate diameter can be found in standard tables), and the second operation the dimension (and tolerance) of the thread.
Important: Always add a cosmetic thread to your 3D CAD model instead of modelling the thread directly to it.
Tolerances define a range of acceptable values for a certain dimension of the part. Tolerances tell a "story" about the function of the part and are especially important for features that interfere with other components.
Tolerances come in many different formats and can be applied to any dimension on a drawing (both linear or angular).
The simplest tolerances are the bilateral tolerances, which are symmetrical around the base dimension (for example, ± 0.1 mm). There are also unilateral tolerances (with different upper and lower limit) and interference tolerances that are defined in technical table (for example, 6H).
Note: Tolerances are only required on a technical drawing when they must exceed the standard value. When you place an order with 3D Hubs, the standard tolerance is ±.125 mm (or ±.005'').
A more advanced way to define a tolerance is GD&T (Geometric Dimensioning & Tolerancing). A flatness tolerance (⏥) was defined in the example above. Here is short introduction to GD&T:
Geometric Dimensioning & Tolerancing (GD&T)
The Geometric Dimensioning & Tolerancing (GD&T) system is more difficult to apply than standard dimensioning and tolerancing, but is considered superior, as it communicates engineering intent more clearly. Using GD&T overall looser tolerances can be defined, while still fulfilling the main design requirements, improving quality and reducing cost.
In the above example, true position (⌖) was used to define the tolerance of this pattern of holes. Other common geometric tolerances include flatness (⏥) and concentricity (◎).
It is out of the scope of this article to describe in depth how you can apply GD&T to your designs, as it is a very complex subject. An excellent introduction to the topic can be found here.
We will give you though the basic knowledge you need to read them in case you ever encounter them in a drawing. Here is an example:
This callout defines eight holes with a nominal diameter of 10 mm and a tolerance of ± 0.1 mm to their diameter. This means that no matter where you measure this diameter, the result of the measurement must be between 9.9 and 10.1 mm.
The true position tolerance defines the location of the center of the hole in respect to the three main baseline edges (datum) of the part. This means that the center axis of the hole must always be within an ideal cylinder that has a center at the location defined by the theoretically exact dimensions in the drawing and a diameter equal to 0.1 mm.
This practically means that the center of the hole will not drift away from its designed location, guaranteeing that the part can fit to the rest of the assembly.
On 3D Hubs, we encourage the addition of GD&T to your parts, but it is recommended to use them only for critical assemblies and at later stages of the design process (for example, during full-scale production), as they have higher metrology requirements, increasing the cost of a one-off prototype.
- A technical drawing is necessary when your part contains threads, tolerances or finishes on specific surfaces.
- It is recommended to fully dimension the technical drawing to avoid errors.
- To save time, you can dimension only the features you want to be measured by the CNC machining service provider.
About 3D Hubs
3D Hubs is the world's largest network of manufacturing Hubs. With services connected in over 140 countries, we'll find the fastest and most price competitive manufacturing service near you.See how it works