Create a ECAD component in CREO

This paragraph shows the necessary steps to create a new electronic component for the Creo library. New components must be saved in the most suited subfolder of cad‑libraries/libraries/electronics.

Things to know before starting

The following details should be available before starting the design of a new library component:

• The Alias to name the file with.
• The datasheet with the footprint of the component (usually this datasheet can be found in Wingst).
• The 3D model or the datasheet with the dimensions of the component.
• The position of the origin of the component in the electronics library counterpart.

The file name must be decided in accordance with the electronic team.

Step by step guide

1. Open an issue to track the development of the new electrical component (Issue: New commercial ECAD component link).

opening a ticket is mandatory in the following cases:

• Plug components
• component we need positioning on the mechanical layout ( Baseline )
• Components with particularly complicated shape

When is not mandatory:

• for resitances or capacitor
• simple components that are normally placed by the electronic designer
• test point, label or other minor comp.

2. Create a new part using the default template and the right file name (refer to the naming convention above). As an example:

3. Make sure the origin of the component matches the one chosen by the electronic team. Example:

The little yellow dot shows the ***origin*** chosen by the electronics in the center of the pad of the `pin 1`. This is where the ***origin*** of the Creo model must be.

>**TIP:** generally the coordinate system is defined with the `z-axis` coming out of the monitor and the `x-axis` towards the right (ask if in doubt). The `y-axis` goes accordingly to form a right-handed coordinate system.
In most cases the ***origin*** is in the center of the `pin 1` or in the simmetry line of the component, if there is any.
Different locations shall be confirmed by the electronic team.  

4. Select the correct plane to start modeling. The base of the component must be the xy-plane:

5. Search for the footprint drawing in the component datasheet.

6. Create a sketch to define the component footprint. Pay attention to compare the origin of the electrical component with the coordinate system of your model during the sketch of the footprint.

7. Import the model from the internet ( see HERE for more details ) or draw it from scratch. See the section Model your part or download the 3D model below.

   TIP: it is a good practice to create a middle plane to ease the assembling of the mate plug connector, unless one of the starting planes is already in the middle of the component.

8. Check that the component units are correct.

9. Color the pin 1 in red.

10. Fill in the following parameters:
    • TIPO = ELTR.
    • DESCRIPTION = same as Wingst.
    • Set ELTR_COMP_MAT as the material for the model. The MATERIAL parameter will be updated automatically.
11. Save the model in the right subfolder of cad‑libraries/libraries/electronics.

ATTENTION!!!

TO create resistor or capacitor read the follow page:

How to create capacitors and resistor using a family table

Mandatory coordinate system for plug components

When generating a plug component, it is mandatory to add a coordinate system called MATE_CONN with proper origin and orientation in both the plug component itself and its respective PCA connector. This will simplify the placement using Creo constraints.

With regard to the "on board" component, it is good practice to include a cosmetic of the plug component footprint as follows:

Create a copy geometry inside the components of the corrispettive plug component:

Use the sys MATE_CONN to fix the geometry

Copy all surfaces of the plug ( you can select a surface and keeping pressed SHIFT select an an adjacent surface, use CTRL to add other surfaces)

rename the features of the copy with plug_"filename"

Create a layer called "PLUGS," add the plug surfaces and keep them hidden as defaults.