Footprints are groupings of objects that include one or more objects of type Pad. Footprints are placed in the document as objects of type Device. They are defined and exported via Frame objects.

Objects for defining footprints

The following objects can be used to define a footprint:

To draw a footprint

The tools and the working environment are the same as those used for the production of the drawings and PCBs. For example, to draw the footprint of a component with container DO-41, perform the following steps.

  1. Defining the footprint with the Frame object

    A frame object must be designed for each footprint. These objects, graphically represented with a rectangle, allow you to delimit the objects that make up a footprint. Only objects that are entirely enclosed within the rectangle of the frame object will form the footprint.

    After drawing the frame object, you can use the edit tool to reposition the fields: part number, name and description.

    1. Activate the Library layer and create the Frame. See To add one or more frames.

    2. Open the properties window of the Frame object and specify the name of the footprint and a brief description. See Properties of the Frame object.

  2. Set the origin

    The origin point, or insertion point, must be specified via an object of type Hotspot. The point of origin is the point from which the dimensions of all the elements that make up the footprint are measured. The origin is also the centre of rotation of the footprint.

    1. Select the "Copper view".

    2. Select a 2.5mm snap grid. See Coordinate system bar.

    3. Add a Hotspot object to the center of the frame to specify the origin point, or insertion point, of the symbol. See To add a Hotspot.

    4. Place the origin of the reference system at the origin point of the symbol (center of the Hotspot object). See Set the origin via the Hotspot.

  3. Place pads

    Select the "Copper view" and place the pads.

    1. Select the optimal pad style for the component's terminal diameter. If it is not available, create it as follows:

      1. Choose the Settings » Style Manager command or click on the tool in the toolbar.

      2. Open the PCB group and click on Pad Styles.

      3. Click the Add button. The New Pad Style dialog box opens.

      4. In the dialog box, click on TH Pad for round lead and specify the value 0.78mm in the field Maximum lead diameter.

      5. Click on OK.

    2. Place the first pad in the point (x=-5.0mm, y=0.0mm). See To place a single pad.

    3. Place the second pad in the point (x=5.0mm, y=0.0mm). See To place a single pad.

  4. Draw the outline of the component to be printed on the PCB

    Select the layer "Top legend".

    1. Select the "Empty" fill style.

    2. Select the "PCB Silkscreen outline round" pen style.

    3. Draw a rectangle centered in (x=0.0, y=0.0) and dimensions (w=3.7mm, h=2.35mm). See To draw a rectangle by specifying the center and dimensions.

    4. Draw the line of the first terminal from the point (x=-1.85mm, y=0.0) to the point (x=-3.85mm, y=0.0). See To draw a single line.

    5. Draw the line of the second terminal from the point (x=1.85mm, y=0.0) to the point (x=3.85mm, y=0.0). See To draw a single line.

    6. Draw the polarity line from the point (x=-0.85mm, y=1.175mm) to the point (x=-0.85mm, y=-1.175mm). See To draw a single line.

  5. Add Reference

    For footprints, you must also specify an object of type Reference. See To add a Reference object.

  6. Add Value

    For footprints, you must also specify an object of type Value. See To add a Value object.

  7. Drawing the footprint courtyard

    Select the layer "Top courtyard".

    1. Draw an object Courtyard centered in (x=0.0mm, y=0.0mm) and dimensions (w=12.0mm, h=3.0mm). See To draw a rectangular courtyard.

  8. Drawing the solder mask

    Generally the templates for the solder mask are generated automatically and correspond to those of the pads, or are slightly larger. They create openings in the solder resistance layer at the welding areas. If you need to add additional areas in the solder mask in addition to those of the pads, you can use the graphic objects to draw on the layer "Top Soldermask".

    1. Select the layer "Top Soldermask".

    2. Draw graphic objects.

  9. Drawing the paste mask

    Generally the templates for the paste mask are automatically generated and correspond to those of the SMD pads, or are slightly smaller. They define the areas of the PCB where the solder paste is to be applied. . If you need to add additional areas in the paste mask in addition to those of the SMD pads, you can use the graphic objects to draw on the layer "Top Pastemask".

    1. Select the "Top Pastemask" layer.

    2. Draw graphic objects.

  10. Draw the black and white shape for assembly

    To draw the black and white outline of the component and any useful information for the assembly of the component on the PCB select the "Top assembly" layer. The view changes to "Top assembly".

    1. Draw the component terminals:

      1. Select the "White" fill style.

      2. Select the "Assembly Pin Outline" pen style.

      3. Draw a line from the center of the first pad to the center of the second pad. See To draw a single line.

      4. Convert the line to an object Shape. See Convert objects to different types of objects.

      5. Expand the shape to a thickness of 0.7mm. See To expand a shape.

    2. Draw the body of the component:

      1. Deselect objects.

      2. Select the "White" fill style.

      3. Select the "Assembly Body Outline" pen style.

      4. Draw a rectangle centered in (x=0.0, y=0.0) and dimensions (w=3.7mm, h=2.35mm). See To draw a rectangle by specifying the center and dimensions.

    3. Draw the polarity symbol:

      1. Deselect objects.

      2. Select the "Black" fill style.

      3. Select the "Empty" pen style.

      4. Draw a rectangle, with square corners, centered in (x=-1.0mm, y=0.0) and dimensions (w=1.0mm, h=2.35mm). See To draw a rectangle by specifying the center and dimensions.

    NotaNote:

    If the black and white assembly drawing is not inserted into the footprint, the component image or the drawing to be printed on the PCB silkscreen will be used.

  11. Drawing the graphic image of the component

    Select the layer "Top image", the view changes to "Top view".

    1. Draw the component terminals:

      1. Select the "2D Image Pin" filling style.

      2. Select the "2D Image Pin Outline" pen style.

      3. Draw a line from the center of the first pad to the center of the second pad. See To draw a single line.

      4. Convert the line to an object Shape. See Convert objects to different types of objects.

      5. Expand the shape to a thickness of 0.7mm. See To expand a shape.

    2. Draw the body of the component:

      1. Deselect objects.

      2. Select the "DarkSalmon" filling style.

      3. Select the "2D Image Body Outline" pen style.

      4. Draw a rectangle centered in (x=0.0, y=0.0) and dimensions (w=3.7mm, h=2.35mm). See To draw a rectangle by specifying the center and dimensions.

    3. Draw the polarity symbol:

      1. Deselect objects.

      2. Selezionare lo stile del riempimento "Nero".

      3. Select the "Empty Style" pen style.

      4. Draw a rectangle, with square corners, centered in (x=-1.0mm, y=0.0) and dimensions (w=1.0mm, h=2.35mm). See To draw a rectangle by specifying the center and dimensions.

Adding information to the footprint

You can add data and information to your footprints.

  • Footprint attributes. To add package and footprint information click on the Footprint attributes tab in the Properties of the Frame object dialog box.

  • Internal attributes. Internal attributes only have a data structure and can be associated with any object. The value of an internal attribute can not be displayed directly in a drawing. See Internal attributes of objects.

  • Graphic attributes. Graphic attributes are objects of type Attribute and can only be associated with the following object types: Group, Symbol, Sheet, Device. Graphic attributes can be used to display the value of internal attributes.

See also