Quadcept - STEP 2: Place Pads

Quadcept : Creating Footprints

Pads are land shapes for electrically connecting PCB component terminals.

The following will explain how to place pads.

Placing Pads

Place a component pad.

(1)	Select [Draw] => [Pad] => The "Pad" screen will open.

(2)	Configure each setting and then click "OK"
	Configure settings for the pad type, size, solder resist, etc. For more details on each setting, refer to "Pads".

* Array Settings can be configured by specifying the Number, Direction, and Interval.

(3)	Click on the document to place it

Type	Content
SMD	Pad without a hole. Pad shape for surface mounted components such as Chip components.
Through	Pad with a hole. Pad shape for through hole mounted components such as Dip components.

Item	Content
Top	Sets the land size of the Top surface.
Inner	Sets the land size of the Inner layer. (For the Inner layer, all are the same size.) * Only the "Through" pad type can be configured. * When no routes or planes are connected to the Inner layer, it is possible to use the option for toggling deletion of the inner layer land ON/OFF. For more details, refer to Hide Unrouted Inner Layer Pad Land and Via Land. * When each layer is set individually by placing a check for "Show all layers", the settings for shape, size, etc., for each layer will have priority.
Bottom	Sets the land size of the Bottom surface. * Only the "Through" pad type can be configured.

Item	Content
Electric	Sets the copper layer. These are land settings.
Paste	Sets the area where paste solder is applied. * Paste solder is also referred to as solder paste, solder cream, cream solder, etc. This is data used for creating metal masks created for component auto mounting.
Solder	Sets the solder resist area. Here, the area outside of the resist coating is specified.

Item	Setting Contents	Content
None	None
Circle	Width (Diameter)
Square	Width Radius
Oval	Width Height
Rectangle	Width Height Radius
Imitation	One Side (One Side over size)	Settings can be configured based on the size of the land (Electric layer). When it is a positive number, it is larger than the land, and when it is a negative number, it is smaller than the land. If it is the same size as the land, specify "0". This is convenient because you can specify using One Side over size for Customized Pads or Cut Pads. * This can only be selected when the layer is "Paste" or "Solder".

When a Radius is input for a Square or Rectangle, you can specify the roundness of a square pad.

* This can only be set when "Through" is selected as the pad type.

Item

Content

Shape

Sets the drill shape and size.

Circle	Angle	Oval	Rectangle

W: Width
H: Height

Tolerance

Sets the tolerance for the drill diameter. This is shown for NC Drill Files and Print NC Drill Lists.

Plating

Possible to set whether to plate a hole. Normally, "Plating" should be checked for component pads.

When Multi-pin Arrangement is enabled, multiple pads can be placed together by specifying the Number, Direction, and Interval for pad placement.

Item	Content
Number	Specifies the number of arranged pads.
Direction	Select either "Top to Bottom", "Bottom to Top", "Left to Right", or "Right to Left".
Interval	Sets the pad-to-pad interval.
Snap Cursor to Center	Check for whether to place by snapping the cursor to the center of multiple pads. If this is not checked, the cursor snaps to the first pad.

For more details about the pad sizes that our company uses, refer to "Reference: Pad Dimensions".