A PCB decal is a representation of the outline, terminals, and attributes of an electrical component and is used in placement and routing of the component during the design layout process.
You can use the PCB Decal Editor to create new decals or to modify existing ones. To open the Decal Editor, go to Tools > PCB Decal Editor.
The operations listed below will help you to create a basic decal or edit a preexisting one.
The location of a decal's origin affects how decals attach to the cursor when you move a component in the Move by Origin mode. It also affects how pick and place machines populate the board with components. Use one of the procedures below to set the origin of the decal.
Terminals are the pads or pins associated with a decal. The Add Terminals dialog box will allow you to easily create terminals for your decal:
In the Add Terminals dialog box, in the Start pin number area, type values in the Prefix and/or Suffix boxes for the pin numbering. A preview of pin numbers based on your input is displayed below the boxes.
Alphabetic and numeric values can be used in either box. For example, A1 or 1A.
For a single numeric, use either Prefix or Suffix box, and void the other box.
In the Increment options area, choose what to increment by clicking either the Increment prefix or Increment suffix option.
In the Step value box, type a positive or negative number by which to increase or decrease the pin numbers with consecutive or stepped values.
If using alphanumerics, you can select the Use JEDEC pin numbering check box to ensure that legal alphanumeric values are used. This option only ensures that valid alpha and numeric combinations are used. To arrange rows and columns according to JEDEC, use the Assign JEDEC Pinning option on the Tools menu.
You can also add terminals by replicating an existing terminal using Step and Repeat.
You can easily add an array of terminals using the Step and Repeat function.
Terminals are replicated with associated coppers.
You can create copper in the decal and associate it with a pin to create a custom pad shape or heat sink. You can also create unassociated copper heat sink or shielding shapes that move with the decal in the design. To create a copper shape, follow this procedure:
You can associate a drawn copper shape with a terminal/pad. This assigns the copper shape the same net connection as the terminal/pad. You can also use associated copper to create custom pad shapes.
If you are using the associated copper to create an odd shaped pad, maximize the pad shape inside the overlapping associated-copper shape. The underlying pad is still the routing target and also the connection point for thermals if this pad will ever be connected to a copper pour or plane area. If associated copper surrounds the terminal pin by a large amount it could prevent thermal spokes from being generated.
Routing is only completed to the center of the pad. Any thermal connections are made to the pad only, not to the associated copper shape.
You can customize the pad stacks of the pins in your decal. You can choose to customize one pin, or multiple pins simultaneously.
If any of these outlines do not appear after you create them, the color set for the item is probably the same as the background color. Set a different color in the Display Colors Setup dialog box (Setup > Display Colors).
The assembly outline and assembly refdes are used on the assembly drawing to define the exact outline and identify the body of the part. It shows where the part is to be placed during the board assembly process.
Add a second reference designator label on the Assembly Outline Top layer. The reference designator label should be large and located inside the outline.
The silkscreen outline is printed on the board, and remains visible on the board after the part has been placed. This outline, along with its reference designator, pin number and polarity labels, identifies the part and its pins to persons assembling, testing, or servicing the board. The silkscreen also serves as a nudge outline if no actual nudge outline exists on Layer 20.
Silkscreens for large components with many pins often have miniature dots or pin numbers visible next to selected pins to make it easier locate a pin on the board during testing or troubleshooting sessions. If you use text in the decal for these, they will not be movable when the component is placed in the design. Use labels instead; labels can be moved or deleted in the design if necessary.
Some parts need additional spacing compared to others to allow for machine-placement on the physical board. The placement (or nudge) outline is utilized to define these spacings.
You can use a larger outline on layer 20 to ensure that your design placement is correct even though you apply the same body-to-body clearance for all components. On layer 20, draw the 2D line item(s) defining the nudge outline by selecting the Drafting Toolbar icon to display the Drafting Toolbar, then click the 2D Line icon.