Removing Unused Pads & Adding Teardrops to a PCB in Altium NEXUS

Pads and vias are an essential ingredient of a modern PCB design. As well as providing mounting points for components, pads, along with vias, allowing a net to traverse the different layers of a PCB as it travels from one component pin to another. Pads and vias come at a cost though; they consume valuable board space, they create impedance mismatches for high-speed signals, and they create holes in large copper areas defined by polygon pours.

To help reduce their impact on copper areas, Altium NEXUS includes an Unused Pad Shapes removal tool. The tool scans all pads or vias in the design and removes the pad shape from each layer for which the pad or via is not used (meaning it has no other objects touching it on that layer). Polygons that surround that pad or via then only need to create the specified clearance to the pad or via hole instead of to the edge of the unused pad shape. In some situations, such as under a BGA, this can recover a substantial amount of copper lost in polygons.

In addition, teardrops are often added to a routed PCB design to create stronger track-to-pad, track-to-via, and track-to-track connections. This is valuable when the design objects are very small and is particularly valuable for drilled pads and vias, because misalignment between the drill center and the pad/via center can result in the drill hole removing much of the copper connecting the track to the pad/via.

Removing Unused Pad Shapes

This tool is intended to be used once the routing is complete, before the fabrication files are generated. To remove unused pad shapes, select Tools » Remove Unused Pad Shapes from the menus, the Unused Pad Shapes dialog will open, as shown below.

Configure the dialog options as follows:

• Scope
  • Vias - examine all vias in the design, and remove unused pad shapes.
  • Pads - examine all pads in the design, and remove unused pad shapes.
  • Both - use this tool to target the scopes of both vias and pads.
• Operation
  • Remove unused - use the tool to remove unused pad shapes.
  • Restore unused - use the tool to restore removed pad shapes to all vias.
  • Update unused - use the tool to restore, then remove unused shapes.
• Selected only - examine only selected vias or pads, and remove unused pad shapes.

• Preserve pads on start and end layers - a pad or via might not use the pad shape on the outer most layers that its structure exists on, these outer-layer pad shapes can be retained if required.

  Confirm that pad-less-outer-layer pads or vias are supported by your fabricator before disabling this option.

Notes About Using the Unused Pad Shapes Removal Tool

• To ensure that existing polygons recover all available copper area that was lost to unused pad shapes in pads and vias, run the Tools » Polygon Pours » Repour All command after removing unused pad shapes.

Using Teardrops

Teardrops are especially valuable in flex designs to help prevent a crack forming where the track meets the pad/via or when the drill hole is not in the center of the pad/via. Teardrops are created out of region objects, requiring only one region per teardrop, which can have either straight or curved edges. Teardrops can also be added to the junction of two tracks at both a T-junction and a neck-down junction.

Adding Teardrops to a Design

Teardrops are added (or removed) by selecting Tools » Teardrops from the main menu. When the command is selected the Teardrops dialog will open.

Teardrops can be added and their properties defined as follows:

• Working Mode - the tool can be used to both Add or Remove teardrops.
• Objects - define the coarse-level scope of teardrop addition/removal. Either consider all objects (All), or only those objects currently selected in the workspace (Selected only). This setting is used in conjunction with those object types enabled in the Scope region of the dialog.
• Teardrop style - the edge of the region object used to create the teardrop can be straight (Line) or Curved. This option is available only when adding teardrops.
• Force teardrops - if this option is enabled, teardrops will be applied to all vias and/or SMD pads, even if this results in a DRC violation. This option is available only when adding teardrops.
• Adjust teardrop size - if this option is enabled the teardrop size is automatically reduced to meet applicable design rules.
• Generate report - create a text report listing both successful and unsuccessful teardrop sites. This option is available only when adding teardrops.
• Scope - enable which objects to consider for teardrop addition/removal - Vias, SMD Pads, Tracks, T-Junctions - in conjunction with the coarse-level scoping defined in the Objects region of the dialog. When adding teardrops, you can configure teardrop sizing as follows:
  • Via/TH Pad - specify the length and width of the teardrop as percentages of the via/thru-hole pad diameter (d). The defaults are 30% and 70%. Click the blue percentage values to change these as required.
  • SMD Pad - specify the length and width of the teardrop as percentages of the attached track width (w). The defaults are 100% and 200%. Click the blue percentage values to change these as required.
  • Tracks - specify the length of the teardrop as a percentage of the attached track width (w). The default is 100%. Click the blue percentage value to change this as required.
  • T-Junction - specify the length and width of the teardrop as percentages of the primary track width (w) (the horizontal track in the image). The defaults are 300% and 100%. Click the blue percentage values to change these as required.

For more information on the dialog settings, refer to the Teardrops dialog page.

Notes About Using Teardrops

• Teardrops are automatically removed whenever an edit action is performed on either the pads/vias or the track. Click and hold on a teardropped pad to observe this behavior.
• Teardrops can be re-added by re-running the Tools » Teardrops command. There is no need to remove existing teardrops before re-running the command.
• Current teardrop settings are stored as an environment setting on the PC, not in the PCB file.