www.eda.co.uk

One of the most common questions we get for Altium Designer is how to create slots or square holes in PCB.  In this TechWatch I've taken some information from Altium's most commonly asked questions to help answer this. 

Version Altium Designer 6.3 onwards

With the release of Altium Designer 6.3, slots and non round holes in pads are now supported by adding slot and square style cut-outs in pads. These new options can be found within the Pad Properties dialog box along with a new preview area.

The outputs for the slots and square holes are generated as part of the NC-Drill, with separate files for each type based the CNC-7 format

Details of drill type will also appear in the Drill Drawing Legend for your manufacturer to see. This is a special string you place on your PCB, which is interpreted upon output.  use the command Place » Text String and select the .Legend string to place on the Drill Drawing layer.

Note: Best check with your PCB manufacturer if they are able to support the output manufacturing files from the new release. Always alert your manufacturer that there are slots on board.

Versions Previous to Altium Designer 6.3

With earlier versions, the common practice includes describing the slot on a mechanical or keepout layer, with text instructions included. Some designers will place a cluster of overlapping through-hole pads or vias to define the area to be drilled out, although this may ruin drill bits.

As methods of fabrication for irregular holes differ from one board house to the next, you should find out how your board house prefers these to be handled.

So there are three ways to define slots.

1.  Add details to a mechanical layer that is given to the manufacturer
2.  Add multiple overlapping Pads or Vias
3.  Use CAMtastic NC Drill features

For an example of this layout, where mechanical layers are used to depict slot information, please see the LiveDesign Evaluation Board example, 'EB1_Spartan_II_1_02.PcbDoc'

The PCB is found in the folder, C:\Program Files\Altium Designer 6\Examples\LiveDesign Evaluation Board\Reference Designs\LiveDesign Evaluation Board (EB1 EB2)\Spartan_Specific\Spartan III BGA456 1.02 EB1

Details are stored on the mechanical layer 'Plated Route Details'. Here you will see lines detailing the routed slot for components J1, J6, and J2S on this board. Switch to single layer mode to see the primitives on each layer (single layer mode is toggled by the shortcut shift+s).

The routing detail is included in the component so it moves with the component if shifted.

Before you adopt this approach, check with the PCB Manufacturer to see if this method of defining slots is acceptable.

For this setup, the pad and slot area have been built up as follows to provide enough information to the manufacturer.

•  A multilayer pad with hole set to 0 units. This defines the pad area.
•  A start and end multilayer pad on the ends of the slotted area. The hole size for these pads are set to the width of the slot cut-out.
•  A line on the 'Plated Route Details' mechanical layer placed from the centre point of the start and end pads. The line width is the width of the slot cut-out.

You also need to carefully consider the internal plane connections for slotted pads. For solid connections and large enough voids on internal planes, the thermal reliefs and voids will need to be setup manually.
On this PCB example, thermal reliefs have been used - created manually with arcs and lines. See pad 1 of component J6.
In conjunction with the power plane connect rule for the pad set to Direct connect.

Refer to the design rules, to see the Power Plane Connect Style design rule set to Direct Connect for these slots 

(rule: PlaneConnect_Obround_Pads, plus a class has been set for these pads in Design » Classes to make it easier to setup in a rule.)

You can choose the simpler option to direct connect these slotted pads if you are not really concerned with thermal reliefs for ease of soldering when assembling the boards.

Finally, slotted pads which do not connect to the plane such as pad 2 and 3 of J6 need copper void areas over the cutout. Hence adding a line or other object over the cutout on the internal plane will act as void area, since planes are output in the negative.

As you output your Gerbers or ODB++ files, carefully review the connections to internal planes. Remember to include the Plated routing details mechanical layer and advise your PCB manufacturer of the slotted pads on your PCB.