How to define a slot in footprint

I am wondering about what are the ‘best practices’ to produce a slot as part of a footprint.

For a particular connector, there is a slot used for a ‘snap-in’ plastic part of the connector which assists in retaining/ supporting the connector.
This does not need to be electrically connected.

The particular slot is 3.2mm long by 2.2mm wide.

Looking at previous postings, there appears to be two possible approaches:

  1. Add a ‘NPTH, Mechanical’ ‘oval’ ‘pad’ in the footprint editor.

In addition to defining the hole shape oval X and Y size, is it necessary to also define the ‘pad shape’ as being oval and of the same dimensions as the oval hole?

If I understand correctly, if the ‘Pad size X’ and ‘Pad size Y’ values were set to zero (or less than the hole dimensions), it would imply/ result in solder mask being place over the hole (i.e., empty space!) - which may make the PCB fabricator unhappy?!

If on the other hand the pad is made somewhat greater than the hole dimensions, it would result in the solder mask being spaced away from the edge of the hole?
Would that be a good practice, bearing in mind manufacturing tolerances for mask placement, etc.?
Refer graphic:

  1. Define the slot in an ‘Edge cuts’ drawing.

Looking at the JLCPCB capabilities web-page, they state:

Min. Plated Slots
0.5mm
The minimum plated slot width is 0.5mm, which is drawn with a pad.


Min. Non-Plated Slots
1.0mm
The minimum Non-Plated Slot Width is 1.0mm, please draw the slot outline in the mechanical layer (GML or GKO)

If I understand the JLCPCB capabilities correctly, for the current application, I should use approach 2, i.e., define the slot in an ‘Edge cuts’ drawing.

Is the ‘GML or GKO’ layer that JLCPCB refer to the Kicad ‘Edge cuts’ layer?

For other applications, I envisage a need for Plated Slots so am also interested in understanding the best practices for such slots.

1 Like

With my four used pcb-manufacturers both approaches work well. (both tested after switch to Kicad on the first kicad-project).

Currently I use mostly option 1 if the slot is only a straight slot:

  • NPTH, mechanical
  • hole shape oval with desired values for x/y. These values should be >= the minimum values for nonplated holes+milling according to the pcb-manufacturer (0.8mm in my case)
  • 0 < pad x/y <= hole x/y (pad > 0 because otherwise it’s hard to select)

The advantage of using a pad instead of a drawn edge.cuts-graphic: changing the pad-dimension (for modifying the slot) is easier than modifying a graphic shape.

For non-straight slots (for instance some complicated isolation barrier below a ACDC-module) I use method 2 with a drawed polygone on edge.cuts.

1 Like

My assumption for the JLCPCB’s distinction (this is an assumption with only a basic understanding of how PCBs are fabricated) is they probably use different CNC machines for plated and non-plated board cutting. PTH holes/slots are done before copper etching because the bulk of the plating is done by electroplating. Boards start with copper thinner than the finished copper thickness. Holes and slots are milled into the board panel. Then the boards get a very thin layer on all exposed surfaces with a chemical process, I’m not sure if the bare copper reacts to the chemical process or not. Then the boards are electroplated that brings both the plated holes/slots and the surface copper to the finished thickness. Then all the etching, masking, and silkscreening is done. If there are any v-scores than this is when they are done, older processes score across the entire fabrication panel. There may be newer processes (that I’m unaware of) that can start and stop a v-score in the middle of the fabrication panel. Finally, the fabrication panel is loaded into a CNC machine that cuts NPTH holes, NPTH slots, drills mouse bites (just another type of NPTH hole as far as the fabrication process is concerned) and cuts the individual finished boards (potentially different boards for different customers) out of the fabrication panel. Because the first CNC process and the last CNC process can potentially be different machines, they can have different tool loadouts. In JLCPCB’s case, they probably don’t have any milling tools that are smaller than 1mm on the last machine.

For your design, you don’t need to have NPTH holes for your plastic retention fingers. But does it really hurt to have them plated? If not, what is stopping you from simply designing your footprint with a PTH slot using a minimum annular ring? (Minimum defined by you, but constrained by the minimum published spec from your manufacturer.)

As @SembazuruCDE suggests, it seems that JLCPCB indeed uses different processes for each alternative.

This impression is reinforced by such as the following from their ‘Capabilities’ page:

Rectangle Hole/Slot
Don’t support
Rectangle/Square Slots, we don’t make rectangular or square plated holes,only make oval or round plated slots.

For non-plated slots, rounded corner-rectangular or square slots are supported. The recommended minimum size is 3x3mm.

Also (in what appears to be a recent additional statement), they state:
PTH
0.2mm
We make NPTH via dry sealing film process, if customer would like a NPTH but around with pad/copper, our engineer will dig out around pad/copper about 0.2mm-0.25mm,
otherwise the metal potion will be flowed into the hole and it becomes a PTH. (there will be no copper dig out optimization for single board).
[This statement/ sentence seems somewhat overlong and is not completely understandable, i.e., what are the alternatives and pros/ cons of each possibility/ variant?!]

The general impression is that using PTHs potentially simplifies the manufacturing process and offers the potential benefits of (if required) finer geometries.

Yes, “it [doesn’t] really hurt to have them [the slot] plated” so probably I shall go for a PTH slot with a small pad size (if I understand correctly, this relates to the “minimum size of annular ring around through hole pads” which is specified as being 0.25mm). [There is not a lot of separation from other pads so the “annular ring” would need to be around the minimum possible.]