Hey all, I’m trying to create a custom symbol and a footprint for the PB61304 switch. (Pictures linked below.)
Being new to electronics, and the few YouTube videos available don’t have similar information on their datasheet, I’m finding it hard to apply the information to my datasheet.
Hoping I can get some help here with some questions…
For the symbol you might save yourself some work by adapting the symbol SW_Push_DPDT from the standard libary. To add the LED lamp you could add a LED symbol, or put it in a separate unit. Also you can see from the standard symbol that the pin type should be Passive.
Ø1.0 is shorthand for 1.0mm diameter. The hole should probably be made slightly larger.
Nah, there’s no need for a symbol’s layout to look anything like the physical part’s layout. Put the diode horizontally on top of or below the switch.
This approach means that you may have to run wires to the LED even if they are connected to a faraway part of the circuit. You could avoid that by using labels to make the connections.
The other approach is the put the LED in a separate unit from the switch. Multiunit symbols are commonly used for stuff like logic gate ICs where each gate has a unit, and the power pins are in a separate unit too.
Whenever placing pins, make sure you use a 50mil grid, otherwise your symbol won’t connect on your schematic.
All the tools to make the circles and lines are under your pin icon. Try them out beside your new symbol, then erase afterwards.
To get a thick line, draw a thin line and then double click to edit its thickness.
Use a fine grid to to draw a diagonal line.
2nd icon from the bottom is an “anchor”. This is where your mouse grabs your symbol to place it on the schematic. Click that icon and then click mouse again when you have the cross hairs on a pin end, otherwise your symbol pins won’t land on the schematic grid correctly.
Footprint is OK but, you might want to move the anchor to a pad or the centre of the footprint instead of a corner.
There is not much copper on the pad and it needs to be mechanically robust because it is going to be pushed.
Maybe increase the outside diameter of the pads, maybe change the shape to oval?
So when I place the symbol in the schematics, I will have to connect L1 to pin3 and L2 to pin6?
Or can I do this in the symbol editor now so I don’t have to worry about it later?
No.
Worry about it later. Keep them separate for now.
If you want the LED permanently on it will need to connect to a supply. If you want it to indicate the switch position, one side of the LED will have to join a switch pad. The pad depends on if you switch the LED to Gnd or V+ or whether you want the other set of contacts to be open or closed.
Are you saying you think you have to connect the LED pins to the switch pins? Why? As far as I can tell the LED just happens to be in the same housing and you have to arrange to supply current to it independently. How that’s done depends on your design.
Well strictly speaking not necessarily. For example the switch might be an input to a microcontroller and after reading the switch and checking other prerequisites it turns on the LED to indicate “all good”.
Oh, and check what kind of LED it is, with built-in current limiting resistor or just a bare LED. The symbol seems to indicate a bare LED, but without reading the electrical characteristics one cannot say. If it’s a bare LED you need a current limiting resistor, and its value is calculated from the LED forward voltage, desired current, and supply voltage. Otherwise if you wire it directly across the power supply, it will glow brightly. Once! Very briefly!
From your latest picture, it seems as if you are drawing a silkscreen outline straight over the pads. This is not considered to be good practice, so consider making it around the entire part. And yes, the datasheet is quite useless as the body size itself isn’t dimensioned (I tried making a 3d model for practice).
Your footprint anchor has moved, but consider making it symmetrical along the y-axis aswell (i.e. footprint anchor centered between L1 and L2, and pads 2 and 5.
Just a note: it might not be important in this case, but have you considered if the footprint or datasheet drawing are from the top or bottom of the part or PCB? I mean that as in, if you hold the part in your hands, with the L2 pad near you and L1 facing away from you, are pads 1,2 and 3 then on your left, or right side? I guess for the switch functionality there is rotational symmetry anyway, but not for the L1 and L2 pads.
Which reminds me, consider marking one of the pads as positive or negative on the silkscreen layer. Not sure how the part itself is marked, but the datasheet does seem to imply a visible difference on one side.
Also, are my eyes deceiving me or is your hole size for L1 larger than the others?
EDIT: You also mentioned 1.3 mm hole size for 1.0 mm pins. The datasheet shows pin size of 0.3 x 0.6 mm and suggests a hole size of 1.0 mm? As for the pad size: I usually just double the hole size, so 1.0 mm hole and 2.0 mm pad (or 2x3 if you like oval pads).
