Review PCB Library Design - NO/NC Push Button

Thread Starter

Digit0001

Joined Mar 28, 2010
100
Hi All,

I would like a review of the following library i have created for the APEM IP5PAD NO/NC Momentary Push Button. The main concern is the connection with P$1 and P$2 since they are both Normally Open functions I have wired them together and left P$3 as the NC function as per datasheet. The project i am working on only requires the NC function, hence i have not included the NO schemactic. See below snippnet from Eagle software and attached datasheet.

1590982771985.png
1590982858419.png

A two pin push button is straight forward but becuase you have an additonal pin it becomes a bit confusing how i should wire it.
Any assistance would be greatkly appreicated.
 

Attachments

jpanhalt

Joined Jan 18, 2008
9,740
Is this what you are trying to design, except with PCB terminals?
1590995218944.png
That is not the same as you have drawn. A lot of pushbutton switches have pads that are internally connected, for example:

1590995661410.png
I use this as the symbol connected "OR:"
1590995893329.png 1590995947514.png

Assuming there are only 4 pads and both NC and NO functions on your switch, I would use the manufacturer's symbol (shown above) dressed up anyway you want. The only thing that is important is the pad layout. In your case, it doesn't appear you need an OR connection.

You might also want to reconsider the pin direction assignment. Otherwise, you may be nagged with "I/O pin unconnected" warnings in ERC.
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
If internally the push buttons has 4 pads, than physically it means it must have 4 pins?

I thought it was three due to the image on the datasheet but now it makes sense.
 

jpanhalt

Joined Jan 18, 2008
9,740
Your symbol looks fine. As I said before, you can leave them as "I/O," but I think you will regret that later. Depends (maybe) on your ERC settings. I would make them "PAS."

As for your Device/Footprint, are you sure those pin numbers match your symbol? Opposing pins might be switched pairs. The datasheet doesn't show that specifically, but for the LED + switch, it appears to be that way.

You haven't mentioned the program you are using. In Eagle, changing the ratio of hole diameter to oval pad size can be less than obvious. Read about "restring," if your version still has that. If you want an oval pad, you can also chose a pad with an offset hole. That will ease your crowding if arranged perpendicular to the axes. You can also use a round, square, or hex pad. They don't all have to be the same. Finally, if your CAD program supports plated slots, I would strongly suggest considering that.
 

shortbus

Joined Sep 30, 2009
7,760
@Digit0001



View attachment 208664


If that's the image of the switch, it doesn't seem like it's even meant to be PCB mounted. The holes in the tabs are usually used to solder attaching wires. And how would the nut for mounting to a panel work if it is PCB mounted?
There are other push button switches that are made for PCB mounting.
 

jpanhalt

Joined Jan 18, 2008
9,740
I think the TS has the PCB version:

1591020915421.png

Unfortunately, that datasheet is silent on the layout. Maybe there's a more detailed DS somewhere else. I agree, we are all guessing on the footprint. I suspect it is through-hole. Maybe straight PC terminals means pins like on a DIP?
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
i am using Eagle software, and as per the datasheet i beleive there is an option for through hole
Not sure if Eagle has plated slot, the method i would be using is applying the milling layer over the pad hole to the desired area.

The datasheet is not clear on the pin arrangement as such i have based on the labelling of NO or NC to determine the pin arrangements
 

jpanhalt

Joined Jan 18, 2008
9,740
i am using Eagle software, and as per the datasheet i beleive there is an option for through hole
Not sure if Eagle has plated slot, the method i would be using is applying the milling layer over the pad hole to the desired area.
That is dependent on the version. It really depends on how Eagle CAM handles it -- not how you draw it. See Oshpark.com for a discussion. If you can get a definitive answer from your PCB FAB house, so much the better. I could not a few months ago. Just gibberish. It's been three months for JLCPCB to respond, and it hasn't.

The datasheet is not clear on the pin arrangement as such i have based on the labelling of NO or NC to determine the pin arrangements
If it's not in the datasheet, the only option is to buy the part and measure it or go to a part with a complete datasheet. You could also try contacting the manufacturer. Sometimes they respond; sometimes not. The cost of mistakes is not in dollars, but in time lost fixing errors.
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
I am using Eagle version 9.6.1 .

I will see if the manufacturer has a complete datasheet, if not i may have to purchase one
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
Can anybody tell me if having overlapping solder masks on footprint pads can cause solder bridging issues. see attached image
1592339072892.png
 

jpanhalt

Joined Jan 18, 2008
9,740
Why such huge pads with such small holes? Have you read any of my posts?

Yes, if there is no soldermask between pads, getting a short is more likely, but definitely not a certainty.
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
As i will be manufacturing through OSHPark, i have followed their instructions to create the plated slot.

dimension:
pad diameter: 1.9mm
plated slot: 2x0.5mm (initially 0.4mm however OSHPARK minimum is 0.5mm for guarentee facbrication)
annular ring = (pad diameter - drill hole)/2 = 0.7mm

my only concern is my pad diameter maybe a bit to big or not enough.
 

Thread Starter

Digit0001

Joined Mar 28, 2010
100
1) Created the pad size
2) Created the drill hole
3) Drew a line for the plated slot in the milling layer with an 0.5mm width
 
Top