Pin numbers and names

[ltrakal]

Since I'm at a new job now, I'm making libraries from scratch and I have some standards to follow for example pin names and number for resistors are 1 and 2. My question comes at the point when I have to make a diode that the package has actually three pins. Of course two of those pins are the same, let's say Anode. So in my schematic I have A and K for pin names and numbers in a diode. How I should manage a diode with three pins? Should I called the pin numbers 1, 2 and 3, or Just A, A and K?
Sorry if this is a stupid question but I found the same problem with transistors with four pins, so I would like to call the pin numbers and names the same but should i have two Anodes or two Emitters? or just called them with numbers?
Thanks for your help and sorry for the long post.

Laszlo

[randychase]

I think it is a good question.

You need to assign unique names to the pins, so a part that has two Anodes and one Cathode for example, can not have A, A, and K.

I use K, A1, and A2 for the alphanumeric.

Same with FETS that have tied pins.

Other people may have other solutions.

[ltrakal]

that's a nice solution for the pin names, thanks for you reply randy..
so do you use the same convention for the pad numbers? just A1, A2 and K? or you use numbers like 1,2 and 3?

Laszlo

[randychase]

Keep in mind that all parts in PADS have pin numbers no matter what. These are like gospel to the part.

I use the alphanumeric aliases whenever I can. On the part type, I tie the A1, A2, K to the correct pin numbers on the decal, because for that part, the alphanumerics should always be correct.

Now if you have a netlist from a schematic that calls out pin numbers only, it will override the alphanumerics, so be careful.

For example, let's say you use a TO-220 Transistor. Looking at the front, it is numbered pin 1 on the left, and then 2 and 3. Now you create a schematic that uses a negative 5V regulator and it's functional pin names are COM, OUT, IN. You create a Part Type that calls the TO-220 Decal, but assigns COM, OUT, IN to the pins in that order, even though the schematic CAE decal uses the standard Voltage Regulator of pin 2 being COMMON.

Everything is hunky dory! The system of names overrides the pin numbers. Everything matches up.

But... let's say you need a new design. You create a new part type that calls up the TO-220 decal, but you don't assign alphanumerics in the schematic. Using this netlist means that the nets will connect to pins 1-3 without regard for function.

For this reason, you just have to be careful when you use alphanumerics, and if you can, make the pin numbers match anyway.

I don't ever recommend using alphanumerics as a method of re-assigning pin numbers. You know like saying pin 3= pin 1 and so on. It's possible, but you can get yourself in trouble too easy.

[ltrakal]

so let me see if i understood, first i want to say that i'm really new in pads, i just installed it LOL... so my experience with other programs is when you have a pin in an schematic part you assign to it a name and a number, so supose in the diode case we have three pins:

NAME OF THE PIN NUMBER

A1 1
A2 2
K 3

the pin number MUST match the pad number, in the part footprint in the pcb library...
so my question is can i called the pads A1, A2 and K, i mean the name of the pin equal to the number of the pad? so i don't have 1, 2 and 3 for my pad number..

thanks again

[randychase]

I think it would makle it easier for you, if you looked at it differently.

Everything in PADS (powerpcb and logic) is driven from device.pin

Pin numbers are the key. Even if you assign names to them, it's still a pin number.

So you create a part, it will have a PIN 1, PIN 2, etc. After that, you can create an alias chart in the part type which defines the alphanumeric equivalent of that pin NUMBER.

So you make a part and it has PAD 1 and PAD 2 in the decal. Then in the part type, you assign CATH to pin 1 and ANODE to pin 2 (for example).

Similarily in Logic, it's still Pin 1 and Pin 2, but you can assign pin names to those pins, if I recall correctly.

[ltrakal]

thanks randy, i think it will be easier to put numbers, is less complicated, i just wanted to see if i can see in my netlist or in the schematic the pin number reflected as A or K, and not as 1 or 2..

thanks again

Laszlo

[randychase]

I agree, you should still assign pin names to the pins so you get A and K, it makes checking the netlist a lot better.

Just know that you are first dealing with numbers and then assigning pin names for both Logic and PowerPCB.

[ltrakal]

thanks one more time