Many devices connected with one footprint - question

[jprzezdziecki]

Hi, I'm just starting to build my own library. It's well explained but something is confusing for me.

I have created to JFET N-Channel devices and connected them to the one TO92 package. Unfortunately, these devices have different pinout. Should I create two different (named) T092 packages for those devices? How this should be done. When I use the same TO92 package it conflicts with a second device with different pinouts (the connected pinouts are wrong).  

I have checked with "transistor-fet.lbr" and 2N3819 and BF245 have different pinouts BUT they are connected to the same TO92 package. 

Thanks Jurek

[skndungu75TT4N3]

Hello @jprzezdziecki 

From what I understand from your posting is that there is a conflict in the names and hence Eagle can't save your new library. What I would propose you do is to name the library itself, let's say for example Transistor_2N3819, or Transistor_2N3904 or any other name - then for the symbol name, you can name it 2N3904 then for the Footprint Name call it that particular package"TO92", in that case, there would be no conflict as the "TO92" is the name of the footprint not the library what normally conflicts is library name rather than the symbol or footprint name.

May I also point out the if one library has several symbols and footprints then the names should also be different.

Just watch this and your symbols will be okay

Please let us know if this helps!! 

// Mark as a solution if it solves your concerns thanks 

[one-of-the-robs]

---

@jprzezdziecki wrote:
Should I create two different (named) T092 packages for those devices? How this should be done. When I use the same TO92 package it conflicts with a second device with different pinouts (the connected pinouts are wrong).  

I have checked with "transistor-fet.lbr" and 2N3819 and BF245 have different pinouts BUT they are connected to the same TO92 package. 

---

I think @skndungu75TT4N3 misunderstood your question, or at least understood it differently to me, which isn't necessarily the same thing.

There is nothing to stop you associating the same package with multiple devices and no reason they can't have different pin-outs. Look at the TTL library, for example - many devices sharing the DIL14 package with totally unrelated pin-outs.

The schematic symbol has a set of "pins" with names that you assign when you create it. For a FET, these will typically be "G", "D" and "S".

The package has a number of "pads" with names that you assign when you create it. In most cases, the JEDEC or other appropriate spec. allocates plain numbers, "1", "2", etc., although sometimes there are special cases.

When you create a device, that device contains one or more symbols as "gates", and one or more packages associated with "variants". Since you name the variants, you can easily identify them. Within this association, you define a mapping from symbol pins to footprint pads.

There is nothing to stop you assigning the same package/footprint to multiple variants. If you do so, you can define different pin/pad mappings for different pin-outs.

There is one caveat. Although I said above that the footprint normally has simple numbers for the pads, some people draw footprints and give functional names to the pads. This is bad practice, especially if they have named TO-92 pads as "G", "D" and "S", because not only do some FETs have different pin-outs, but some (many!) TO-92 devices are not FETs. If your library has such a "customised" TO-92 footprint, you can still re-allocate the pin-out on your second device variant, but it gets confusing. It's better to rename the pads. Eagle will automatically adjust any devices using that footprint, so it's not hard.

[jprzezdziecki]

yes, you are right. Thank you for this answer because you raised exactly the problem I encountered. I think my problem is not understanding the "variants" issue. Let me clarify again what I am struggling with. At the moment I have two FET transistors - 2N5457 and BF245. They have completely different pinouts but I have connected these devices with one TO92 package. And here a problem appeared - BF245 has GSD configuration relative to pins in the order 1,2,3, while 2N5457 has DSG. And here I have a connection conflict - a change in one device causes a configuration change in another As I understand to solve it, do I have to define two different variants?

[jprzezdziecki]

---

@one-of-the-robs wrote:

---

@jprzezdziecki wrote:
Should I create two different (named) T092 packages for those devices? How this should be done. When I use the same TO92 package it conflicts with a second device with different pinouts (the connected pinouts are wrong).  

I have checked with "transistor-fet.lbr" and 2N3819 and BF245 have different pinouts BUT they are connected to the same TO92 package. 

---

I think @skndungu75TT4N3 misunderstood your question, or at least understood it differently to me, which isn't necessarily the same thing.

There is nothing to stop you associating the same package with multiple devices and no reason they can't have different pin-outs. Look at the TTL library, for example - many devices sharing the DIL14 package with totally unrelated pin-outs.

The schematic symbol has a set of "pins" with names that you assign when you create it. For a FET, these will typically be "G", "D" and "S".

The package has a number of "pads" with names that you assign when you create it. In most cases, the JEDEC or other appropriate spec. allocates plain numbers, "1", "2", etc., although sometimes there are special cases.

When you create a device, that device contains one or more symbols as "gates", and one or more packages associated with "variants". Since you name the variants, you can easily identify them. Within this association, you define a mapping from symbol pins to footprint pads.

There is nothing to stop you assigning the same package/footprint to multiple variants. If you do so, you can define different pin/pad mappings for different pin-outs.

There is one caveat. Although I said above that the footprint normally has simple numbers for the pads, some people draw footprints and give functional names to the pads. This is bad practice, especially if they have named TO-92 pads as "G", "D" and "S", because not only do some FETs have different pin-outs, but some (many!) TO-92 devices are not FETs. If your library has such a "customised" TO-92 footprint, you can still re-allocate the pin-out on your second device variant, but it gets confusing. It's better to rename the pads. Eagle will automatically adjust any devices using that footprint, so it's not hard.

---

Suppose I want to assign exactly the same TO92 footprint (same pad size, shape, etc.) to two different transistors that differ by pinout - in the description I define two different "variants"? However, if two footprints are slightly different (e.g. different pad shape), then I have to create two different footprint names, e.g. TO92 ROUNDED PADS / TO92 SQUARE PADS? In this case, the description of the "variants" will not be enough?

[one-of-the-robs]

Look up some of the tutorials on library creation. There are some very good ones out there.

How you deal with different transistors having different pin-outs on the same package will depend on how you want to organise your library.

Option 1:

The library contains a "DEVICE" for each transistor type. Thus you would have a DEVICE called "2N3819" and another called "BF245". Each of these devices will only require one variant, which can have a blank name. If you want to support both round and square pads, you could do this by adding two variants of each device, one called "-R" and one called "-SQ", assigned the relevant two footprints. Then, in your schematic, you can add a "2N3819-R" or a "BF245-SQ" or whatever.

Option 2:

The library has a single device called "FET". This device has many variants. One of these variants would be "-TO92-GSD", associated with the TO-92 footprint and with the connections made for GSD pin-out. Another variant, called "-TO92-DSG" would use the same footprint but with different connections. In your schematic, you add a FET-TO92-DSG and set its VALUE to "2N3819" (or whichever way round they are).

Personally, I prefer option 1 most of the time, although option 2 can feel easier for a quick-and-dirty "oh, I think I'll use this other TO-92 FET that I haven't used before".

[jprzezdziecki]

---

@one-of-the-robs wrote:

Look up some of the tutorials on library creation. There are some very good ones out there.

How you deal with different transistors having different pin-outs on the same package will depend on how you want to organise your library.

Option 1:

The library contains a "DEVICE" for each transistor type. Thus you would have a DEVICE called "2N3819" and another called "BF245". Each of these devices will only require one variant, which can have a blank name. If you want to support both round and square pads, you could do this by adding two variants of each device, one called "-R" and one called "-SQ", assigned the relevant two footprints. Then, in your schematic, you can add a "2N3819-R" or a "BF245-SQ" or whatever.

Option 2:

The library has a single device called "FET". This device has many variants. One of these variants would be "-TO92-GSD", associated with the TO-92 footprint and with the connections made for GSD pin-out. Another variant, called "-TO92-DSG" would use the same footprint but with different connections. In your schematic, you add a FET-TO92-DSG and set its VALUE to "2N3819" (or whichever way round they are).

Personally, I prefer option 1 most of the time, although option 2 can feel easier for a quick-and-dirty "oh, I think I'll use this other TO-92 FET that I haven't used before".

---

Thanks a lot. The first method is more convenient. Already watched some videos about this topic and it is much clearer for me. Anyway, one thing is still confusing me - numbering pads in reference to the datasheets. I don't really understand if the part is numbered by looking from the top or the bottom? For example, this Autodesk tutorial about simple transistor https://www.youtube.com/watch?v=fOzvXkk8x_s&t=910s - look at 34:02 there are 1,2,3 numbered pins of the part BUT later he is counting in reverse - C as 1, B as 2 and E as 3... (3,2,1) - I don't understand the difference those pictures are the same POW, right? 

[skndungu75TT4N3]

Hi @jprzezdziecki 

I am glad to see you've got more assistance on the issue and that you are now doing much better, To make your life much simpler always name your pins and pads with the same name, use the info or the name command to change the names of the pins/pads, this way during association of the two(symbol and footprint) you will be sure of which orientation and which pin connects to which one. I hope this helps

[jprzezdziecki]

---

@skndungu75TT4N3 wrote:

Hi @jprzezdziecki 

I am glad to see you've got more assistance on the issue and that you are now doing much better, To make your life much simpler always name your pins and pads with the same name, use the info or the name command to change the names of the pins/pads, this way during association of the two(symbol and footprint) you will be sure of which orientation and which pin connects to which one. I hope this helps

---

Thanks, but besides that - do we look at it from above or below? I think from above.

[jprzezdziecki]

Also, the same 2N3904 in "transistor-neu-to92.lbr" has totally different pinout - I don't understand... Why the Collector is in the middle?

[skndungu75TT4N3]

Hi @jprzezdziecki 

Please note that different transistors the pin arrangements may change - however seems like you want to keep the consistency of your symbol names to that of the footprint -  this is not the case you arrange your footprint pins as per the datasheet. 

For instance, you may have name 1 for Collector on the symbol, 2 for Gate and 3 for Emitter - Now when doing the footprint be keen on the arrangement how the pin numbers follow each other is not of concern, that's why I mentioned you could name them as C, G, and E then also name C, G, and E for the footprint - you will then place you pads as per the datasheet, this is also a 3pin THT component so as long as you have the middle one done well you have least to worry about.

Supreme rule follow the datasheet

[one-of-the-robs · Accepted solution]

---

@jprzezdziecki wrote:

---

Anyway, one thing is still confusing me - numbering pads in reference to the datasheets. I don't really understand if the part is numbered by looking from the top or the bottom?

---

The Eagle footprint is always drawn from the top, as it will appear on the board viewed from the top (component) side.

Whether the datasheet labels pins from a top view or a bottom view is not 100% consistent. Usually it's top, particularly with more complex packages like ICs, but some transistor datasheets do show the "pin end" view. You need to read the datasheet carefully to see which it is.

[jprzezdziecki]

---

@one-of-the-robs wrote:

---

@jprzezdziecki wrote:

---

Anyway, one thing is still confusing me - numbering pads in reference to the datasheets. I don't really understand if the part is numbered by looking from the top or the bottom?

---

The Eagle footprint is always drawn from the top, as it will appear on the board viewed from the top (component) side.

---

Thanks for this.I thought so because it seemed logical to me. However, the example below (see attachment) is misleading for me. On one side, the pins of the symbol are numbered so that they do not correspond to the numbering of the pads. Is there a reason for this? This is the original Eagle library.

[one-of-the-robs]

That does look as if the pads are numbered backwards compared to the datasheet, but the pin mapping adjusts for that. It may be the particular variant of TO92 was drawn for a datasheet that numbered the other way, then re-used for the 2N3904.