Make dual channel FET library

Question

I am trying to make a lib for a dual channel FET the FDMA1024NZ . I looked at similar libs and saw that you make two symbols in the symbol editor and name them A and B. I did this and connected the relevant pins to the pads of the package OK. The problem I have is that when I import the symbol into a schematic it shows the symbol for both channels locked as a group whereas the lib that I used as an "template" only imports one channel's symbol at a time if that makes sense This makes is very messy to connect both channels within a schematic and is obviously not the correct way to do it. I found only one other post that was similar to this problem but unfortunately it does not help me does mainly to my lack of understanding. 
 Attachments: FDMA1024NZ.zip

autodeskguest · Accepted Answer

Am 13.02.2019 um 20:09 schrieb Peter Newman: Thank you for both your replies Markus and Joern. I will attend to the suggestions that I understand and read up on those I do not I am thinking that my biggest mistake was adding two symbols to the symbol editor rather than adding two instances of it into the device editor ? I will redo the device after reading up on "Set Addlevel to "next" (or "always", as you like)" Most of the other suggestions I understand so they will be done and if it is OK I will re-post my lib once I think I have it done correctly. -- To view any images and attachments in this post, visit: https://www.element14.com/community/message/271655 One of the "important" rules is :copy and paste, meaning copy a similar symbol, package, device into your OWN library and modify it there. Don't change the original library. Turn on the PIN layer if editing a symbol. It shows if the pin is on grid (100mil) and the electrical direction of a pin (important for ERC). For your double N-FET I would just grab the symbol out of the transistor-fet.lbr and throw it 2 times into the device editor. You just have to give different names like A and B or so. Then add (your) package and connect as you did in the device connection list. Imho the best thing to understand the add/swap- levels is to check other libraries, like 7406, 6 inverters and why they come out one behind the other and not in one piece. Or op-amps, why the power symbol must be REQUESTed, or relays for MUST and ALWAYS. It's a good idea to show your result here because then it is much easier to make/tell corrections. -- Mit freundlichen Grüßen / With best regards Joern Paschedag

autodeskguest · Answer

Hello Peter, Am 13.02.2019 um 01:54 schrieb Peter Newman: I am trying to make a lib for a dual channel FET the FDMA1024NZ . I looked at similar libs and saw that you make two symbols in the symbol editor and name them A and B. That's wrong already. Just create (or re-use) a symbol with a single MOSFET and ADD two instances of it in the device(!) editor. Then NAME them A and B or whatever you like. Set Addlevel to "next" (or "always", as you like). You might want to change Swaplevel to 1 or so. See also HELP ADD. HTH Markus

autodeskguest · Answer

Am 13.02.2019 um 01:54 schrieb Peter Newman:

I am trying to make a lib for a dual channel FET the FDMA1024NZ (https://au.element14.com/on-semiconductor/fdma1024nz/mosfet-nn-ch-20v-microfet-2x2/dp/2101471?rpsku=rel1:1813537&isexcsku=falsehttp://). I looked at similar libs and saw that you make two symbols in the symbol editor and name them A and B.

I did this and connected the relevant pins to the pads of the package OK.

The problem I have is that when I import the symbol into a schematic it shows the symbol for both channels locked as a group whereas the lib that I used as an "template" only imports one channel's symbol at a time if that makes sense

This makes is very messy to connect both channels within a schematic and is obviously not the correct way to do it. I found only one other post (/message/194012/l/re-multiple-gate-trouble-when-creating-part-in-library#194012http:)that was similar to this problem but unfortunately it does not help me does mainly to my lack of understanding.

I had to attach my lib as a txt file due to restrictions on file upload types.

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/271538

Attachments:
FDMA1024NZ.txt.zip

No wonder. Your connection points in symbol are not on grid (100x100mil

crossing)

Without that you will not get connections to other devices/nets.

If you want to built your own device then use the existing symbols and

packages of existing libs.

In transistor-fet.lbr you find a symbol for an N-Fet to copy and put it

in your own lib.

If you don't like it you can modify it THERE.

Your transistor has its connections as IO-direction which is not

correct. Should be imho pas(sive).

If directions of devices are not correct one cannot use the ERC correctly.

For double devices it's imho best to set the addlevel "next", so the

transistors come separately, better if they are on different pages.

If one has more pins/pads with the same name use "@" to separate them

(goes for symbols and packages) like drain, drain@1, drain@2... or gnd,

gnd@1, gnd@2, gnd@3...

Help pin should give you more info, or just hit the F1 key

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Pedro147 · Answer

Thank you for both your replies Markus and Joern. I will attend to the suggestions that I understand and read up on those I do not

I am thinking that my biggest mistake was adding two symbols to the symbol editor rather than adding two instances of it into the device editor ?

I will redo the device after reading up on "Set Addlevel to "next" (or "always", as you like)"

Most of the other suggestions I understand so they will be done and if it is OK I will re-post my lib once I think I have it done correctly.

EDIT - Just reading up on AddLevel and it appears that the default is Next ?

autodeskguest · Answer

Am 14.02.2019 um 12:40 schrieb Peter Newman: Thanks for sticking with me on this Joern I really appreciate all the help I have gotten on various forums. I am hoping that this version looks a bit better than my first and I hope that I followed most of Markus' and your suggestions. I copy / pasted and modified as necessary a Sparkfun Github library that I found earlier today and just made it into a single item library that I hope is OK now -- To view any images and attachments in this post, visit: https://www.element14.com/community/message/271692 Attachments: FDMA1024NZ.lbr.zip That is almost perfect The ALMOST is for a few personal things as I see them: With a tiny script you make all layers visible (use separately in board and device/symbol) Set Used_Layers ALL; DISPLAY all; display you will see a lot of layers which are not "official" and I would remove them. Usually (check other libs) the body of a package is drawn in layer t_place, while t_docu is for documentation. (Help layer). In device editor bottom right you see VALUE off / on. ON is for mass ware like resistors which will be given individual values. For Transistors one wants to know what type it is in the drawing,so set it to OFF. In OFF position the value (Name of the transistor) is printed out. At least in device editor add a description. I usually copy the important values from the datasheet in there. That is much faster to access than the datasheet itself. All this are suggestions. Try out what you like best. Don't trust datasheets in general and also not those in forums etc. because mostly they have as direction IO and so the ERC is worthless, or the physical body is not correct. So verify before use! Have fun with eagle. -- Mit freundlichen Grüßen / With best regards Joern Paschedag