Can anyone direct me to a tutorial (nice, easy and direct?) for Eagle on -HOW- best to add an alternate 'package' to an existing part?
Example:
I want to use some SMD male headers for a PCB..
These will be for a Pro-Mini and a DFPlayer....
Their current footprint/packages are set up for your normal through hole male headers...
I'd like to (somehow/easily) add ANOTHER package for the part/footprint.. so that when I want to use these modules in future projects.. I can just select between the normal package.. and the one that utilizes the SMD headers.
I went into the lib that has the Pro-Mini package.. and added a NEW package: Pro-Mini-SMD
So I have my 'blank' screen up..
update:
I -can- copy from a library to another library (I was original trying to copy form my BRD file...duh)..
My problem now is.. how to get my new 'package' associated with the current Pro-Mini footprint/device?
How do I map out the pads to same -names- used in the other profiles/packages/devices?
They do take up more 'space'.. but the other side of the board is filled with 5050 package leds.. so no real space for all these through holes packages..
What I was trying to do was add an alternate package to the -already existing part in the library-....
But I'm not sure -HOW- to do that...
For the most part.. I just ended up creating a WHOLE new part..
NOT editing a current part that just has 2 optional package options.. (hope that makes sense)
Update:
I see now that each package variant needs to have its own 'variant name'.. once that was changed.. I was easily able to add a new 'package' to an existing part/footprint.
However.. I seem to have duplicate entries for my part when trying to add/replace in the schematic side of things:
How can I remove these? So there is only 1 SMD entry (and the normal/default) options in there?
see attachment *
** been a while since messing around with custom parts in Eagle! LOL
First the nomenclature so we understand each other. Under Libraries you start by right hand clicking the library, which contains the part, and select Open. This opens the library in what Eagle calls the Table of Contents. There are 4 columns - Device, Footprint, 3D Package and Symbol.
From your description I assume you have the Device and Symbol as required. You also have a new Footprint you want to associate with the Device. You can copy a Footprint from any other library to the open one. You can also duplicate (RH click and select Duplicate) one of the existing Footprints and then edit it to meet your requirements.
Now:
Right Hand click the Device you want to add the new Footprint to, and select Edit. Eagle shows the current symbol and a list along the right of the currently available Variants/Packages.
Click the New button along the bottom and select Add local package.
This will list all the available footprints with at least the number of pins required by the Device.
Select your new Footprint from the list and enter a Variant name at the bottom of the window and click OK. This will add a new entry to the list on the right. It will however have a yellow exclamation triangle at the end.
Select the new entry and click the Connect button at the bottom.
Select a Pin Name and its matching Pad Name then click Connect at the bottom. Do this for each of the Pin-Pad combinations.
Click OK and your done.
While having the Device Edit window open you can select any wrongly added or duplicate entries in the list, then simply RH click delete them.
Thats more or less what I did, but when adding a new package/footprint to the existing part/device.. I was getting an error because that both had the default "" variant names. (but the error wasnt apparent/clear to me)
I was getting an error because that both had the default "" variant names. (but the error wasnt apparent/clear to me)
Yes, if you add two new Packages/Variants without entering a variant name, Eagle shows a message saying Package variant already defined..... It does allow you to then add a Variant name for the new one (This is in Eagle version 9.5.2). Is that the error you refer to?
RH click an entry and rename, adding, or changing, a variant name to it.
Sometimes Eagle is really difficult to get used to.
This was/is for Eagle v6 (very out dated, but I never made the jump once bought out by AutoCad)..
still works and does what I need..
Yes.. I needed to rename.. but the error was not CLEAR that, that was the issue. It was a more generic error/response instead of same 'duplicate variant name'..etc..
And by Default.. the stock package variant name(s) are usually just "" (blank)..
either way it all worked out.. posted for use and/or review (in case I messed something up)..
but I'm still working on the PCB design stuff...hopefully it all works out.
xl97:
This was/is for Eagle v6 (very out dated, but I never made the jump once bought out by AutoCad)..
still works and does what I need..
OK. I only started using Eagle after the take over. In any case, they seem to have added a few more messages to help - like the popup to force you to add a variant name for the second.
Glad it all worked out.
I would like to see your board when done, please post a pic.
for Eagle on -HOW- best to add an alternate 'package' to an existing part?