How to make a library availabe for the "add part" in the schematics editor?

[hhermFHT6J]

Sorry I'm still a bit lost:

• I copied an external library to my eagle documents folder.
• I find it with the library manager in the tab "in Use"
• I can open it for editing

But I don't find it in the schematic editor with the "Add part" button .... there are many available but not this special one.

So there might be one step to make it known to be available for adding in the schematics editor, which I had neglected?

[jorge_garcia]

Hi @hhermFHT6J,

I hope this message finds you well. You've done everything right. The only reason is might not show up in the Add command is if the library does not contain devices. If it's a library that only has footprints or only contains symbols then it will not show up in the add command.

Can you confirm that's the case with this library?

Let me know if there's anything else I can do for you.

Best Regards,

[hhermFHT6J]

@jorge_garcia 

Thank You for Your suggestion. I guess, You are right, that the device was missing.

But I'm stumbling into the next thing, I do not understand.

Now that I have created a library, containing device footprint and symbol, I tried to add the library contents to a schematic. Eagle's error message was that it woudn't contain a footprint, what obviously is not true.
Did I miss at some point, to somehow define a relation between device and footprint or something like that? Isn't it sufficient that both are the same library?

If I try to add the footprint to the board-file, I get the (expected) answer, that I would have to add the device to the schematics first.

[one-of-the-robs]

Your screen shot is unhelpful. What we need to see is how you've defined that DEVICE. It's not enough just to have the same name - there's no linkage by names in the library - it must have the footprint (and the symbol) explicitly associated. So show us your library with the device editor open.

[hhermFHT6J]

@one-of-the-robs  , @jorge_garcia 

How do I link device, footprint and symbol? I guess that might be the keypoint of an answer?

Here is the screenshot of the device editor

[one-of-the-robs]

Do you see on the right hand side of that screenshot, there's a section with "Package" and "Variant" headings? And at the bottom of that, there's a "Neu" button? That adds a new package option to the device, after which the "Connect" button lets you map the schematic symbol pins to the footprint pads.

This is all fairly well documented in the PDF manuals that are installed with Eagle. It's worth having a read.

[hhermFHT6J]

@one-of-the-robs 

Sorry, but I have real difficulties to understand the manual. I usually try what I understand what I read and run into dead end roads a multiple times. Usually I understand the manuals only in the retrospect - and only than it becomes obvious to me, what the manual means.

I never saw, that the creation of a package was indispensable for the library to become working at all.

I tried "New" "Create with package generator" in the bottom right corner of the device editor. But then  I got a list of suggestions like "Axial" "BGA" "Chip" "Chip Array" etc ..... but nothing looking approxmately like a daughter board and I didn't know what to do with it.

So, not knowing that the usage of a package editor is indispensable, I guessed, it was one of the dead ends of my trials.

[one-of-the-robs]

You don't want the package generator! Sorry, that's a recent thing and doesn't exist on the older version I use. What you want is the traditional "New->Add local package" (which used to be the only option) and then pick the footprint you've already created.

[hhermFHT6J]

@one-of-the-robs 

Sorry I'm still lost.

Where do I find this

---

"New->Add local package"

---

In the Control Panel, I can select

• New/project
• New/schematics
• New/board
• New/library
• New/designBlock

Nothing like package at that point. Choosing New/Library lets me Add Device/FootPrint/3DPackage/Symbol ... something, I had gone through already earlier. So it doesn't seem to be, what You mean.

In the Schematics editor I only  can choose File/New ... that only opens a new schematics, not a package

In the library manager, there is no menu start with New ... so that is not the menu You mean.

So, OK going back opening the library's device with a double click, I see at the left hand side the menu, where the only thing I could "Add" is "Add Part", but not Add local package.
Or I could go to the lower right, and select Connect, where I get told, I should first use the package command.

[one-of-the-robs]

You should be in the DEVICE editor, with your device open, and the empty package list on the right hand side. There's a "Neu" button below that, which you clicked on earlier, as I todl you before, and you reported that you had chosen "Create with package generator". That's wrong, but you should have had "Add local package" as the first option off that button. That's the one you want.

[hhermFHT6J]

@one-of-the-robs 

Ah,starting with the "Control Panel", I select   "File/New/Library"

Go to the device column, choosing "Add Device". Then I select "Import" and choose the Device from the list.

The at the lower right I select "New/AddLocalPackages" and not "Create with the package generator"

One step further ! Thank You !

To add the symbol I do not to have to complete a step like this as well?

Trying to fetch my newly created library into a schematics with "Add Part", I now get another message:
Device has unconnected Pin (G$1/1)! and nothing is added to the schematics.

OK, I learned that I have to go to the Device editor and choose Connnect in the lower right. The I get a list of Pins and Pads, I could select and highlight pairwise. I Just have to find out, what is G$1.1, G$1.2 ... and  the Pads Numbers on the other side.

So what I tried is, to select a pin in the Device editor to ask Info for the properties. But I cannot select them. I also don't see a selection filter? So, surprise, it seems I have to move to the Symbol Editor to select individual pins to check the indentity of pins.

Is there a way to make the pin names show up in the  Device Editor

[one-of-the-robs]

The intention is that, when you create your library, you label the pins on the symbol with meaningful names from the component datasheet, and don't just leave them as "P$1". Similarly, although it's unimportant for a single gate device, you should name the gate (symbol) in the device, so as not to get the "G$1" bit. Then you also would name the pads on the footprint to match the standard package allocation.

If you've done that, the CONNECT step should be a matter of following the datasheet again.

For a connector, where the symbol pins are just numbered, they would normally be numbered the same as the footprint pads, so you just connect 1 to 1, 2 to 2 and so on.

[theguru_999]

To understand it more first open the symbol and right click each pin and select properties. This shows you the name of that pin. Name them to something useful. If you have a datasheet name them using the pin names on the datasheet. Save the symbol. Now open the footprint and name the pins 1, 2, 3, 4, 5, 6 etc. as per the datasheet.
Now open the Device and select Connect. You might see a list G$1.1, G$1.2 etc. Ignore the G$1, the last number after the period is the pin/pad number. While referencing the datasheet click the pin in the left column and its associated pad in middle column and click connect. The symbol pin and footprint pin are now connected and move to the right column. Repeat until all pins/pads are connected and shown in the right column. When done click OK and the device will show with all the pin numbers and signal names showing. Make sure it is correct as per datasheet. If you don't see pin signal and pin number edit the symbol pins, right click each pin and select VISIBLE BOTH for all pins (or group all pins and use the change tool to change all pins to Visible Both at the same time). If you only want the number showing select Visible Pad. If you only want the pin signal name showing select Visible Pin. Save the library, go to the schematic editor and you should be able to add your part.

Also another common newbie error is if you made a new library or downloaded one off the net and put it in your library dir then it's probably not turned on. You need that little green dot next to ALL libraries you want to access otherwise when you use Add Part that library won't show. If the dot is grey the library is not enabled. Go to Control Panel Libraries and check it. If grey dot click it to make it green. Check the screenshot attached.....

[ge25vij]

Hi, I have the same problem and there is no device, how do I 'Add' the Device? (Do I design it or is it a file I should have)

[theguru_999]

Follow the standard procedure for making a new part.....

Open the Library

Click Add Device

Type a new name for that device or import it from another library.

If new part, go back to table of contents (book icon), create a symbol and footprint then go back to the device and add the symbol and footprint and then connect the symbol pins to the footprint pads.

Save the library and you should be able to Add your part to the schematic.

If this doesn't help you will need to provide more info or a screenshot showing your exact problem.