How do I create a library with a device from a schematic and a board

David Waring wrote:

 

I want to add a device to my project. It is a BMP180 barometer board from Adafruit. I have the .sch and .brd from the vendor. The board is complete and wired, but when I use the ULP script to export the library I get a library that has no device which represents the board itself, just the components. So there is no connection between the library that was created and the original board. There is no way for me to use this library to add the board to my project. Am I missing something here? What is the point of exporting the library if all you get is the individual parts and the the layout?

 

I am using Eagle 7.7.0

The library export is simply to allow parts used within a board to be exported so they can be used elsewhere or updated within the design if all you have is the .sch and .brd. Otherwise it would be difficult to take an existing design and update it without having to recreate components from scratch if you don't have access to the original libraries.

If you want to create a device which adds the appropriate footprints to allow you to incorporate the Adafruit board into another design then you have to create the library part for that yourself. Creating your own library parts is a fairly simple task and there are loads of good tutorials on how to do it (Adafruit have quite a good tutorial) and there is the EAGLE help too.

Best Regards,

Rachael

It seems strange to me that this is true. I can understand how exporting a schematic will allow the things on it to be reused, but if a schematic and a board have been created, then the board itself is obviously a device that could be used in some other board. For example Adafruit goes to the trouble of providing a schematic and board for their barometer, but this can't be used by someone who is trying to put that barometer onto a printed circuit, when that seems like the only reason someone who purchased that barometer would have for the Eagle files. It seems like all the information is there so why not create a device for the board when exporting the library. Again, am I missing something?

David Waring wrote on Tue, 15 November 2016 13:35

It seems strange to me that this is true. I can understand how

exporting a schematic will allow the things on it to be reused, but if a

schematic and a board have been created, then the board itself is

obviously a device that could be used in some other board. For example

Adafruit goes to the trouble of providing a schematic and board for their

barometer, but this can't be used by someone who is trying to put that

barometer onto a printed circuit, when that seems like the only reason

someone who purchased that barometer would have for the Eagle files. It

seems like all the information is there so why not create a device for

the board when exporting the library. Again, am I missing something?

Hi

Obviously you are missing something and that is to clearly describe what

you wish to achieve.

Reading between the lines I guess you are attempting one of the following.

(1) You wish to take a barometer board and plug it into a socket on the

board you are designing.

(2) You wish to copy the layout of the Adafruit design onto your board and

surround it with your additions.

Let us know which of the above is your case and someone will be able to

describe how you should proceed.

The Eagle files are provided in the 'open' world so you have the

information about the design, no more.  With them you could build a board

yourself from scratch, rather than buy the finished product from the

source. Beyond that you can do whatever you want with them. There is no

promise that you will be able to do what you think you should be able to do

with them. You are limited by the way Eagle, or any other software,

functions.

HTH

Warren

--

http://www.eaglecentral.ca :: The original and best browser access to CadSoft EAGLE support forums.  Supported by EAGLE licenses purchased through us :: http://www.eaglelicenses.com

David Waring wrote:

 

It seems strange to me that this is true.

And yet it is, as evidenced by what you actually obtained by exporting the library....

David Waring wrote:

 

I can understand how exporting a schematic will allow the things on it to be reused, but if a schematic and a board have been created, then the board itself is obviously a device that could be used in some other board.

And like any other device, you can create a library part for it yourself from the information which is available. In this case it's simple to open the board, work out where the holes and connectors are, and the board dimensions and then go create that as a library part. I dare say I could have done that in a fraction of the time it took for you to write your original post.

David Waring wrote:

 

For example Adafruit goes to the trouble of providing a schematic and board for their barometer, but this can't be used by someone who is trying to put that barometer onto a printed circuit, when that seems like the only reason someone who purchased that barometer would have for the Eagle files.

As an example, someone could purchase a barometer from Adafruit and use it on a prototyping board hooked up to an Arduino to prototype an idea and then incorporate that design directly into a new PCB they were creating themselves in EAGLE by importing the .sch and .brd files into their own design.

David Waring wrote:

 

It seems like all the information is there so why not create a device for the board when exporting the library.

It probably would be possible to write a ULP to create a library part from a board file but it wouldn't be fully automatic as EAGLE wouldn't necessarily be able to work out which parts on the supplied .brd would be external interfaces on the new "device" and it wouldn't know how to create the matching symbol in a usable way necessarily. It could certainly be assisted by a ULP that helped extract information but I don't think it could create a completely usable library part without user intervention. In most cases I suspect it'd just be quicker to create the library part yourself anyway.

David Waring wrote:

 

Again, am I missing something?

Yes. See above.

Best Regards,

Rachael

Warren thanks for your concern but if you could not understand what I was trying to do it is solely because you did not read properly, as evidenced by the first response to my question which clearly understood. Obviously option 1 is what I described. I don't expect software to do just what I think it should do. But I do expect that if there was something that was 99% but just didn't quite do it and it seemed obvious I could try to find out why it didn't go 100% of the way and that is why I asked if there was something that I was missing that made this last step impossible.

... as EAGLE wouldn't necessarily be able to work out which parts on the supplied .brd would be external interfaces on the new "device" and it wouldn't know how to create the matching symbol in a usable way necessarily.

That is the part that I was missing. Thank you.

Try "hierarchical_v1.1.zip" in ULP download area. it transforms a couple schematic/board to a normal device in library, which you can connect to it also.

HTH

Thanks this looks like what I need.

On 19/11/2016 8:25 a.m., David Waring wrote:

Thanks this looks like what I need.

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/209799

 

Hi David

I think what you need is the supplied ULP

make-group2pac.ulp

From the baro board, clear the group.

Then start a new group.

Group only J2 and the top two mounting holes.(Hold down the CTL key and

click on those objects)

The board outline on layer 20 is always included so don't bother

selecting that.

Then run the ulp

The script of the commands that will run is displayed

Accept it.

In the new library you will have new package that has 7 pads for the J2

header and two for the mounting holes (ie the screws and spacers to hold

the baro board to your new mother board.

The outline of the board has only 0 width and its still on the dimension

layer so you need to increase that to the width of you silk screen print

and move it to the tPlace layer so that outline prints on your mother

board (if you want it). Tidy up the package as you see fit. Create a

symbol with the 7 pins and  and perform the 'connect' to mate it to the

package.

HTH

Warren

Wow - thanks for that info Warren.  I had been giving the same issue some

thought and was going to suggest this morning that the solution would be to

bring the board (.brd) file into the editor, remove all the components,

traces, vias etc. then group/copy the remainder and insert it into the

package editor.  Both Sparkfun and Adafruit have some neat gadgets that

would be really nice to be able to stick them on a board just like other

components and I had searched before for information on how to create a

package from a board (in my case, I wanted to create a device for the

Huzzah board).  Creating the symbol is no big deal, but getting the

mounting holes, pins etc. was the question.  Your answer sounds like it

solves that problem.

mikey

--

http://www.eaglecentral.ca :: The original and best browser access to CadSoft EAGLE support forums.  Supported by EAGLE licenses purchased through us :: http://www.eaglelicenses.com