Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Internal Connections Eagle Library Part

Status
Not open for further replies.

whybjorn

Newbie level 4
Joined
Nov 16, 2010
Messages
6
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,327
I have a DC/DC Converter that has two ground pins that are internally connected. I would like to make this internal connection when I create the part in the eagle library, so that there are no air wires between the two ground pins when it is on the board in eagle. Is there a way to make this connection in the library file?
 

I have a DC/DC Converter that has two ground pins that are internally connected. I would like to make this internal connection when I create the part in the eagle library, so that there are no air wires between the two ground pins when it is on the board in eagle. Is there a way to make this connection in the library file?

In the library, you name the first pin GND, and the second one GND@1 third GND@2 etc.
@1, @2, @3 characters will be invisible, and pins will be connected by default in board with airwires.
 

That won't actually create the connections - you will still end up with airwires you need to route. Even if you draw a track in the footprint between the two pins it will not connect when you get it on a board - you will have to draw a track again. You cannot put a polygon assigned to a net on the footprint. If you put a polygon on the footprint it will still say they are unconnected on the layout (and report overlap errors).

It is a bit of a limitation of the way the software is written. It means you have to device how handle it. Draw the connection later in the layout or add it in the footprint and then accept the errors and re-draw the net to remove the ratsnest.

Keith.
 

That won't actually create the connections - you will still end up with airwires you need to route.
It is a bit of a limitation of the way the software is written.
Keith.
Routing that connection should be made when routing the board, like any other electrical signal in the circuit. So it's not a limitation, it's how it should be.
 

Some parts have defined ground areas of the footprint which also need to be connected. It would be logical for these to be made part of the footprint. The software doesn't allow you to do that. Cadsoft are aware of the limitation, if you look at the Cadsoft forums.

Keith.
 

Some parts have defined ground areas of the footprint which also need to be connected. It would be logical for these to be made part of the footprint. The software doesn't allow you to do that. Cadsoft are aware of the limitation, if you look at the Cadsoft forums.

Keith.

The ground areas can be made with rectangles on the routing layer (top or bottom). The DRC "errors" that appear in this case can be "approved"....
But any signal between two electrical pins should be made when routing the board, not when creating the library.
And I'm aware of the Cadsoft's forums.
 

It is a matter of opinion. I don't see any logical reason why a footprint should not contain essential connections which is what the original poster wanted. The feature in version 5 of Eagle to "approve" DRC errors seems to be half a solution to the problem which presumably is difficult for them to solve. This also manifests itself where you need to create a footprint with a pad that cannot be created with with a single SMD. Some of the Coilcraft inductors/transformers are an example. With a single component you can end up with dozens of errors which need approving and after routing you get a few dozen more. It is a problem I would really like them to fix (along with a lot of other people).

Don't get me wrong, I like Eagle and have used it for many years but sometimes its limitations are frustrating and need work-rounds which is not ideal.

Keith.
 

It is a matter of opinion.
Agree
I don't see any logical reason why a footprint should not contain essential connections which is what the original poster wanted.
well... footprint is one thing, routed component is an other thing. I like to keep things separately.
The feature in version 5 of Eagle to "approve" DRC errors seems to be half a solution to the problem which presumably is difficult for them to solve.
maybe Eagle 6 will found a solution to satisfy everyone. But discussions should be made on the official forums to be listened ;)
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top