Is there anyway to exclude parts from the PCB

it cannot become this still with the eagle
do not wait for marvels from eagle

read here
http://www.element14.com/community/message/118034/l/re-beta-version-6911-available#118034

On 3/26/2015 4:38 AM, Derek Tombrello wrote:

In Eagle Cad, is there anyway to exclude components on the schematic

from the board view? I have several parts that will be wired to screw

terminals. They still need to be shown in the schematic, but I do not

need or want them on the board. I can't leave them outside the board

area, so what's a guy to do? Thanks...

 

--

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

http://www.element14.com/community/message/145238

 

Hi Derek,

I hope you're doing well. This is possible. In the library for those

components create an attribute with the name EXTERNAL. This tells

EAGLE that this part is off board and therefore doesn't require a

package on the board layout.

In order for this to work the device can not have a package. So you may

need to create a variant of those parts without packages.

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

Best Regards,

Jorge Garcia

I know this is an Eagle forum, but is there any program (Linux) that CAN do this? Thanks for the reply.

I will bet that there is a file like XML which can be problematically changed if the layout is well known. But why would you want to do this? A simpler way would be labelling them optional. Or create separate views one with and one without. Just think "outside the box".

Clem

"Outside the box"... if you were to see the circuit I am trying to build, you'd probably tell me to get back into the box! lol... I don't understand "label them optional" but I do have two schematics - one with and one without the components - but the problem with that is that if I make a modification to the circuit, I have to remember to update TWO schematics instead of just one. And my memory is NOT that great!

Why would I want to? My current circuit has an off-board IR receiver-transmitter pair. Obviously, they are important to the circuit, so that have to be shown on the schematic, but since they are off-board, they do not need to be placed on the PCB view. It's like if you are designing an (admittedly old-school) amplifier. The volume control is panel mounted, so you don't need or want to have a footprint or pads for that on the PCB board, but it still needs to be in the schematic. Does that make sense?

Derek Tombrello wrote on Thu, 26 March 2015 22:14

I don't understand "label them optional" but I do have two schematics -

one with and one without the components - but the problem with that is

that if I make a modification to the circuit, I have to remember to

update TWO schematics instead of just one. And my memory is NOT that

great!

That is a case where I think the work flow of gEDA or Kicad is superior to

EAGLE.  With either of those, it is a one-way trip, whereas EAGLE is

two-way.  What I mean by that is that with gEDA and Kicad, you make a

schematic with symbols, then you process that schematic to add the packages

for the board, and then you do the layout.  If you want a different board

(e.g. surface mount instead of through hole), you process the schematic

again and make a separate layout.  If you make any changes to the

schematic, you have to remember to go through the process again to

propagate changes to the board, but at least you have only one schematic to

maintain.

EAGLE is a two-way process; they call it forward-backward annotation.  That

ties the board back to the schematic, so that you can make certain changes

in the board and the schematic gets updated.  I think this is a much better

way of working on designs that have one schematic and one board, but it's

not ideal for single schematics with multiple board layouts...

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 27/03/15 06:16, Doug Wellington wrote:

EAGLE is a two-way process; they call it forward-backward annotation.  That

ties the board back to the schematic, so that you can make certain changes

in the board and the schematic gets updated.  I think this is a much better

way of working on designs that have one schematic and one board, but it's

not ideal for single schematics with multiple board layouts...

It may not be ideal for that case, but that's a case where nothing's

ideal. Frankly, I find the KiCad / gEDA method utterly unusable.

Anyway, this whole sub-thread was fired off by a troll who wasn't

up-to-date with the latest Eagle, as Jorge pointed out in his reply.

Derek's actual requirement can be supported that way.

I see many designs in different groups making them easier to analyse. But I see the problem with two managing updates. Yikes.

Jorge Garcia wrote:

On 3/26/2015 4:38 AM, Derek Tombrello wrote:

In Eagle Cad, is there anyway to exclude components on the schematic

from the board view? I have several parts that will be wired to screw

terminals. They still need to be shown in the schematic, but I do not

need or want them on the board. I can't leave them outside the board

area, so what's a guy to do? Thanks...

 

Hi Derek,

I hope you're doing well. This is possible. In the library for those

components create an attribute with the name EXTERNAL. This tells

EAGLE that this part is off board and therefore doesn't require a

package on the board layout.

 

In order for this to work the device can not have a package. So you may

need to create a variant of those parts without packages.

To do this I open the respective library and then in the control

center right-click on the device-set I want to create the package-less

variant off and copy to library.

Eagle asks for a different name (because the device-set already

existst); I append -NP (no package) to the original name.

Now I open the new device-set, remove all packages and add the

EXTERNAL property.

Save the library and update the schematic.

--

Lorenz