wiring diagram

Ryan B wrote on Tue, 31 August 2010 16:20

Has anyone been able to get Eagle to work for wiring diagrams.

Of course.  Schematic capture is one of its main functions.

Quote:

When I try and create some schematic only components (wire housings,

ferrules, etc..) I get error messages that there is no PCB footprint.

If you want to put things only on the schematic that aren't real parts on

the board, you can either draw them directly in the schematic or use a

canned symbol from a library.  Annotation text is a good example of the

former, and schematic frames for individual pages are common examples of

the latter.

Quote:

We are getting to crunch time and I need to get this moving.

As always, reading the manual saves time.  It sounds like you've already

wasted more time bumping around in the dark than it would have taken to

read the manual and do it correctly from the start.

--

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

On 8/31/2010 1:20 PM, Ryan B wrote:

Hello all,

>

Has anyone been able to get Eagle to work for wiring diagrams. When I

try and create some schematic only components (wire housings, ferrules,

etc..) I get error messages that there is no PCB footprint. OF COARSE,

this is for the wiring I plan to associated with the board I have created.

>

We are getting to crunch time and I need to get this moving. Maybe I

just need to have the SolidWorks team work on this for me.

>

Thanks

Ryan

You can draw directly into the schematic, or make library symbols that

don't have an associated package and use them as device. The problem

with either of these approaches as that you can't then rubberband the

nets with the parts because you can not include pins in the device

without the package footprint. This makes any changes somewhat tedious.

As Olin suggested, look at the drawing frames for an example of devices

without footprints. There are also some libraries on the CADsoft website

with common schematic symbols for AC power and such.

I would prefer if EAGLE would allow schematic pins without an associated

package for just the problem you have run into.

Gary Gofstein wrote on Tue, 31 August 2010 16:59

I would prefer if EAGLE would allow schematic pins without an

associated

package for just the problem you have run into.

It can.  Ground symbols are a common example of this.  A device can have a

symbol without a package.

--

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

> I get error messages that there is no PCB footprint.  OF COARSE,

this is for the wiring I plan to associated with the board I have created.

I sometimes use SET CHECK_CONNECTS OFF; might be suitable.  From the

menu select Options | Misc (tab) | Check Connects

From the help:

"The ADD command checks whether a pin has been connected to every pad

(with CONNECT). This check can be switched off. Nevertheless, no board

can be generated from a schematic if a device is found which does not

have a package."

Regards,

Neil

On 8/31/2010 2:21 PM, Olin Lathrop wrote:

Gary Gofstein wrote on Tue, 31 August 2010 16:59

>> I would prefer if EAGLE would allow schematic pins without an

>> associated package for just the problem you have run into.

>

It can. Ground symbols are a common example of this. A device can have a

symbol without a package.

>

Thank you Olin, that's very good to know. It will not work if the device

is created with pin directions "passive", although "supply" will allow

the device to not need an associated package!

On 08/31/10 23:26, Neil Allison wrote:

>> I get error messages that there is no PCB footprint.  OF COARSE,

>> this is for the wiring I plan to associated with the board I have

>> created.

 

I sometimes use SET CHECK_CONNECTS OFF; might be suitable.  From the

menu select Options | Misc (tab) | Check Connects

 

From the help:

"The ADD command checks whether a pin has been connected to every pad

(with CONNECT). This check can be switched off. Nevertheless, no board

can be generated from a schematic if a device is found which does not

have a package."

Actually this should read

  "The ADD command checks whether every pin has been connected to a pad..."

I've changed that in the online help for the next version.

Klaus Schmidinger

--

_______________________________________________________________

Klaus Schmidinger                       Phone: +49-8635-6989-10

CadSoft Computer GmbH                   Fax:   +49-8635-6989-40

Pleidolfweg 15                          Email:   kls@cadsoft.de

D-84568 Pleiskirchen, Germany           URL:     www.cadsoft.de

_______________________________________________________________

Gary Gofstein wrote on Tue, 31 August 2010 18:32

It will not work if the device is created with pin directions

"passive", although "supply" will allow

the device to not need an associated package!

I didn't realize this was limited to the supply pin direction.  That means

this method comes with certain ERC issues.

--

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

Klaus Schmidinger wrote:

>On 08/31/10 23:26, Neil Allison wrote:

>>> I get error messages that there is no PCB footprint.  OF COARSE,

>>> this is for the wiring I plan to associated with the board I have

>>> created.

would it be possible to add a new pin direction 'no_pad' or something

to the effect that symbol-only devices are possible?

--

Lorenz

On 8/31/2010 4:20 PM, Ryan B wrote:

Hello all,

>

Has anyone been able to get Eagle to work for wiring diagrams. When I

try and create some schematic only components (wire housings, ferrules,

etc..) I get error messages that there is no PCB footprint. OF COARSE,

this is for the wiring I plan to associated with the board I have created.

>

We are getting to crunch time and I need to get this moving. Maybe I

just need to have the SolidWorks team work on this for me.

>

Thanks

Ryan

Hell all,

I seem to have a way around this, I am making all the pins on the supply

direction.  While this allows for a symbol without a package to be used

it does connect all nets together; although since the drawing will not

be a PCB this is not an issue.  These cable drawings will be for ref.

only and then used to translate into manufacturing drawings in a cad

system.

For those of us here that will be trouble shooting and repair the cable

diagrams made in Eagle will serve as a pin-pin reference.

Thanks

On 9/1/2010 10:43 PM, Lorenz wrote:

Klaus Schmidinger wrote:

>

>> On 08/31/10 23:26, Neil Allison wrote:

>>>> I get error messages that there is no PCB footprint.  OF COARSE,

>>>> this is for the wiring I plan to associated with the board I have

>>>> created.

>

would it be possible to add a new pin direction 'no_pad' or something

to the effect that symbol-only devices are possible?

just reiterating my support for symbol only devices.

But I think it better to have it at the package level than at the pin

level... there may be advantages to having it at the pin level, such as

a pot mounted on a board, the 3 terminals are part of the package and

the case can be shown grounded on the schematic without incurring a

footprint pad. This could also be done in the current system with a

special footprint, since there will need to be a ground connection

somewhere. Maybe someone can think of a better reason to make it a pin

direction rather than a package level option 'off_board' ??