Off Board Parts

Hi Dave

I assume that by 'offboard connections' you are referring to inputs such as pots/pedals etc?

If you could upload a pic of the particular part/s you are having problems with then I may be able to help.

I use Molex connectors myself to make offbaord connections to speakers,power,sensors etc. I find that they are cheap, I can solder them easily, and they are quite tough.

If I am on the right lines let me know and I will help with more detail.

Regards

David

"Without the ability to make off board connections I will have to find software that can handle them."


"I use Molex connectors myself to make offbaord connections to speakers,power,sensors etc. I find that they are cheap, I can solder them easily, and they are quite tough."

Ding ding ding!!! We have a winner!! What a brilllliant idea!(Yeah, I feel like a dolt now)
Yeah, just need to do pots, switches etc..

I've been doing this stuff by hand hand for so long when I finally got behind a computer I kind of lost my mind..

Thank You Very MUCH

Dave

Op Tue, 27 Mar 2012 19:33:23 +0200 schreef Dave Cader 

<noreply-99913@element14.com>:

"Without the ability to make off board connections I will have to find 

software that can handle them."

 

>

"I use Molex connectors myself to make offbaord connections to 

speakers,power,sensors etc. I find that they are cheap, I can solder 

them easily, and they are quite tough."

 

Ding ding ding!!! We have a winner!! What a brilllliant idea!(Yeah, I 

feel like a dolt now)

Yeah, just need to do pots, switches etc..

I've been doing this stuff by hand hand for so long when I finally got 

behind a computer I kind of lost my mind..

 

Thank You Very MUCH

Dave

 

Hello Dave,

Even with the above solution you'll probably want to put the "off-board" 

parts in the schematic for documentation / clarification purposes.

Andreas Weidner wrote a great ULP for that. With it you can take any 

component from any Eagle library and 'explode' it, meaning that the 

schematic symbol will be transformed into just lines on a documentation 

layer and the PCB package will be removed. So you can add the parts that 

are not on the board which makes reading the schematic a lot easier.

You can find the ULP from the 'downloads' section on the Cadsoft website.

Richard

On Tue, 27 Mar 2012 14:50:20 +0000, Dave Cader wrote:

Hello my name is Dave and I am new to Eagle and the forum but not PCB

design. I make pcbs for guitar effects pedals. These have several

off-board connections. I have checked the manual and tutorial to no

avail. Without the ability to make off board connections I will have to

find software that can handle them. Any ideas or suggestions would be

great..

Either use connectors as suggested, or make a library "component" that

has the right schematic symbol and gives you the right number of pads

(clearly marked in silk) on the board to which you solder your flying

wires.

If I wanted connectors I might go as far as to make a part that has a

symbol for a potentiometer or a switch, but lays an appropriate connector

on the board.

Alternately, there are library parts for single-terminal pads that you

can just drop into the schematic -- but that makes it harder to use the

schematic as a document of how the circuit functions.

In either case, you should be using the tool to make what you want, not

altering what you want to fit perceived limitations in the tool.

--

My liberal friends think I'm a conservative kook.

My conservative friends think I'm a liberal kook.

Why am I not happy that they have found common ground?

Tim Wescott, Communications, Control, Circuits & Software

http://www.wescottdesign.com

Hi Richard

Thanks. You just helped me solve a problem that has lain dormant for a while.

Just tried out the ULP you suggested with an LCD. I have often used a Molex connector for this and other devices.

The ULP works a treat and makes the schematic easier to read, as you said!

Now I am going to adopt this method so that my designs are easier to read, for myself and others...lol.

David

.. . and FWIW, if anyone is looking for Andreas Weidner's ULP mentioned by Richard Herman, it's called explode.ulp, and the current download location is: http://www.cadsoftusa.com/downloads/file/explode.ulp

After some messing around with this problem, I've come to the (tentative) conclusion that the explode.ulp method isn't very handy.  Explode transforms the visible parts of the component into a possibly large number of line and text elements on a drawing (not wiring) layer of the schematic.  This accomplishes the desired effect of hiding them from the PCB, but the large number of pieces are a pain to deal with -- moving them requires grouping, which becomes tricky if there's no easy way to drag a rectangle around them (without including nearby parts).

Instead, I'm finding it easier to maintain an "off-board" library, and then:

• copy a needed component into the off-board library
• in the library editor, edit the device's symbol(s)
  • delete the pins
  • replace the pins with wire stubs. Possibly on a different layer, so the component is visually distinct from the normal on-board component
• edit the device to delete its package(s)

The resulting library component can be dropped as usual on to a schematic, and can be moved around as usual. Its only shortcoming is that wires run to its (non) "pins" obviously don't stick. But this is to be expected, short of Eagle actually implementing a flag for "real" components to be ignored on the PCB, I think.

Any other ideas welcome!

Instead, I'm finding it easier to maintain an "off-board" library, and

then:

• copy a needed component into the off-board library

• in the library editor, edit the device's symbol(s)* delete the pins

• replace the pins with wire stubs. Possibly on a different layer, so

the component is visually distinct from the normal on-board component

 

• edit the device to delete its package(s)

 

The resulting library component can be dropped as usual on to a

schematic, and can be moved around as usual. Its only shortcoming is

that wires run to its (non) "pins" obviously don't stick. But this is to

be expected, short of Eagle actually implementing a flag for "real"

components to be ignored on the PCB, I think.

 

Any other ideas welcome!

 

--

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

http://www.element14.com/community/message/157085

 

Hi Graham,

You can leave the pins in, if you make a device that only has the

symbol. To define that as an external component simply create an

attribute name EXTERNAL and EAGLE will treat it as an off board component.

hth,

Jorge Garcia

Hi Jorge, and thanks once again for your on-point and crucially useful reply.

I don't know whether to say "Yay" or "ARRRRGGGG!". I guess this feature sneaked in for version 6.2. And though it is documented in both the manual and the in-app Help, it's a bit hard to find unless you know that it's called "External".

Quick note for others: the actual attribute name is the word EXTERNAL with underscore before and after. (Can't show that in this forum, because it's the markup for underscoring the enclosed word -- or maybe there's special additional markup to show it.)

Now, the manual blurb on this (section 8.7 "External Devices without Packages") says: "This attribute [EXTERNAL] has to be created in the library; creating the attribute in the schematic won't work!" The new library device must have only symbol(s), and no package(s).

So actually, the salient thing is to create a library Device that has no Packages; the role of the EXTERNAL "flag" is simply to permit that Device to be used on a schematic, where normally device-without-package is an error.

I guess implementing that was easier than the more user-friendly idea of changing Eagle PCB to ignore schematic Devices with EXTERNAL set on the schematic -- which would have avoided the run-around of having to proliferate new library Devices (in same library? In a new library?) just to get the off-board effect.

Regardless, this is a better-workaround than previous workarounds. Thanks for bringing it to our attention.

-- Graham