2 schematics 1 board?

Greetings John Suhr,

  on Mon, 28 Jan 2008 you wrote saying :

Is there a way to do this?

I have two different schematics but I want to use 1 universal board

Most of the parts are empty or values changed.

I cant think of a clean way to do it

Normal practice is to design the schematic as the super-set, but set the

values of many of the components as "do not fit" or similar. You end up

with a schematic which, at first sight, makes no sense - and often fails

ERC because there are multiple output pins on a single net. However,

it's a common enough technique and board populating houses are generally

quite happy to handle parts lists with unfitted parts.

What it doesn't do well is really different boards, or simple selection

of which variant you're building. Your description suggests maybe the

two circuits you want to build are quite different, so the usual trick

may not suit, but it does work well for variants such as normally

fitting an  RS-232RS-232 interface but having the option of RS-422 instead

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of this | Windows NT crashed.

message are purely   | I am the Blue Screen of Death.

my opinion. Don't    | No one hears your screams.

believe a word.      |

"Robert Pearce" <news@bdt-home.demon.co.uk> wrote in message

news:uaJF47KzilnHFwKn@daniel.huneausware.local...

Greetings John Suhr,

 

on Mon, 28 Jan 2008 you wrote saying :

Is there a way to do this?

I have two different schematics but I want to use 1 universal board

Most of the parts are empty or values changed.

I cant think of a clean way to do it

 

Normal practice is to design the schematic as the super-set, but set the

values of many of the components as "do not fit" or similar. You end up

with a schematic which, at first sight, makes no sense - and often fails

ERC because there are multiple output pins on a single net. However, it's

a common enough technique and board populating houses are generally quite

happy to handle parts lists with unfitted parts.

 

What it doesn't do well is really different boards, or simple selection of

which variant you're building. Your description suggests maybe the two

circuits you want to build are quite different, so the usual trick may not

suit, but it does work well for variants such as normally fitting an

RS-232RS-232interface but having the option of RS-422 instead

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

 

Well we populate the board so that isnt an issue

But in order to have connectivity of the schematics with the board and one

of the schematics the board and schematic need the same name as I

understand.

So I could keep changing the name but this is a pain.

Also to show part VALUE on the board for assembly I can think of no other

way except for instance X-470K where first value is product 1 and second

value is product 2 then I need to highlight the second value with a marker

to make sure my gals stuff the right part.

The way I used to do it the board and schematic were not linked so I could

just generate a report from each schematic I was also able to change the

text color which is helpful

Thanks

JS

John Suhr wrote:

...

The way I used to do it the board and schematic were not linked so I could

just generate a report from each schematic I was also able to change the

text color which is helpful

 

Thanks

JS

 

 

You can still do this in the current version of EAGLE.  We do.

When you have a completed board/schematic that contains all parts that

are used in all products, create copies of the schematic only for each

of the unique products.  You'll then have to go through each of the

schematics and manually update part values and place a "Not Used", N/A,

or whatever you want in the value for all parts not used.  We don't keep

a board file for these "schematic only drawings" since they don't match

the physical board.  The "real" schematic for the board never gets

published as a drawing, only the "schematic only drawings".

Instructions for putting parts on the PCB are created as a separate

drawing in OpenOffice.org.  They contain tables as follows

A seperate table is created for SMD and through-hole parts.  Then a

component map picture is included to aid in locating parts.  Special

notes concerning assembly (IPC standards, conformal coating, etc.) are

also on this drawing.  If you need x-y coordinates for each component

there are several ulp files available from EAGLE that do a great job.

I've probably said way too much, but that's how we solve the issue.

That said, version 5 of EAGLE will have attributes for parts that you

can specify.  You will be able to create an attribute containing part

value, your company part number, or whatever else for each part.  Then

based on these custom attributes you could create a parts list report

for each product.  I haven't tried this with the beta version yet, but

if I understand the feature correctly, it should work.

   Tom Sneddon