Back Annotation of references

Keith Cress schrieb:

I've searched but cannot find how to force a 'back annotation' of all the

component reference designators.

 

Once I'm done with a layout I want to 'run something' that reorders the

refs; top to bottom, left to right.

There are some "renumber" ULPs around, but they work on the schematic.

If you want the part names orderd by their board location, you'd

probably have to modify one of those.

Tilmann

On 3/12/2010 1:50 AM, Keith Cress wrote:

I've searched but cannot find how to force a 'back annotation' of all the

component reference designators.

 

Once I'm done with a layout I want to 'run something' that reorders the

refs; top to bottom, left to right.

 

How's it done?

 

Thanks.

doesn't cmd-renumber.ulp work in the board? but I thought by ref

designator he means the drawing coordinates like B3. Anyway if you just

want to change the component names like C223, then maybe this ULP will

work for you.

Hi Gary.

When you hand a board to an assembly house they are not pleased by a

completely random spattering of the part numbers.  R1 at the bottom R40 at

the top and R41 next to R1.  This increases labor time for anyone working

on the boards.

The normal schematic to PCB process results in this random placement on the

PCB.

All the other packages I've ever used had a Back Annotation Feature. (which

is not the same as what Eagle calls Back Annotation).

Typically you run the Back Annotation Feature and it asks a few questions

like; What is the horizontal stripe width? - which paces how parts are

renumbered verses their vertical physical separations.

It then scans the PCB making a table of all the part numbers of every type

of parts reference based on the selected scan pattern.  Rx, Cx, Lx, etc.,

etc.

It then re-assigns all the Reference Designators in the desired pattern,

typically like you'd read a book.  Of course it's vital that this be

reflected back to the schematic.

As far as I can tell this is such fundamental requirement of good layout,

that it must have been provided somehow or somewhere.  I'm just not seeing

it.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

kcress wrote on Fri, 12 March 2010 20:23

When you hand a board to an assembly house they are not pleased by a

completely random spattering of the part numbers.

Then you need a better assembly house or better documentation.  I renumber

the component designators for reasonable order in the schematic, and things

fall where they fall on the board.  However, I do provide a board drawing

with all the component designators on each part and a locator index that

gives both the schematic coordinate and the board coordinate of every

part.

So far no assembly house has complained about that.  In fact, one local

assembler even mentioned to me she likes my boards because of the nice

documentation I provide.  The ULPs and scripts for making the assembly

drawings and the locator index are included in my Eagle Tools release

available from http://www.embedinc.com/pic/dload.htm.  In particular,

INDEX.ULP generates the locator index, and GRID_BRD.ULP in conjunction with

GRID_TOP.SCR and GRID_BOT.SCR create the assembly drawing.  These also

assume the component designator for each part is in the tDocu layer of all

packages.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Olin Lathrop wrote:

kcress wrote on Fri, 12 March 2010 20:23

When you hand a board to an assembly house they are not pleased by a

completely random spattering of the part numbers.

 

Then you need a better assembly house or better documentation.  I renumber

the component designators for reasonable order in the schematic, and things

fall where they fall on the board.  However, I do provide a board drawing

with all the component designators on each part and a locator index that

gives both the schematic coordinate and the board coordinate of every

part.

 

So far no assembly house has complained about that.  In fact, one local

assembler even mentioned to me she likes my boards because of the nice

documentation I provide.  The ULPs and scripts for making the assembly

drawings and the locator index are included in my Eagle Tools release

available from http://www.embedinc.com/pic/dload.htm.  In particular,

INDEX.ULP generates the locator index, and GRID_BRD.ULP in conjunction with

GRID_TOP.SCR and GRID_BOT.SCR create the assembly drawing.  These also

assume the component designator for each part is in the tDocu layer of all

packages.

I'd have to agree with Keith. It is not so much assembly houses, they

have Gerber and PDF viewers with OCR and all that so they'll find R41 in

a jiffy no matter where it's hiding out. It's technicians who have to

repair boards and they often don't have such tools. A good practice

layout for a product that is field-repaired or shop-repaired at the

board level needs to have orderly designators.

But I can't speak to Eagle's available methods here as I farm out all

layouts. Back annotating my schematics by hand in Eagle is a bit of a

pain. But my layouter also often generates an Orcad schematic from mine

and there it's no problem.

--

Regards, Joerg

http://www.analogconsultants.com/

Joerg wrote on Sun, 14 March 2010 17:52

It's technicians who have to repair boards and they often don't have

such tools. A good practice layout for a product that is field-repaired

or shop-repaired at the board level needs to have orderly designators.

That can go just as well for the schematic.  Unfortunately you can't have

it both ways.  One is probably just as good or bad as the other.  I usually

order the designators in the schematic, but then provide a cross reference

list for locating every part in both the board and schematic.

Quote:

But I can't speak to Eagle's available methods here as I farm out all

layouts.

I use one of the renumber ULPs from CadSoft I grabbed a copy of long ago.

I think there are renumber ULPs for the board too.  If not, it shouldn't be

hard to modify a schematic renumber into a board renumber.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Olin Lathrop wrote:

Joerg wrote on Sun, 14 March 2010 17:52

It's technicians who have to repair boards and they often don't have

such tools. A good practice layout for a product that is field-repaired

or shop-repaired at the board level needs to have orderly designators.

 

That can go just as well for the schematic.  Unfortunately you can't have

it both ways.  One is probably just as good or bad as the other.  I usually

order the designators in the schematic, but then provide a cross reference

list for locating every part in both the board and schematic.

 

True, you can't have it both ways. But the preferred method is to have a

clean board because often the people doing the repair don't do the

diagnostics. They are simply told "Replace Q13 and U28". Folks who read

schematics are either advanced technicians or engineers and they will

have a computer with the required SW at their workplace so they can

instantly find the locations.

Quote:

But I can't speak to Eagle's available methods here as I farm out all

layouts.

 

I use one of the renumber ULPs from CadSoft I grabbed a copy of long

ago. I think there are renumber ULPs for the board too.  If not, it

shouldn't be

hard to modify a schematic renumber into a board renumber.

 

I would also think it should be possible. However, layouts are often

farmed out because that saves cost. In my case many of them are done on

PADS, others on MicroCad, and so on. Whatever a client prefers. Back

when I used Orcad one simply fed it the back-annotation file from the

layouter and ... whoopdidou ... the schematic was updated. It always

worked. I guess one could write something that would allow Eagle to also

do that. But I am not that great of a SW writer.

--

Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.

Use another domain or send PM.

I would also think it should be possible. However, layouts are often

farmed out because that saves cost. In my case many of them are done on

PADS, others on MicroCad, and so on. Whatever a client prefers. Back when

I used Orcad one simply fed it the back-annotation file from the layouter

and ... whoopdidou ... the schematic was updated. It always worked. I

guess one could write something that would allow Eagle to also do that.

But I am not that great of a SW writer.

The ULP cmd-renumber.ulp renumbers components on the PCB in a logical order,

and if the schematic is open, back annotation happens automatically.

Am I misunderstanding the original request?

Exactly so Joerg!  I don't care what the schematic refs are.  Debugging a

design is all about what the components are on the schematic then where

they are on the board.  Once you head to the part on the board you have to

find it!  With 300 components on a board it's a chore to find it and a

really big chore if the board is covered with random refs.

Greg; You are not misunderstanding in the least!  That's exactly what I'm

after!  I'll try it on my current layout when I get to that point.

Many thanks.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

On 3/14/2010 8:28 PM, Greg Erskine wrote:

I would also think it should be possible. However, layouts are often

farmed out because that saves cost. In my case many of them are done on

PADS, others on MicroCad, and so on. Whatever a client prefers. Back when

I used Orcad one simply fed it the back-annotation file from the layouter

and ... whoopdidou ... the schematic was updated. It always worked. I

guess one could write something that would allow Eagle to also do that.

But I am not that great of a SW writer.

 

The ULP cmd-renumber.ulp renumbers components on the PCB in a logical order,

and if the schematic is open, back annotation happens automatically.

 

Am I misunderstanding the original request?

 

 

yeah, isn't this what I wrote? afaik if the schematic and board are

opened together back annotation is automatic, you don't have to do

anything special, but both need to be open at the same time. so when you

run the ulp it will reassign the component names in order on the board,

and the schematic will sync to that as well.

I was just confused by your use of the term "reference designator" for

what EAGLE calls "part names". I assumed that you knew what ULP's are

for and how to use them. If you don't know, they are extensions to EAGLE

that manipulate the board. Usually the renumber ulp's ( they are several

) will ask you what scheme to use such as start number, horizontal and

vertical stripes, etc. you just run it from the board window and it

should b/a automatically as long as schematic is open.

and why are you lecturing me on the need to order the components on the

board? i never said that was a problem, i just never heard of "reference

designator" before and was wondering if it referred to the board

coordinates that are sometimes printed in the drawing frame to assist in

locating components or to the component names.

sorry to confuse you.