Searching \ for '[EE] Question to Eagle experts' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=eagle
Search entire site for: 'Question to Eagle experts'.

Exact match. Not showing close matches.
PICList Thread
'[EE] Question to Eagle experts'
2005\04\20@103610 by Arkady Skorokhod

picon face
Hello.

I have a problem, which must be quite common. I need a part that I cannot
find in libraries I know of, or there is such a part, but the library does
not offer a package I need. So I have to create the drawings by myself
somehow. While it may be not so difficult to draw a symbol in the schematic
editor, what I'd like to avoid is creating the package I need for the board
editor manually. On the other hand I got a library called "SMD" (cannot
recall now whether it was in the original Eagle package or I picked it up
somewhere on the NET) that contains the package I need.

My question is what is the simplest way (if possible at all) to 1) create
new component from the package, or 2)"attach" this new package to existing
component. While automated creation of the package from a component symbol
is obviously impossible, the backward operation should be quite simple, at
least theoretically. Of cause, one cannot expect to get a complete symbol
with, say, names of all pins this way, but for me that would be enough. Does
Eagle have any tool for such automated component symbol creation from
existing package drawing?

2005\04\20@115159 by Rob Young

picon face
>
> My question is what is the simplest way (if possible at all) to 1) create
> new component from the package, or 2)"attach" this new package to existing
> component. While automated creation of the package from a component symbol
> is obviously impossible, the backward operation should be quite simple, at
> least theoretically. Of cause, one cannot expect to get a complete symbol
> with, say, names of all pins this way, but for me that would be enough.
> Does
> Eagle have any tool for such automated component symbol creation from
> existing package drawing?
>
> --

1) Create your schematic symbol first in your custom library.
2) From the library editor, open the "smd-ipc.lbr" or whatever library you
have determined has your special part.
3) Display the pads, etc.  make sure all the necessary layers are turned on.
4) Use the "group" and "cut" commands to put a copy onto the clipboard.
5) Close that library and re-open your custom library.
6) Create a device, you will be confronted with the blank editing screen.
7) "paste" from the clipboard.
8) Make any necessary changes and save.

Rob

2005\04\20@115309 by PicDude

flavicon
face
On Tuesday 19 April 2005 10:33 am, Arkady Skorokhod scribbled:
> ... what I'd like to avoid is creating the package I need for the board
> editor manually. On the other hand I got a library called "SMD" (cannot
> recall now whether it was in the original Eagle package or I picked it up
> somewhere on the NET) that contains the package I need.
>
> My question is what is the simplest way (if possible at all) to 1) create
> new component from the package, or 2)"attach" this new package to existing
> component. ...


If I understand you correctly...
       (a) you have a component already, but it does not offer the package variation
you need;
       (b) you have the correct package but in another library.
Do this...
(1)  Open the library with the SMD package, and open the SMD package drawing.
(2)  Highlight it all, then "cut" it (with the scissors tool).
(3)  Open the library with the correct component/symbol.
(4)  Create a new package called <whatever the package name is>.
(5)  Paste the package drawing.
(6)  Save it.
(7)  Open the component device, then add the new package variation and connect
the pins accordingly.

Cheers,
-Neil.



2005\04\20@121111 by Anthony Van Herrewege

picon face
Hi,

It's quite simple and making your own symbol for the part only takes 5 minutes extra.
Here's a tutorial, once you get the hang of it it's really fast and simple: http://www.brobertson.com/eagle-pcb-tutorial

Btw, if you create your own library with parts, you can copy the package you want to your own library. Open up the library with the package in it. Group everything and click the copy button, then click right mouse to copy the complete package. Next open up your own library, click the package button, create a new package and paste the package you just copied with the paste button.

It seems all complicated at first, but really, it's easy.

Anthony


Website: http://members.lycos.nl/anthonyvh

               
---------------------------------
Do you Yahoo!?
Yahoo! Small Business - Try our new resources site!

2005\04\20@124102 by Hulatt, Jon

picon face
Another way of doing it, which in this instance is NOT the easiest way,
but it a useful trick, is to script a whole library. you can easily
navigate the outputted script in a text editor, then past the bits you
want into  the command window.

this is for example a great way of duplicating a lot of packages or
similar.

jon

> {Original Message removed}

2005\04\20@130011 by olin_piclist

face picon face
PicDude wrote:
> (1)  Open the library with the SMD package, and open the SMD package
> drawing. (2)  Highlight it all, then "cut" it (with the scissors tool).
> (3)  Open the library with the correct component/symbol.
> (4)  Create a new package called <whatever the package name is>.
> (5)  Paste the package drawing.

Or just use the COPY command.

*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

2005\04\20@235210 by Vitaliy

flavicon
face
From: "Arkady Skorokhod" <spam_OUTark1TakeThisOuTspammyrealbox.com>
>> My question is what is the simplest way (if possible at all) to 1) create
>> new component from the package, or 2)"attach" this new package to
>> existing
>> component. While automated creation of the package from a component
>> symbol
[snip]

I just want to mention something that can help you avoid frustration later
on.  Whenever you want to modify a component, make sure you copy it into
your own custom library.  Modifying standard Eagle libraries is a bad idea -
there is no easy way to migrate modified components to the new version of a
standard library.  When you upgrade Eagle, your old libraries will be
overwritten.

Vitaliy

2005\04\21@015528 by Arkady Skorokhod

picon face
Many thanks to all replied to my question. I have already created few new
devices I needed. It was realy not so complicated as I expected.

Arkady

2005\04\21@071051 by vasile surducan

picon face
On 4/21/05, Vitaliy <.....vitaliyKILLspamspam@spam@maksimov.org> wrote:
> From: "Arkady Skorokhod" <ark1spamKILLspammyrealbox.com>
> >> My question is what is the simplest way (if possible at all) to 1) create
> >> new component from the package, or 2)"attach" this new package to
> >> existing
> >> component. While automated creation of the package from a component
> >> symbol
> [snip]
>
> I just want to mention something that can help you avoid frustration later
> on.  Whenever you want to modify a component, make sure you copy it into
> your own custom library.  Modifying standard Eagle libraries is a bad idea -
> there is no easy way to migrate modified components to the new version of a
> standard library.  When you upgrade Eagle, your old libraries will be
> overwritten.

I'm really wondering who is using any Eagle library like was
originaly created? I've guess nobody. There are so many problems in
the Eagle's library starting for example with silkscreen which is
superimposed on the smd pads on the component layer and going further
to custom drill diameters, or wrong pads diameters etc on every
through holes component library.

best reagrds,
Vasile

2005\04\21@075759 by olin_piclist

face picon face
> I'm really wondering who is using any Eagle library like was
> originaly created? I've guess nobody. There are so many problems in
> the Eagle's library starting for example with silkscreen which is
> superimposed on the smd pads on the component layer and going further
> to custom drill diameters, or wrong pads diameters etc on every
> through holes component library.

I've learned to just ignore the Eagle libraries.  Like you said, they have
too many annoying and downright stupid things in them.  The few times I've
used them I've regretted it in every case.  The last time was probably 4
years ago.

Instead of using the Eagle libraries, I have built up a large set of
libraries of my own.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

2005\04\21@083533 by Josh Koffman

face picon face
Out of curiousity Olin, when you make a part that requires power, say
a PIC or a logic chip, do you put the power pins on the schematic
symbol, or do you have them as seperate pins you need to invoke? My
stuff is usually fairly simple, so I like to keep them on the part.
Otherwise I occasionally forget to invoke and connect them.

Josh
--
A common mistake that people make when trying to design something
completely foolproof is to underestimate the ingenuity of complete
fools.
       -Douglas Adams

On 4/21/05, Olin Lathrop <.....olin_piclistKILLspamspam.....embedinc.com> wrote:
> Instead of using the Eagle libraries, I have built up a large set of
> libraries of my own.

2005\04\21@091731 by olin_piclist

face picon face
Josh Koffman wrote:
> Out of curiousity Olin, when you make a part that requires power, say
> a PIC or a logic chip, do you put the power pins on the schematic
> symbol, or do you have them as seperate pins you need to invoke? My
> stuff is usually fairly simple, so I like to keep them on the part.
> Otherwise I occasionally forget to invoke and connect them.

It depends on the part.  On PICs I include the power and ground pin, because
these are often an important consideration in the design.  I like to put the
power pins on top and the ground pins on the bottom.

For jellybean logic parts and especially parts that have multiple "gates"
(using the Eagle term) in a package, I make a separate "gate" for the power
and ground connections.  This applies to things like 74x04 inverters or
LM324 opamps, for example.

Eagle can help you to remember to connect these power gates.  When you
create a gate in a device, you can specify one about a half dozen
attributes.  I don't remember them all off the top of my head, but there are
choices like, NEXT, REQUEST, ALWAYS, and a few more.  Some of these are
specifically intended for power gates that must always be there if any other
gate is used.  If you give the power pins the PWR attribute, then you will
get ERC errors if they are unconnected.  I've never had a case where there
was a problem due to accidentally leaving power pins unconnected.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

More... (looser matching)
- Last day of these posts
- In 2005 , 2006 only
- Today
- New search...