[PCB_FORUM] Re: symbols form libraries and BRD database
- From: Michael Catrambone <mcatramb@xxxxxxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Thu, 16 Sep 2010 23:11:43 +0000 (UTC)
William,
I think I am following what you are saying. I don't think this has anything to
do with the library paths or the symbols in your library. Basically, when you
use clipboard copy from one design it grabs the symbol as it is defined in that
design not the library. Now if you clipboard paste it into another design the
symbols will be based from the old design and not the external / embedded
libraries because the symbol structure is contained in the clipboard file.
This means that the name of the placed symbols will be the same but one will
have exploded but linked symbol elements while the other will be based on the
embedded libraries in the .brd. Hopefully that makes sense. Lot of words but
I hope you get the idea. I can see if your library changed from having the
symbol origin based on Pin 1 and they changed to Body Center it would look very
wrong. Using Display > Element on the symbol that came in from the Clipboard
Paste will indicate "The following pins(s) have been edited:" which tells that
they have been exploded from the symbol and no longer match the embedded
libraries.
One suggestion to quickly get the design back to normal is to do the following:
1) Clipboard paste the reused circuit
2) Export a placement file using File > Export > Placement and be sure to
select the Placement Origin "Body Center"
3) Delete the symbols that came in from the Clipboard.
4) Place the symbols that you deleted in the previous step using File > Import
> Placement and be sure to select the Placement Origin "Body Center" again.
These steps will place the component based on the Body Center and the symbols
will be then driven by the embedded library in the .brd if they already exist.
You will not need use Refresh Symbols unless you want to update your design
with the external libraries on disk.
Hope this helps,
Mike Catrambone
Hope this helps,
Mike Catrambone
----- Original Message -----
From: "William Billereau" <William.Billereau@xxxxxxx>
To: icu-pcb-forum@xxxxxxxxxxxxx
Sent: Wednesday, September 15, 2010 11:33:39 AM
Subject: [PCB_FORUM] Re: symbols form libraries and BRD database
Hi Gary.
Thanks for your reply.
Before making the test you suggest, I just checked that placing a new part uses
the new definition in 16.3.
In fact, no, fortunately.
If I have a c0805 placed and I place a new one, the symbol is the same.
The problem is somewhere else:
I think that I first made a “refresh symbols”, then the definition was the new
one.
After that, I used a clipboard copy/paste for similar blocks from an old board
which was using an old definition of the C0805.
As the symbol definition is written in the clipboard the “pasted” components
also have the old definition.
So this behavior can also happen with any release of Cadence..
Very dangerous….
William.
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: 15 September 2010 17:37
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: symbols form libraries and BRD database
Hey William,
I didn’t see any replies, so I’ll through something out.
I have no idea if this will work, but you could try it: Before you Import
Logic, you could temporarily “break” the path to your libraries (e.g. rename
the library directories, edit your env file etc.). If the libraries can’t be
found, it can’t grab the latest versions of your symbols.
Regards,
Gary MacIndoe
Senior PCB Layout Designer
Contract - Kelly Services
Covidien
EbD R&D
5920 Longbow Drive
Boulder, CO 80301
303.476.7458
www.covidien.com
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of William Billereau
Sent: Wednesday, September 15, 2010 3:03 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] symbols form libraries and BRD database
Hello All.
We have a problem that seems to be appeared in the 16.3 (to be confirmed).
If you start a BRD from another containing some symbols definition, before this
release 16.3, if you added a new component using this symbol definition Allegro
took the definition embedded in the BRD.
If the symbol has been modified on the disk, you had to make a “refresh symbol”
to get the new symbol definition in the BRD file, even for recent placed
components.
Now, if you place a component, it seems that Allegro reads the definition of
the symbol on the disk without using the embedded one.
This means that you got in the BRD old symbol definition for components already
placed in the BRD and new symbol definition for newly placed component.
Then, it is not really a problem within Allegro.
We modified a lot of component applying IPC and LPWizard rules.
One of this rule is the symbol origin.
For a 0805 resistor, in the past, our symbol had the origin on pin one.
Now the origin is the body center of the resistor.
If you apply a refresh symbol, you have to move all previously placed
resistors, nothing critical, just a little bit annoying.
But the main problem is for assembly.
ODB++ output or Fabmaster output contains 2 different kind of 0805 that are
finally the same!
It results in a displacement from the copper for some of them depending on
which definition is taken first:
If the first definition is the body center, then all resistors defined with
origin on pin on have an offset of the half on the right or left, according to
their rotation.
And vice-versa.
Is there a way (User Preferences?) to force Allegro to keep the embedded symbol
definition for all new placed components?
If not, we will have to implement an automatic refresh for all new BRD….
Thanks in advance.
William.
Other related posts:
