[PCB_FORUM] Re: symbols form libraries and BRD database
- From: Phaik Kiau Tan <phaikkiau@xxxxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Thu, 16 Sep 2010 13:44:13 +0800
Hi,
I saw this kind of problem in SPB16.2.
our normal practice when CPU netlist changed, we import only netlist.
after import, the symbol will be in unplace manual, i got to grad it
and place again on brd.
The dra for the symbol change frequently due to the symbol still in
development phase, so when the dra updated, i deleted the symbol from
board and grab again from unplace manual, the symbol is not same with
the dra that updated!
After i placed the symbol and did a refreshed, then only the symbol
can be updated.
Previously i work with SPB15.7, once delete the symbol from board and
grad it again from unplace manual, the symbol will be updated
automatically.
both with same library paths.
I do think this is a problem coz allegro is not carrying the good
stuff from older version.
On Thu, Sep 16, 2010 at 1:18 AM, William Billereau
<William.Billereau@xxxxxxx> wrote:
> Gary,
>
>
>
> It is not solved but understood…
>
> In fact we are not playing. J
>
>
>
> The main goal was to get a new (good, better) definition for some symbols
> without reinventing the wheel….
>
> (setup with different path and so on..)
>
>
>
> As long as Allegro still works as we expected, no problem:
>
> Old designs use old symbols definition or new one in case of a refresh.
>
> And new designs automatically use new symbols… nothing dangerous.
>
>
>
> The trap is the clipboard copy/paste.
>
> Now we know that…
>
> So after a refresh and then a clipboard copy/paste, we only have to take
> care that a new refresh has to be done to get only one symbol definition.
>
>
>
> But as it is a “human” process, it would be better to have an automatic
> control for that.
>
> Thus the problem is almost solved, thanks.
>
>
>
> Cheers.
>
>
>
> William.
>
>
>
>
>
>
>
>
>
> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
> Sent: 15 September 2010 18:58
>
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Re: symbols form libraries and BRD database
>
>
>
> Hey William,
>
>
>
> Sounds like you’re playing some games, be careful!
>
>
>
> Also, you can really fine tune your library paths within a design: Setup ->
> User Preferences, Library under Paths.
>
> Click on the box in the Value column (e.g. for “psmpath”), then in the
> pop-up window check the “Expand” box, bottom left.
>
> This will modify the library paths only for the design you are in.
>
>
>
> So is your problem solved?
>
>
>
> 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 10:34 AM
> To: icu-pcb-forum@xxxxxxxxxxxxx
> 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.
>
>
--
Regards,
Phaik Kiau
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
Other related posts:
