Hey Bill, I agree with you. I believe what he is seeing is the result of creating a clipboard from a database which used an older version of the library then importing it into a new database which has has used a newer version of the library. The resulting symbols that come in thru the clipboard file will be skeleton symbols with exploded pins built based off the clipboard file that may not match the symbols currently placed in the design even if they have the same name. This is the only way I have ever seen what is described. Mike ----- Original Message ----- From: "Bill Zembek" <billz@xxxxxxxxxxx> To: icu-pcb-forum@xxxxxxxxxxxxx Sent: Friday, September 17, 2010 1:15:04 PM Subject: [PCB_FORUM] Re: symbols form libraries and BRD database Hi, I have been reading the responses and took the time to do some testing. I can not confirm the behavior you have described. I took a board and placed an IC. Saved the board and copied the footprint to a new directory (my working directory) and replaced the padstack and saved it with the same name. I then read in a new netlist and placed another part with the same footprint name as the one placed. The part placed was the one copy in the brd database and not the new one. This is the behavior I have always seen. If you can provide a test case demonstrating this behavior you should submit it to Cadence. Regards, Bill Zembek Technical Support – Allegro Specialist EMA Design Automation, Inc. 225 Tech Park Drive Rochester , New York 14623 Phone 585-334-6001 Opt 5 Fax 585-334-6693 www.ema-eda.com www.timingdesigner.com Cadence ® OrCAD ® Capture CIS with Digi-Key ® Integration View a live demo • Register Now! From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of William Billereau Sent: Wednesday, September 15, 2010 5:03 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.