Цитата(B-52 @ Dec 25 2013, 16:43)
Всем привет!
Есть готовая плата в 7.9.4.
Открываю плату, нажимаю "Сохранить", закрываю.
При очередном запуске на 13% рассказывает следующее:
Error: Unable to find padstack 'via040018' for via range 1 to 8.Error: Unable to load design (E:\PROJECT\TEST\PCB\Work\Layout_Temp\LayoutDB.lyt). Padstack missing from Padstack partition. No padstack called "via040018" defined for via layer range 1 - 8
После этого плату открыть не получается.
Был такой проект от пользователя. Проблема была в том что слили схемный проект с pcb из другого проекта (результат в правилах в схеме 2 слоя в плате 4) - типичная российская проблема, схему и топологию делают два разных человека удаленно друг от друга и не делают передачу данных как положено. Вот цитата менторовского инженера
Цитата
I think we need to try and find out a little more about the history of this design. The problems we’re getting with the padstack messages are typical of cases where the Customer tries to ‘glue’ or ‘marry’ a front-end from one project and a PCB from a different project together, and sync them up as one design; you absolutely cannot do this! Again, please review TechNote mg48468 and ESPECIALLY AppNote MG581492 for more details on supported ways of achieving this result.
Решения было два:
его
Цитата
At this point, you will need to make a copy (in the Job Management Wizard) of the project without the PCB part of the design (create a new project, and add the .sbk files from the old project; else you could manually delete the PCB directory and the pointers to the .pcb file and Layout Template in the .prj file (not officially supported, do at own risk!), and then ‘recover’ the layout using Circuit Move & Copy via the Layout Clipboard or via a Layout Template, i.e. similar techniques to those described in TechNote mg48468 and AppNote MG581492. You would have to use the above ‘trick’ of disassociating the project from the PCB in order to open the original layout in order to use the Circuit Move & Copy technique – however, you should be able to make a Layout Template in the Central Library without having to do that (so, that is the best option for your Customer); then, using your ‘new’ project which does not yet have a PCB associated with it, you just point to the Layout Template you created from the original layout, when you create your new PCB design. This also has the advantage of setting up your stackup, via definitions, plane definitions etc. etc., whereas if you use the CMC technique you would need to set all that up manually in the new layout.
мое
- открыл проект в 2005
- отключил CES
- привел проект в нормальное состояние - чтобы везде (схеме-топологии) было одинаковое кол-во слоев
- затем все заработало и в 7.9.5
HELP c Expedition 7.9.4!, Открываю > Сохраняю > НЕ открывается!!!
Dec 25 2013, 12:43
