Have you recompiled the design before running the BOM or part manager tool? (Export physical.) That'll do it every time.
Yes Ihave tried to EXPORT PHYSICAL and also expand .. everyway I have. But I couldn't manage to solve. I guess this problem might be an extreme case. I don't know why this happens.Thank you all.
OK, long shot, becasue I don't know how the replace works. Make sure the property you're trying to change is a soft property eg. $LOCATION rather than the hard property LOCATION.Two more courses of action 1/ Delete and re-add the correct part.2/ Raise an SR !!
Thanks for your answers. I have opened an SR for this event but actually they don't pay much attention to that case. And I said OK this one may be an extra case just related to me and they closed the case. Yes you are right I could delete and put a new one but there are more resistors that has the same problem. Actually in the library definition of resistor there are no other tricks or special things defined.Again thank you for your answers.Best regardsAhmet
Hi Ahmet,If you are not happy with the status of the SR with Cadence then please don't let them close it until you have some sort of resolution. In this case Cadence will almost certainly need a testcase to look at the problem - this is by far the best way for them to give you an accurate answer/solution to your problem. One last suggestion - is there an existing pcb layout for this design? I ask this because removing the OPF view may cure this - BUT this is not something that is too be done lightly. The PART_NUMBER property is stored on the schematic (schematic value) and in the OPF (Occurence Property File) which is generally used in hierarchial designs. It looks like the OPF is not being updated with the new PART_NUMBER value. If there's no hierarchy specific properties in the design and a pcb is not yet done then removing the OPF may be an option.I would try this on a archived copy of the design first to see if this resolves the problem - BUT I'll go back to my first statement here, this is something that Cadence can do for you in an SR of they have a testcase to work fromAndy
First of all thank you very much for your suggestions. Yes it worked. I have deleted all the *.opf files in the directory and recompile it and then the problem is solved. The PART_NUMBER property is changed now. We have the PCB board is drawn already but when I compile it (after deleting opfs) I don't use the UPDATE PCB option and backannotating option.
I thought this problem is gonna die with me but it solved:)
Thank you again.
With my best regards