I'm moving to a new library and I need to update the symbols
in DxDesigner, Is there a way to do tools -> update symbols... without causing the symbols to rotate/flip ?
Tools - Update Symbols will update symbols in-situ without affecting rotation or flip, if a symbol is flipped it will remain flipped unless you've changed the orientation in the symbol definition.
MAny thanks for the answer!
I checked both of the Libraries (old and new) and the resistor symbol is different between the libraries hence old res.1 is horizontal new res.1 is vertical.
when it comes to capacitors the symbols are the identical in terms of vertical horizontal and pin numbers but the pin names are different a,b VS b1,b2 and the end result is all capacitors are flipped 180.
do you see how it can be avoided or bypassed ?
There is no control over this using Update Symbols, you wil have to fix the rotated symbols manually after the update, changing the orientation of the basic symbol is a fairly major change.
Interesting question snaor, can you post on here if after you have updated your symbols this causes any track rip-up on your pcbs.
We have a problem with our Expedition/DxDesigner system whereby if the DxD schematic have out-of date Resistors symbols on it and we do the tools -> update symbols action then when we forward annotate to the pcb the resistors connections are swapped.
Don't know why it does this or how to prevent it happening, but it is really annoying.
In the library we have defined the resistors pins as swappable so thought that the software would take care and not swap the connections.
(attached in picture showing the library mapping of a typical resistor showing that pins 1 and 2 are swappable)
sorry but I still cannot package the design so I cant tell.
The symbol update is based on pin name and not pin number but this should not make any difference to an update. Testing with a simple test case indicates pin swaps are kept in place and traces remain on the PCB after updating a symbol that has had a pin sap in Expedition (i used a resistor defined to allow pin swaps).
As a side issue, using this discussion thread as a basis, I found the reason why the resistors where flipping in our designs.
The pdb had pin A1 mapped to 1, but the symbol had pin name A1 mapped as pin number 2.
Corrected the symbol mapping to be the same as the pdb and it now appears to work fine, no flipping of connections on forward annotations.
I learned a while back from another user that IPC-7351 has guidelines for defining parts at zero orientation (i.e. pin 1 always on left, cathode always pin 1 for a 2 pin device, etc.). Having everyone putting parts in the library follow these guidelines helps to reduce these flipping issues.
Retrieving data ...