Set unique names on copy in advanced settings.
Sent from my HTC
to control the objects ( Ref Des ) and net names while copy and paste a parts of an circuit you have some settings in DxD.
Goto Setup-->Settings-->Advanced in DxDesigner:
There are three settings that control the behavior of your objects:
1. Ref Des and pin numbers:
The 'preserve packaging info on copy' option controls if you copy the Ref Des information one to one. If it's checked the copy of your circuit has the same ref des as the orginal circuit. This may makes sence if you copy a part of a schematic to another schematic or project.
2. named Netnames:
the 'unique names on copy' option controls if you copy the netname information one to one. If it's checked the copy of your circuit has new system generated named netnames. If it's unchecked the new copy has the same named netnames.
Only for copy sheets you can use 'copy constraints on copy sheets' option to copy also the constraints of your circuit.
Hint: If you want to copy parts of your schematic from one DxD session to a second DxD session keep all setting equal in both DxD sessions.
This design looks like it has been translated from Design Capture - you can change the settings in the DC2DX translator to handle this situation. For designs where you have inadvertantly created such shorts you can run DRC-121. It mimics the checks in DC where you need inter and intra page connectors to ensure the correct connectivity.
you have to configure DRC-121, first of all you need to configure your link symbols, go to setup-->settings in the special components section.
Check if there is a "link" symbol already attached, if not configure one that you used in the design already.
Then go to DRC 121 and activate "Use Link symbols as internal and flat symbols" and make sure that Internal and Flat checks is also enabled. Now the DRC 121 checks if all nets with the same name on one hierarchy level have link symbols attached, if not an error will occur.
DxDesigner generally does not need such link symbols for connectivity, on one level all nets with the same name are connected, but link symbols are very usefull as you can jump with them to the next area/page where the signal is also used. This works at the PDF printout also.
I was trying in EE7.9.5 version, it was not worked.
It works for me on VX2.1 version,
There is “Use Link symbols as internal and flat symbols” enable option.
Thanks for your help.
In 7.9.5 you have to configure the individual symbols used for inter-page (between sheets) and intra-page (on same sheet) connectors, in this case use a different annotate symbol for intra-page connectors and define them as libraryname:symbolname.1
I am using EE7.9.4 and I have the same issue. I need a check to find this kind of mistakes.
Under DRC-121 I can not find the option "Use Link symbols as internal and flat symbols". Intra-page connectors are defined in special components settings.
Is this option only available at later versions of DxD? From what version on?
Thanks for you help.
Use of links was a new option at VX.1.n (I don't recall the exact release as we are at VX.2.3 currently), in the prevous post you will see I indicated this with EE7.9.5 as well, which is later than the release you are using.