Orcad error when making netlist for hierarchical schematic

[Bavananth]

While I made a hierarchical schematic using orcad Capture CIS 9.2. But while I tried to male netlist for "pcb layout" It gives error messages as given below. I don't know what to do. Any help please?




********************************************************************************
Netlist Format: LAYOUT
Design Name: D:\BAVNB\ORCADDY10\MAIN_HIERACHICAL.DSN
ERROR [MNL0019] 'U1.4' is tied to nets 'N07942' and 'N07977'.
ERROR [MNL0019] 'U1.4' is tied to nets 'N07942' and 'N07977'.
ERROR [MNL0019] 'U1.4' is tied to nets 'N07942' and 'N07977'.
ERROR [MNL0019] 'U1.4' is tied to nets 'N07942' and 'N07977'.
ERROR [MNL0019] 'U1.1' is tied to nets 'N08776' and 'N09148'.
ERROR [MNL0019] 'U1.2' is tied to nets 'N01390' and 'N09148'.
ERROR [MNL0019] 'U1.7' is tied to nets 'N08119' and 'N09170'.
ERROR [MNL0019] 'U1.6' is tied to nets 'N08798' and 'N09170'.
ERROR [MNL0019] 'U1.9' is tied to nets 'N08149' and 'N09196'.

Continues...........

 

[pedro_nf]

error [mnl0019]

Check your diagram, you have a short between two nets...

 

[R00KIE]

is tied to nets

A short between two nets would make them the same net, I don´t see a problem there, although it doesn´t hurt to check.

Did you for some reason copy and paste some components in the sub-blocks instead of instantiating them? If so you need to update all the components references. Go to the Window menu and select your .opj then select your .dsn . On the toolbar you should see a black U with a blue question mark like U? the tooltip says Annotate, click it.
Usually I leave everything as it is except the action, I use "Unconditional reference update". Click OK and it will ask you to change and save your design, say ok and then try creating the netlist again.

 

[stepannp]

Re: is tied to nets

A short between two nets would make them the same net, I don´t see a problem there, although it doesn´t hurt to check.

Did you for some reason copy and paste some components in the sub-blocks instead of instantiating them? If so you need to update all the components references. Go to the Window menu and select your .opj then select your .dsn . On the toolbar you should see a black U with a blue question mark like U? the tooltip says Annotate, click it.
Usually I leave everything as it is except the action, I use "Unconditional reference update". Click OK and it will ask you to change and save your design, say ok and then try creating the netlist again.

Thank you very much!

 

[flanello]

The problem is that you have in the two sub designs the same U parts. Thus eg. U1.1 is tied to two nets (the net in first and second sub design)
You can change the name of the part for each sub design in the property window of that part (if necessary).
Do it automatically as stated by Rookie is often the easiest way.

 

[atripathi]

Also make sure you have correct mode set for project. If you using a complex hierarchical design you should have occurrence mode set instead of instance mode.

You can set this option from Tools>Annotate form