it is not possible to connect different nets, this would always be seen as a short. One possible work around would be to find and replace the netnames, i.e. replace AGND with GROUND. This will rename all AGND nets to GROUND and you will only have one net left. The diasadvantage is that you will still have different Global Symbols in your schematic.
Thanks for your suggestion. I'm reluctant to go that way because it would leave a feature of the design that might be hidden from someone re-using one or more sheets from it. If there was a linking symbol, that would always be visible and alert a user of the designs to the fact that two loads are in fact supplied from the same source.
If the two loads come from the same source, they are the same net, and should be named that way. +5V is +5V everywhere it is actually connected. Create your schematic the way you need it (schemaatic should describe the circuit, not the physical connections). If someone wants to reuse part of it, they will need to do some mods anyway.
If you are using ReUse Blocks, there is a dialog to rename the Globals. I don't think you are so...
It is possible to merge 2 nets together using the | pipe. This includes Globals. In the image below, I have merged VDD and the PWR nets throughout the design. The pipe is used in the Global Signal Name on one of the TAPS.
Have you checked out my blog at http://blogs.mentor.com/dxdesigner/
If only life was so simple! In an ideal world, we would do as you suggest but it would be better for us not to have to traverse the whole design changing the TAPs for this board not least because of the risk of error when modifying a design which has many elements not designed by this team.
Thanks for showing an example of the "pipe in name" feature.
We did give this a try and found that nets connected to such a TAP retain their net name and that name is then added to the text associated with the TAP, in addition to the name1|name2 text. We were left wondering what would happen when the design is flattened and a netlist produced. Do name1 and name2 become one net?
If so, we could use a structure like this to acheive the effect we want:
I tested today with hierarchy, you would have to use the pipe command to merge the nets on each page for a design with hierarchy or run the power through the hierarchical block symbol to maintain connectivity.
Thanks for trying that out!
Unfortunately, if we have to merge the nets on each sheet we would be as well to manually change all the TAPs.
We would consder bringing power to a pin on sheets and symbols we expect to re-use. That seems to be a good way of encapsulating the circuit for re-use while still using global nets for connections to many places in the design.
1 of 1 people found this helpful
You only need to connect the Global's on ALL sheets (and hierarchy levels) if you want to see the combined Netname on all sheets in the Navigator Window.
If you also use Supply_Rename property in DxD, please check also the value. The value MUST be the combined Netname NOT only one of the Nets.