If you are using PADS Layout, then you can use the 'Copper bridge' function.
Draw a piece of normal copper (not copper pour or plane), and mark it as a 'Copper bridge'.
Then define which nets to bridge.
In the example below I have bridged $$$22735 and $$$22736. But I guess this may normally be done with AGND and DGND or similar.
The bridge will not show up as a clearance error.
It is possible to find all bridged nets by using 'Edit > Find' function.
as you posted your question in the dxdesigner community, you seem to be using dxdesigner, right? Just recently I investigated this myself and found the following hint (please don't ask me the thread, I don't remember...)
Use the pipe "|" to connect two nets together as shown below:
The result in the net-list is the follwoing:
- This will only work with two net names, merging more nets like "NET_A|NET_B|NET_C" will not work. (but "NET_A|NET_B" and "NET_B|NET_C" will do the trick...)
- Besides, the nets won't be linked together when you export the schematics as a pdf. You can follow "NET_A" from one occurrence to the next, or "NET_B", but you won't be forwarded from "NET_A" to "NET_B".
- I tested this with PADS Designer VX2.3. the original thread was ancient, so it should work with older versions too. Not yet tested with VX2.4.
Hope this helps.
You got your answers already, but both solutions (one for Layout, one for xDx Designer) are dangerous (the firs), not really a good design (the second).
A net should NEVER be connected to a different one with just a wire. Neither you should use copper bridge, to modify the connectivity. xDx Designer is the Master, Layout is the Slave. Connectivity is established at schematic-level.
If you really need to connect two different nets, then use a jumper. Jumper can be real or "fake". For fake I mean that you can use a small segment of trace as decal, in this way you don't add footprint. I mean, you do actually, but you can treat it as a normal trace that will be covered with soldermask.
In this way, you do not need more space or to modify the Layout, just to reroute a small piece of the net.
A net should NEVER be connected to a different one with just a wire.
in general, you are right with what you say about connecting two nets. But sometimes it is acceptable, at least for me. You have to be careful when you use the "pipe in name" feature, and you should write a short comment about why you used it. But in my opinion that's true for "fake" jumpers too.
It's a good habit ofc, but if you put a Jumper (real or whatever) in xDx Designer you have a clear, visible symbol between the two nets you are shorting that says "hey dude, these net are connected!". Without a Symbol you can forget to put the comment, delete it or whatsoever.
Not only this, you can manage the short in the layout since you have a decal for the transition that remembers you that.
In any case, shorting nets it's a practice that require attention and the full awareness of what you are doing.