I've had a little luck creating a symbol without the little pin set as NC and type set to analog. Not an elegant solution, and I'd welcome any ideas.
What about using a drafting item for this? We use the same symbol you're talking about, but it is just a drawing rather than an actual symbol or part.
When you use the drafting symbol, does it get rid of the pin not connected DRC errors?
I'm not sure exactly what you mean. In the schematic, the pins will be visually connected to the drafting item. They should not be electrically connected (netted) to anything else. Do you get errors on no connect pins? The alternative would be to connect them all to the "NOT_CONNECTED" net which is designed to ignore these errors.
When I run DRC in layout for connectivity, it only flags pins that have nets that are unconnected. If a pin isn't netted, there are no errors.
I was getting errors such as "Input pin is not connected," but making it an electrical connection helped. However, I may have some funny business in my netlist as there are all of these No Connect "components" floating around. I will look into that.
What do you mean by drafting item? Are these symbols or simply drawings on the schematic? I thought being un-netted is the same as being not connected?
When a group of no connect pins are assigned to the NOT_CONNECTED net, this creates problems for test engineering when the board is tested as a populated assembly on a in-circuit machine. If any pin happens to become shorted to a NOT_CONNECTED pin, ALL no connect pins on the NOT_CONNECTED net will be indicted when the fail message is printed; or if one pin is highlighted in a cad viewer, they all highlight. Has anyone come up with a good work around for this situation?
I don't know yet whether this works out well, but I'm trying this technique :
Create an "no-connect" bus like this, for example: "NC[01-99]". Then, connect each no-connect pin sequentially to one wire of the bus.
+ each no-connect pin is accounted for.
+ nc pins are not connected together on a single "NC" net.
- You have to keep track of which bus subscripts are used and which are unused.
- PADS may bother You with warnings, at some point, about the NC bus lines being connected only to one point.
1 of 1 people found this helpful
This is very easy with DxDesigner and PADS Layout :
make a "power symbol" which is named e.g. NC, so the pins are shorted in the schematic. In the PCB Foward Dialogue there is a field where you can add a net which will be deleted from the netlist. Type in "NC", and the net will not be in the layout.
Thanks for the ideas everyone.
It seems that the general consensus here is that it's easy to do, but not readily apparent. In addition, most of the solutions involve shorting all non-connect pins which may have adverse DRC effects from design to design.
I'm going to submit a feature request asking for more natural built in support.
For DxDesigner-PADS see these two threads regarding No Connect symbols are their support:
The first post describes how to do it today in DxDesigner for PADS, the second describes how it is handled in DxDesigner - Expedition and the same mechanism will be supported in PADS VX.1