Ah, I think I have an answer for you. The pins are not omnidirectional. There is an inboard side, this points to the symbol body , and an outboard side that will connect to nets.
I am guessing that on the occasion when you seem to connect a net, the net really connects to the inboard side of the pin and lies under the pin looking like it connected to the outside.
What you need to do is flip the pins around, make them point out.
Of course it could be one of a million lesser likely issues. The next issue I would think of is off grid pins or nets. If the symbol was made on one grid, and then placed on a schematic with a different grid. You can drive yourself nuts trying to connect nets but they just will not.
Isn't that the whole point of having a "LEFT" and "RIGHT" pin type? Whats the recommended type for pins on the right side of a component. Seems silly to call a pin a "RIGHT" and still have to flip everything around 180 in the symbol editor.
There is a diamond on one end of the pin in the symbol editor when you select it. I assume that is the "connect to nets" side. It is shown on the outward part of the pins on the right side of my symbol.
Well it was an idea. Happened to me, you are correct the diamond means it connects. What about the grid argument, anything there?
Shouldn't be grid issues. I do the symbol pins on 0.1" grids and I have the schematic editor set to 0.1" grid. I noticed my cursor coordinates in the bottom of the schematic editor are reported in 0.001" increments but I don't think that has anything to do with it. The symbol in the schematic editor is on 0.1" grid.
Well I am at a loss here. You could attach the symbol so I can open it up.
Ahh just figured it out. The symbol outline in the symbol editor did not extend to the outside of the "RIGHT" pins. I auto-fitted the outline in the symbol editor now all is well. Thanks for the help.
Does the symbol outline need to extend to include things like the reference designator?
We usually find that this is the answer:
The pins must touch the Symbol Outline in the Symbol Editor.
The white hashed line is the symbol outline (you can toggle this off/on in File > Preferences > Display)
The green circles show pins that touch and will allow you to add nets, the red doesn't touch the symbol outline and you won't be able to connect.
Glad you got it worked out.
Don't set the autoupdate symbol outline (also refered to as the bounding box)... It often causes the trouble you are seeing if properties stick out farther than your pins do.
The properties don't need to be inside the bounding box.