Two short questions about component creation

[slow_rider]

I am kind of new to Altium (moving form Eagle)... I have created a number of (simple) components and until now everything was pretty much OK, now I have a problem...

I have a dual LED (common cathode) and made a footprint for it in a footprint library, I also made a schematic symbol (with two parts) for 2 diodes. When I want to match the schematic with the footprint I see only 2 holes from the footprint library and not 3. How can I correct this?

Second question, I have made some footprints for some diodes. When I capture a schematic and place a generic diode I add a footprint to it (by pressing tab before placing it) and I select my custom footprint instead of what is available. How can I be sure the polarity matches up correctly?

[David_AVD]

Why does the LED schematic symbol have two parts?  Surely it should be one part due to the common connection?

For the diode, not sure what you mean by "custom footprint".  Why don't you have specific footprints with matching pin names?

[free_electron]

Here is how you this kind of stuff.

The thing to remember is that altium has no restrictions on how you name a pin.

So in the pcb: make a footprint for the led or diode , or transistor and name the pads A and K or B C and E for a transistor or G D S for a mos.
Instead of 1 and 2. Numbers make sense for ic pins.
I even use + and - if i make a footprint for an electrolytic. Altium doesn't care. No restrictions apart from whitespace

So, in the schematic i create a symbol and use the same names for the pins. My led gets A and K

Now, for you dual color led
Lets say ot is a common kathode and is red and green.

So in schematic library you make a symbol with a pin AR , AG and K. anode red , anode green and kathode
Make the pcb symbol and place the pads and name them same. AR AG and K

Everything automatically falls into place then. There is no confusion possible.

Second thing. Make an integrated libray. It saves lots of time .
File - new project -integrated library
File - Add existing to project and select you schlib file
File - add existing to project and select you pcblib file

While in the schematic symbol editor you can add links to digikey and add links to footprint directly. That way when you place the part in your schematic everything is there. You dont need to pick footprints anymore.

I have schematic symbols with the following names
Led-3mm-red
Led-3mm-green
Led-5mm-blue
Led-topled-white
Led-0805-purple

And other combinations...
I also have a pcb footprint for each of those that includes the correct step model including the color.

Now. Once you got the integrated library : compile it.
Project-compile integrated linrary
This creates an outputfile called intlib.

In your schematic editor add the compiled output.
Place part. You get the browser. Click top right on the search.
A new panel opens click topright on the little button with the three dots in it.
A new panel opens. This shows you the loaded libraries. Click the add button and browse to your intlib and add it.

Now altium will automatically find the parts you create.

Whenever you create new parts in your library (you can simply leave that project always open.)
Simp,y hit compile library and the schematic and pcb editors automatically get access to the newly created elements

During compulation you will get a report. Read it ! It will tellyou if there are pin assignment problems. Schematic pin names not linking to pcb pin names etc. go fix those.