Assigned two 3D models to same footprint in Altium

[leventcinar2000]

How can i assign two different 3D models to the same footprintin Altium

 

[Kick]

Create a footprint without 3D and in the layout use place>3D body to import your 3D models. There you can use any 3D models (if your not satisfy with one model, just replace with other model).

 

[leventcinar2000]

I want to assign two or more 3d models to the footprint (such as 3mm red, green, yellow led)
When i use the footprint of led, can i select one of 3d models. Such as, when i use resistor symbol in SCH mode, i can select one of footprints (SMD0805, SMD1206...)

 

[andre_luis]

Although I dont't know how to achieve that, I see this as a quite usefull question. There are components having exactly the same footprint, but available with different profiles ( e.g. electrolictic capacitors ).

 

[ArticCynda]

Creating a separate footprint and swapping the STEP file for one with the correct height appears to be the only solution for this. For easy reference, you could follow the elco naming convention from 3DContentCentral, for example.

 

[zuzu]

Well, at least this kind of feature is quite easily (as concept) in Altium.

1. Create 2D footprint with your LED.
Use A and K as pad designators and blank for pads that are used only for mechanical purposes.
You also can tie them to one existing pins (eg. A or K) if you like, for better thermal dissipation so just name several pins as A or K.

2. Copy-paste this footprint in the same PCB library and name them convenient like:

LED_0603_R
LED_0603_G
LED_0603_B
etc

3. Place in each one, particular 3D model, according your actual component may look

4. In your generic schematic library (since LED is quite generic component) create or copy-paste a LED schematic symbol with the same logical pins that you have created in footprint (eg. only one A and one K need, even several A or K are defined in footprint).
Create a custom parameter named "Color" leave blank it's value for the moment.

5. Copy-paste this symbol in the same library and save each one with parameter modified

Color = Red or Blue or whatever

use convenient names for each schematic symbol:

LED_G
LED_B
LED_R

and add for each one, as many footprints you like (Models -> Footprints) but with the same color.
The idea is your "generic Green LED" to have all your packages of green LEDs

LED_0603_G
LED_0402_G
etc.

6. Done, now you're organized

Anytime you put a LED in schematic you must choose a colorized one, and each one will have as may footprints (with proper 3D) you like.

YO3HCV, Edi