2
\$\begingroup\$

Eagle version 9.6.2

I'm creating a schematic with an dual op-amp, LMC6482. What I'd like to do is place this component on a schematic twice, but have those two diagrams represent the same physical component on the board. The reason is that one section of the schematic will apply to one of the op-amps on the IC, and another section of the schematic will apply to the other op-amp on the IC. But "wiring" them to the same object on the schematic will be a bit messy.

I suppose my fallback would be to place the 6482 on the schematic once, and use labels to connect the nets, but I find that practice not as obvious to the user under this type of scenario.

Is there any way to place a component on a schematic twice but have it represent the same physical component?

UPDATE WITH TOM'S SOLUTION

I edited the library I downloaded, duplicating the symbol three times, one for Gate A, one for B, and one for the Power Rail, and named them appropriately. I deleted the original symbol with all of the pins.

I then reconnected the pins to the three symbols. My existing schematic didn't want to update the components, but since I only had 2 on the diagram I just deleted them.

I then re-added the component from the library. By default it shows the first symbol (which was Gate A). You can then right click on the component and choose "Invoke" and it adds the next component (Gate B). Then I did the same for the power rail.

\$\endgroup\$
0

1 Answer 1

6
\$\begingroup\$

In Eagle you can create a single component with multiple schematic symbols. You couldn't have a complete copy of the part (as the title implies), but you can split a the part into smaller symbols each with some of the pins as the body of the question seems to desire.

For your dual op-amp part, you can create a symbol for each of the two op-amps, and possibly a third for power rails. Then in the when creating the component in device editor in the library you add each of your symbols to the same component, then assign pins.

When adding a component with multiple symbols in the schematic, each of the symbols can be moved around independently.


Here is an example with a dual comparator part. In the library there are three symbols for the part:

Multiple symbols in the same part

Then in the schematic each symbol can be placed wherever desired:

Schematic with symbols A and B

\$\endgroup\$
2
  • \$\begingroup\$ Let me give that a try and will get back to you. The library I had for this component I did not create, but downloaded from pricing.snapeda.com/parts/LMC6482IM/NOPB/Texas%20Instruments/… \$\endgroup\$
    – LarryBud
    Feb 10, 2023 at 14:26
  • \$\begingroup\$ You can use many other opamps from the eagle libraries as long as they have the correct pin assignment and the footprints that you need. You always can rename the part to match yours. Which version of eagle do you use? \$\endgroup\$
    – datenheim
    Feb 13, 2023 at 7:56

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.