How do you add a decoupling cap to a 32KB RAM?

[DON PREFONTAINE]

Eagle v9.1.3 Standard
IC: CY62256NLL-70PXC
Library: memory-sram  Static RAMS (urn:adsk.eagle:library:278)
Sub-library: CY62256LL-?*
Item: CY62256LL-PXC   DIL28-6

The Symbol shows one object for the chip and two other devices that are VCC and GND. They seem to be categorized as P in the Symbol drawing, obviously for Power.

Here's the question: how do I put a decoupling cap on schematic for the IC if the power pins only show on the board?

Thanks,

Don

P.S.  Is there an easier/faster way to add antispike/decoupling caps to ICs in the schematic? Has anyone done a video on this?

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/245009

Attachments:
32KB-SRAM_Symbol.jpg

[David Murphy]

I assume you place the capacitor between the two power pins (14 and 28) on the schematic. Have you tried this? That should then show up to be routed on the board.

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/245021

[Gene Breniman]

Don,

After placing the RAM device on the schematic, move to the side tool bar and select 'Invoke' and left click on the RAM device.  This will pop-up a menu that will allow you to select and place the 'P' part containing the power pins onto the schematic.
Then you can connect the power to part and place bypass caps.

Back in the old days, a lot of schematics would place all of the bypass caps on a separate page.  I guess you could do something like this, place all of the caps together in a 'power supply' section, then when placing parts in the layout, just move the bypass caps where you want them.  I like having the caps on the schematic right near the parts, so I know that I have them in the right spots.

Good luck!
Gene

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/244990

[Rob Pearce]

Post by Gene Breniman
Don,
After placing the RAM device on the schematic, move to the side tool bar and select 'Invoke' and left click on the RAM device.  This will pop-up a menu that will allow you to select and place the 'P' part containing the power pins onto the schematic.

One small addition to Gene's excellent answer:

The reason library is set so that the P "gate" isn't shown immediately
is that Eagle treats pins with "direction" set to "pwr" or "sup"
specially. If not explicitly shown otherwise, they make automatic
connections to a net with the same name as the pin. If your circuit has
only one power supply, e.g. VCC & GND, and if all your components use
those same supply names in their P gate, then you don't need to clutter
the diagram with power connections.

If you take that approach, you can still add decoupling capacitors by
placing them anywhere on the schematic between explicit supply symbols
for the power rails you're using. The nets will automatically connect by
name.

Most people these days prefer to make this explicit, using the "invoke"
method Gene explained. If you're using a non-free version, you can still
declutter the main schematic by having a separate sheet dedicated to all
the power gates and decoupling, if that's your preference.

[DON PREFONTAINE]

Much appreciated, Gene!

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/245046