1
\$\begingroup\$

I wonder whether I can aggreate multiple physical parts (say 10 capacitors of same value and footprint) into a single symbol to reduce the clutter on the schematic. I know that the other way around - one physical part (say capacitor array) can procude multiple individual symbols but feel that the other way around would be just as useful.

Any thoughts?

\$\endgroup\$
  • \$\begingroup\$ The only use I can imagine for this feature is the placement of identical blocking capacitors in a circuit. Are there other uses you can think of? Perhaps there are other, better solutions for your problem available. \$\endgroup\$ – Ariser Jul 30 '15 at 9:18
  • 1
    \$\begingroup\$ @Ariser thats exaclly what I am after. Other uses would be identical filters on a number of ADC inputs or similar. \$\endgroup\$ – Arne Jul 30 '15 at 11:14
  • \$\begingroup\$ Ok, I thought so. I tried to address both use cases in my answer. I hope it's not tltr. \$\endgroup\$ – Ariser Jul 30 '15 at 12:21
  • \$\begingroup\$ Why would you want to do that? I can't think of a single good reason. If your schematic is cluttered, draw it better. \$\endgroup\$ – Matt Young Jul 30 '15 at 12:25
1
\$\begingroup\$

First of all, we should distinguish between Eagle's symbol and device. A symbol is a schematic representation, while device integrates both symbols and a package. You can have only one package for a device being used at a time, so you can not do what you want this way.

However, from what I have read, in Eagle 7, there is a feature called hierarchical design, that lets you combine many devices on a schematic into one block that you can use around your project. I think that it would allow you to combine many capacitors (or any other devices) into one block for better readability.

\$\endgroup\$
  • \$\begingroup\$ Unfortunately I'm stuck with Eagle 6. Thanks for the pointer anyway. \$\endgroup\$ – Arne Jul 30 '15 at 11:15
  • \$\begingroup\$ @Arne So am I. For filtering capacitors you can always just put hem between VCC and GND symbols and move them aside, or to another sheet. Just make sure that net names are the same. \$\endgroup\$ – mactro Jul 30 '15 at 11:49
0
\$\begingroup\$

There's no such feature in EAGLE, and probably neither in other EDA-tools. And odds are low, something like this will be implemented in the near future.

Why that, you may ask. Why is there a possibility to have several symbols in one device, but not more than one package?

It's because this will break the design process. Let's assume your first use case, which still makes some sense in a way. You have a bunch of 100 nF capacitors to place. You want to connect P$1 to VCC and P$2 to GND on every one of them and have only one symbol in the schematic. This will somehow fit, but the drawbacks come up soon. So you placed a C in your schematic and connected the two nets. Automagically 15 packages arise in your layout, their pins already connected with rubber wires. You place and route. First drawback: Your device needs to specify in your library, how many packages resembling your part it connects. So, if you want 14 C, you need an extra device. This will bloat your library by an extra dimension! You may say: "Ok, then let's have the same mechanism, as in the schematic with optional symbols, that must be invoked to be drawn."

I say, you can't compare that. Breaking a part into several symbols in the schematic serves a purpose in the design process. You want to have a description as exact as possible of all functions in the schematic, by maintaining maximum readability. This is, why you split a 144 QFP µC into a bunch of 8-pin ports and some control blocks and a power supply block. This allows you to keep the net lines short by moving the ADC-block of the controller over to — let's say — the analogue part of your schematic and have it even on a separate sheet finally.

What's with your capacitor resembling 1-15 capacitors in reality? Which value to display? 100 nF or 1400 nF, if you invoked 14 elements? In your schematic you can no longer show, that you have a capacitor next to each IC. And you also cannot calculate the electric behaviour of your capacitance for sure, which will break an export to any simulation tool based on schematics like spice.

So even if you were accepting this drawback. How could you implement your second use case? Having several filters on a bunch of ADC inputs? This forthright said makes no sense at all. If you have only one symbol in your schematic, how can you connect it to more nets than the pins it exhibits? Just impossible.

For your first usecase you may go the way of making yourself a blocking capacitor symbol with power pins instead of passive pins. These pins will wire themselves, so you can reduce drawing effort in your schematic. But this will not increase the readability of your schematic, as nobody — except you — will know, which net they connect.

One last thought. If you have so many similar parts with the same function, that you get problems in keeping the overview, you will have enough other parts to spread everything across more than one schematic sheet to sort out the functional blocks.

Remember: You need a schematic to keep the function of your circuit obvious. This is the sole purpose of a schematic. Everything else you can accomplish by editing a netlist in notepad.exe (or vi, which I prefer).

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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