1
\$\begingroup\$

I haven't been able to find many resources on designing schematic views of parts with large numbers of pins in Altium. The Symbol Wizard (Tools > Symbol Wizard), which allows you to copy and paste large numbers of pin names, and creating multiple sub-parts are certainly both helpful, but is there a good way to deal with large numbers of pins that are internally connected?

When a part has more than 100 ground connections, how do you represent them in a schematic view?

\$\endgroup\$
  • \$\begingroup\$ Just out of curiosity, which part are you using that has over 100 ground pins? \$\endgroup\$ – Tyler Jul 24 '17 at 17:17
  • 1
    \$\begingroup\$ @Tyler A large FPGA can easily have 100 ground pins. I've got a Spartan-6 in a 256 ball BGA (which isn't large as FPGAs come). It has got 26 ground pins. \$\endgroup\$ – Nick Alexeev Jul 24 '17 at 17:20
  • 2
    \$\begingroup\$ Mostly with many pins of the same connection I just make the pins, have only one show the signal name, the rest shows nothing and then you put them over each-other. The "hidden" and "connected to" stuff gets messy in some projects. \$\endgroup\$ – Asmyldof Jul 24 '17 at 17:23
  • \$\begingroup\$ As an aside, Eagle has got a way of combining multiple package pins as one schematic pin with multiple pin numbers. See here and here. \$\endgroup\$ – Nick Alexeev Jul 24 '17 at 17:25
  • 1
    \$\begingroup\$ I usually create a "power" symbol and put all the power pins on it. I line up all the GND pins on the bottom. I do not like to have hidden pins. I have never had to deal with 100 GND pins, though. More like 20 or 30. I put all the bypass caps on the same page with the power symbol. \$\endgroup\$ – mkeith Jul 24 '17 at 17:45
1
\$\begingroup\$

I've seen people represent parts like this by having dedicated pages for them. An entire page listing just 200 ground pins and 1.2V rail pins is not uncommon.

I would suggest not to put pins on top of each other in a PCB schematic (this is different form a functional schematic where you try and represent signal flow/dataflow). You want every pin to have a poin in the schematic. This way, when debugging, the person doing the debuging can always consult the PCB schematic to look what function a pin is (this can be very important when looking at say noise issues. "Is this pin next to this trace a digital pin carrying a lot of data and causing noise coupling into my analog rail? Oh, it's +1.2V, so I think it won't be the main cause")

When dealing with a part this large, it is important to split the part up into multiple blocks. Don't have one big yellow blob with 1000 pins on it. Something like a LVDS block, DDR block, POWER, etc.

\$\endgroup\$
2
\$\begingroup\$

I come across this on almost all designs I do. And the answer is always the same.

Place all the pins on top of each other in the schematic symbol, such that their 'active' ends coincide. Hide their pin identifier and name. Place free text in the schematic indicating the internally connected pins, their pin numbers as a list and and their function. E.g.

1-10: GND

I'll update my answer with some pictures as an example next time I'm at my CAD PC.

In the PCB just reference all the pins by their ID and location normally.

That way in the schematic a single connection to a pin completes all the connections in the PCB. The schematic becomes far less cluttered. It becomes impossible to accidently connect pins wrongly.

The only danger with this method is that it hides the 'single pin net' DRC error. Because of this it's important to make sure it's obvious the pin should be connected to a valid signal or power source within the schematic symbol drawing.

\$\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.