6
\$\begingroup\$

I am using a P Mosfet in the schematic, pin 1, 2, 5, 6 are all connected together. How is this done in altium?

enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ IIRC, if you overlay the pins on the schematic (really done in the library editor when creating the symbol), Altium will automatically put in a junction to electrically connect the pins together when you run a wire to that location. If it works you should see a junction dot appear. \$\endgroup\$ – isdi Oct 25 '18 at 1:23
  • 5
    \$\begingroup\$ Personally, I just put 4 pins on the schematic symbol. It's a bit messy, but it makes sure your layout guy knows exactly what you want. \$\endgroup\$ – The Photon Oct 25 '18 at 1:26
  • \$\begingroup\$ I agree with @ThePhoton. This is the way to go. \$\endgroup\$ – Tom L. Oct 25 '18 at 11:58
4
\$\begingroup\$

The easiest (and probably the most common) way of doing this is placing multiple pins on top of one another in the schematic. If you ensure all of the electrical "hotspots" are lined up with one another on the grid, they will automatically be "read" as connected to each other. Then, if you want to show all of the pin numbers (like what is shown in your image) you can adjust the pin number margins to separate them from one another. For example Pin 1 will have a margin of 10 DXP units, Pin 2 will have a margin of 20 DXP units, Pin 3 will have a margin of 30 DXP units, and Pin 4 will have a margin of 40 DXP units. They will show up in the schematic just like your image.

| improve this answer | |
\$\endgroup\$
4
\$\begingroup\$

This is long-requested feature, it has a history on Altium's bug/feature tracker that goes back to 2011. It is currently listed as 'in development'. If you have an Altium Live account you can view the feature request here: https://bugcrunch.live.altium.com/#Bug/317

Another workaround is to assign the same identifier to multiple pads in the PCB footprint, which will cause them all to be connected to the corresponding schematic pin. However this requires customizing the footprint to suit the pin layout of the component. This is not such a big deal in things like SO8 MOSFETS which have a conventional pinout, but would be a pain for ICs that use ganged pins but an otherwise standard package.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Changing the footprint pins designator to all the same pin is very common for Altium. It only requires that you create a separate footprint for that part. A good way of doing this is using a label designator. Altium recognizes phrases as well so you could say "drain" on the pin designator and also on the footprint pad designators. \$\endgroup\$ – Drew Fowler Nov 15 '18 at 21:55
  • 3
    \$\begingroup\$ As of 2018, it's unbelievable that the "industry standard" software lacks such a commonly needed feature. \$\endgroup\$ – Ayberk Özgür Apr 13 '19 at 12:24
3
\$\begingroup\$

Since you haven't gotten a better answer, I'll say you should just add multiple pins to your symbol. It's not as compact as overlapping the pins, but it makes your design intent, and the required connections, crystal clear.

It can look something like this:

enter image description here

| improve this answer | |
\$\endgroup\$
1
\$\begingroup\$

Instead of assigning the same identifier to multiple pads in the PCB footprint you also can assign the same JumperID to pads that connected together. But as you can see this is almost the same because for each type of pattern with connected pins you must have separate copy of "pad record" in library. In the early days of Altium Designer there was another option. Every schematic library element can have pin map for each connected model. As footprint is a model you can have a mapping table. Mapping was designed not only one to one, but also one to list. I mean one pin from schematic library's element to list of pins from pattern. (https://designspark.zendesk.com/hc/en-us/community/posts/115000098289-Multiple-PCB-Pin-for-a-single-Schematic-Pin). This feature was slightly more powerful then dumb patterns with connected pins as this mapping table is not the part of pattern. But still twice messy: this table must not be the part of logic element (i.e. element of schematic library) instead it must be the part of component; pin numbers seeng on shematics never show mapped pattern's pin numbers, so nobody know did you done any remap or don't. For now this type of logic-pattern connections is not supported by Altium though mapping tables for each shematic library element still presents. So, of cource, AD cannot be "industry standard" at list at component's library design.

| improve this answer | |
\$\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.