As far as my experience go, Symbol Editor won't allow you to save new symbol with duplicate names. How are you managing to do that?
I would like to borrow this thread as it has very similar subject as I would give a new one. My question is, how can I avoid naming pins with exact same funcionality differently?
For example, if I have 2 pins that have VD1 potential, and 2 pins with VD2 potential and four pins with VD3 potential. I would like to have only three pins visible - VD1, VD2 and VD3, and others I would like to have hidden.
Now if I want to get to the end without errors, I have to do VD1_1, VD1_2, VD2_1, VD2_2, VD3_1, VD3_2, VD3_3, VD3_4. And the symbol looks rubbish - lots of redundant pins. And the implicit option does not come in handy here, since I don't want to have permanent nets for these signals - net names should come from schematic, not symbol.
I don't know if this is a feature, but for me, it's definetly a bug. Can anybody suggest a solution for this?
I searched for this function as well, but didnt found it...
Right now i had to create for each pin a extra symbol pin, so that i got on some symbols 20 and more pins with the same function, this isnt very nice for the over view...
someone got a trick or solution for this ?
In symbol level, every pin must have a unique name, so for multiple GND pins, you have to name each GND pin with a unique pin name by adding _1,2..N suffix.This is a common methodology. However, you can add a bus pin instead of multiple GND_* pins and it's possilbe to just display GND lable instead of GND[100:0]. I occasionly created such type of symbols for power MOSFET which have multiple drain/source terminals, it make MostFET symbol have a simple 3 terminal apperance.
hmm, just checked it at my symbol editor, there isnt a "bus" - pin type.
theres no chance to use more then one pin number per pin name, by separate the names with a comma or semicolon?
just like this:
Pin Type: Power
Pin Number: A1, A2, A3, A4 ......
would be a great function and would make symbols much easier to create and use.
It is possible to list them as comma separated values, but that's for multi slot symbol only. For example when you have 4 OP AMPs in one package, you can create one symbol and on each pin assign 4 different values.
I too have heard that GND pins could be solved with bus pin, but I haven't found a way how to place them either.
thanks for your fast reply
seems that you all create for each GND / Power pin a separate symbol pin?
the current example is a DC/DC converter, and i got now 40pins:
- 10 input Vcc pins
- 10 input GND pins
- 10 output Vcc pins
- 10 output GND pins
this could be done with 4 simple pins, isnt this a mess?
It is! That's why it's worth to investigate how the bus pin is placed.
Another approach is to use implicit pin property. On a symbol editor, add another attribute named SIGNAL and in value type in the netname followed by pin numbers (ex. GND;7,9,15,16,21,85,86).
The problem with this approach is that these pins are then tied to fixed netname. You will have trouble if you want to connect them to AGND or anything else than "GND". Usually for GND it's not as big of an issue than it is for VCC pins.
If your backend layout is pads or other 3rd parties layout , you can use your method(pin name: multiple pin names, seperated by commas; pin number: mutilple pin nubmbers ,seperated by cpmmas), make all values be invible ,and add text string as pin lable reminder.for icdb flow, there is no need to add pin number on symbol becuase the map of logic pin<->physical pin is from PDB, so only you need to do is keyin pin nambe in bus name type, such as GND[100:0]. I have created a demo data for your reference.
however, you should take care of connecting wire to bus pin, all on your peril.
demo.7z.zip 281.7 KB
hmm okay, maybe the bus pins will be the solution.
yeah, found this function as well, but as you said, its fixed on a special net name and this isnt carryable in my mind.
i talked some minutes ago with another engineer at our company and asked him how they handle this situation / problem with altium.
he gave me the hint to place the symbol pins at the same place, so that it looks like a single pin and hide the pin names (i think this will create a point on the pin for the conection, but it could be a possibility)
maybe i could write a text behind this bin with the hind that this pin is (Pin A1, A2, A3 .... A10)
how do you think about this?
Edit: just tested it, but i`m not able to place symbol pins on the same grid, idea failed as well
will take a look on your example
when i try to open your project, i get an error:
unable to open iCDB connection
[2014.04.09 14:40:38] [0000m.00s.073ms]  iCDB Server PI: ERROR [Server Exception: Category[Server] Error[NewerDatabaseVersion] Description[Database is newer than application version, the project will not be opened.]
i use at the moment EE7.9.3 maybe its a bit to old
I tried this method as well. The great thing about Altium is that you can always find a workaround. I'm afraid Mentor is not made that way.
When you stack multiple pins over each other, you will receive annotation error when you'll try to forward schematic to PCB.
the demo data was create in 7.9.4 Build Id: 514029. Any lower version could open the data. I just creat a diode symbol which map 2 logic pins to 14 physcial pins by defining bus pin, see follwoing picture. Normally we only use bus pin for global signal and connect the bus pin to Global signal symbol. If you wana use this method to deal with normal pins, you have to know how to deal with connecting wire to the bus pin(you have to use bus to connect with bus pin). Although there is another workaround to connect a wire to the bus pin, but i don't talk more because it's not safe.
okay thanks for your help
seems that mentor dosnt support multiple pin numbers at one pin name
ill create now a chaotic symbol with 40 pins