Skill - access to pins List

Question

Hello, 
 I am learning to use Skill language to develop scripts to automate some tasks on Cadence Allegro. As a training, I am trying to write a simple script that asks the user to select a symbol, and then the script lists all the pins on that symbol alongside the net name associated with the pin. I am using this very good serie of videos on the Cadence Youtube channel : https://youtu.be/bzXmQYvpCFc 
 I have some issues understanding how the different interactions between the design, the database and the language itself work. I have these two pieces of code : 
 axlSetFindFilter(?enabled list("noall" "symbols") ?onButtons list("noall" "symbols")) axlSingleSelectPoint() symb = axlGetSelSet() length(symb~>pins) -> RETURNS 1 pinsList = nth(0 symb~>pins) length(pinsList) -> RETURNS THE CORRECT AMOUNT OF PINS 
 
 allDBids = axlDBGetDesign() symb2 = nth(100 allDBids~>components) length(symb2~>pins) -> RETURNS THE CORRECT AMOUNT OF PINS 
 
 As you can see, in the first code, I trigger a selection (forcing it to symbols), then get the result of that selection in a variable (symb), then asks what is the length of the "pins" list. It returns 1, whatever symbol I pick. To get a list with 1 pin per list element, I have to use the nth() function as shown above. In the second code, I get the design DBids, then pick one (random) symbol in the list, and asks for the length of the "pins" list. It give the correct amount of pins right away. 
 Does anyone has an idea about what causes the symb~>pins list to have only one element (that is, in fact, the pins list itself) whereas symb2~>pins works as expected ? Maybe I am wrongfully using the axlSingleSelectPoint() function ? 
 Something I may add : When I try to use -> instead of ~> to access the lists, it returns nil everytime in the first code, but it does work with the second code, and I have absolutely no idea why. 
 
 Is there some place where I could find resources about Skill ? Do you know about some forum (else than this one that I don't want to pollute) or facebook group or anything where people discuss about this language ? 
 Thank you for taking the time to read this, and please excuse English, it isn't my primary language.

B Bruekers · Accepted Answer

One tip, look at each API what the possible return values are. This will save you a lot of headaches... Most of them you can find back in the Allegro SKILL Reference document. (see help documents) 
 From the API description of axlGetSelSet() : 
 lo_dbid List of figure dbids. nil Select set is empty. 
 So it always returns a list when something is selected. Even in the case if only 1 item is selected. 
 Each entry in ' symb = axlGetSelSet() ' is a symbol database ID. This symbol ID contains a list, a so called disembodied property list (DPL). This is basically a list of names and values. For example a name in the Allegro symbol DPL is 'pins'. You can find all entries in the 'The Allegro PCB Editor Database User Model' chapter in Allegro SKILL Reference documentation. 
 A basic LISP operation to get the 1st element of a list is car() 
 With the '->' you can access a variable inside a DPL It returns a single item which can be any valid variable type (list, float, string, etc) 
 With '~>' iterates over a list of items and tries to return the value of the given name. It returns a list containing the values which are inside the requested name 
 
 So; 
 symbols = axlGetSelSet() returns a list of selected symbol(s) 
 symb = car(symbols) ; get first item from list 
 pins = symb->pins ; is a list of pins. Each pin is a database ID. So the list looks like this: (dbid1 dbid2 dbidn) 
 length(symb->pins) ; returns pin count, same as length(pins) since 'pins' was set to symb->pins 
 
 By using symbols~>pins you will get a list containing lists of pins. If there was only 1 symbol selected then the length(symbols~>pins) returns 1, since there is only 1 'pin list' 
 
 Do you want to iterate over all symbols: 
 foreach(symb symbols 
 pins = symb->pins 
 println(length(pins)) 
 ) 
 
 symb2 = nth(100 allDBids~>components) length(symb2~>pins) -> RETURNS THE CORRECT AMOUNT OF PINS 
 This is because you assigned symb2 to the 100th item in the list of symbols. The ~> instead of -> in this case is working since the 'pins' itself is a list. However i suggest not to use ~> in any case, unless you are certain that you can not do without it. 
 
 Some small exercise: 
 axlDBGetDesign()->components Returns a list of component dbids axlDBGetDesign()->components->pins does not work. There is no single 'pins' property name inside the list of components. axlDBGetDesign()->components->pins~>number Same as above, component->pins returns nil, so no single 'number' property can be accessed. axlDBGetDesign()->components~>pins->number does not work. list with pin lists does not have a single property name 'number' axlDBGetDesign()->components~>pins~>number returns a list with lists of pin numbers 
 Difference between ->components and ->symbols: 
 axlDBGetDesign()->components contains all component instances imported from the netlist. No physical data like location, rotation etc. 
 axlDBGetDesign()->symbols contains all placed symbols instances in the PCB, so also the location, rotation etc.

mahimag · Answer

length(symb~>pins) this is returing 1 because the outout of symb~>pins is a list of list. For ex: a= symb~>pins will store ((dbid:000001778BC01148 dbid:000001778BC02038 dbid:000001778BC019C8 )) something like this for a 3 pin part. You need to extract the list by using car(a) or nth(0 a) and then use length function on the output. 
 b=car(a) should look something like (dbid:000001778BC01148 dbid:000001778BC02038 dbid:000001778BC019C8 ) and then when you use length(b) you should get 3 as output.

Stats

Skill - access to pins List

Community Guidelines