These three properties are required by packager tool and cannot be deleted Of the three the packager only needs to consider Part Number, but if all three are defined in the 'part definition' which is the mapping between symbol and footprint (gate info, pin numbers, pin swapping) then packager will evaluate all three so they must all be on the symbol.
Properties are not necessarily symbol defined, they can be annotated from different tools, for example the packager of back annotation from layoit will add pin numbers and reference designators. You may define them on the symbol without values so that you control where they will appear on the symbol as they get added. You may also control visibility by adding them to the symbol as a placeholder.
Other properties may be added from Databook/Search when you add a part into the design. Using Databook/Search to add parts allows you to use a common symbol and annotate different part numbers, values etc. For example you use the res.1 symbol for all of your resistors and in Databook/Search you have many resistors - when you place the part Databook annotates Part Number, Value and any other property you want added to the res.1 symbol to make it unique. The part definition in the library must hacv a corresponding Part Number in the Part Partition and packager then resolves the mapping between the schematis symbol and physical part.
Robert, thank you for the quick answer.
What do you mean, exactly, when you say: "mapping between symbol and footprint (gate info, pin numbers, pin swapping) then packager will evaluate all three so they must all be on the symbol". Isn't this checked already by the check part function in the Part Editor?
I may be a purist, it coul be considered fusiness by many, but honestly I never worked with an ECAD that forces you to put three properties to a component. For me, it doesn't make sense. Also, I wouldn't really know what I should write in those three field. It's really a weird wall to impose to a designer.
And in the Evaluation Guide this part is not explained at all.
Anway, for now I've been rebuilding the Central Library, because some of my precedessor made an insane mess.
And the way that I thoutgh was better to rebuild a new, neat Library (for the knowledge that I have about PADS) consist in: attaching all the properties to a component in the Symbol Editor, leaving them undefined (with the value property field bank).
In this way, in the databook, I have generic part with a lot of fillable properties that allow me to customise the component as I need, and, at the same time, I have a small number of parts and symbol in the Central Library.
I do not want thousands of resistor or capacitors that use same symbol. This is the way that I figured out.
If ther's a better method, like the Databook one related you was talking about, I'll hear/investigate willingly.
The current PADS integrated flow is a bit of a hybrid (those projects that use the central library). The part editor is PADS the central library format PADS Professional/Xpedition so what you see in the UI doesn't really show the required information in a particularly clear way. If you have PADS Professional you can use the central library without a Databook parametric database and simply use the information in the library. This is where the Part Number, Part Name, Part Label usage comes from. In VX.2.4 in PADS you will have the native library Part Editor and the data will become a little clearer to view.
The recommendation from Mentor is to have a unique Part Number in the central library for each part, this guarantees packaging will succeed but means you generally have to duplicate the data between your Databook database and the central library. In this case the Part Number would be unique, the Part Name may be unique but doesn't need to be and the same for the Part Label. Equally you could use a common Part Name and/or Part Label, or have no entry at all.
As an example I used to have a generic resistor Part Number=res0603, Part Name was the symbol name Part Name=res and Part Label was a buying specification ABC123 for example. Then I'd have Part Number=res0805, Part Name=res and Part Label=ABC123. In the native part editor you could set one of the Part Names/Numbrers as the default so with a symbol without any data it would package into the default. Let's say res0603 and add Part Label, Name.
If you have empty Part Name/Part Label then you need Part Number on the symbol, but packager will not evaluate Part Label & Part Name. If you add Part Name to the symbol then it will look up the Part Number and see if there is a part with a corresponding Part Name - in this case it will fail as you have no Part Name entry in the library (but it doesn't apply in your case).
From your description you are mixing Databook and the central library - your Databook database (Access/Excel/SQLite) should have lots of entries, the central library may have a few entries or a corresponding set of entries that match the parametric database.
Anyway, this forum is not a good place to discuss this, the subject is too complicated for such a discussion board. Take a look at the StarterLibrary shipped with the release for one way of doing this (the duplicated set of entries) and read the documentation to discover other options.
So, you are telling me that I can control everything from Central Library? I thought that DataBook was a representation of the CL in xDX Designer!
Every time I added something in the CL, I used to update DataBook with Update Library command, showing the last modification. For me was obvious.
Even because, actually, I don't know how to put components into schematic if not using DataBook.
I don't fully understand you last answer, maybe for the topic itself or for my lack of knowledge or even for the fact that I use PADS VX (not VX.2.4) with the Standard License so I don't have some of the options you described.
Also, "Part Name" "Part Label" for me doesn't mean anything... maybe Part Number but it's actually commonly called "Manufacturer Part Number".
It's really a huge limit and confusing to have something similar but undeletable and chosen from the SW Company that made Mentor, and not by the designer.
Also, for what I saw, in my opinion, some fundamental action and some features of PADS MUST be explained in a more clear and comprehensive way, considering how much expensive is the software.
It's just a consideration.
And for what concern my original question, it has been answered, though, it's not good stuff to hear. I will evaluate this change.
Thank you again.
Part Number is the built in system unique identifier for a physical part in layout - you must have this, it is the index of the central library (look at the Part tree in the Library tools navigator). Any property that is listed as System cannot be deleted.
When working with the 'Databook' window in the schematic you are essentially looking at two separate databases. You will note there are two tabs: Search and CL view. Search looks at the parametric database (if you have one) associated with the central library, but it is not the central library. It may be an Access database, MySQL, SQLite, Oracle or Excel. Here you can define all sorts of information about your parts, Part Number, Manufacturer Part Number, value, rating, tolerance, cost etc. anything you might find useful to search on to find a part or data useful for mining - data sheets for example.
In the CL view tab you are looking at the data as it is defined in the central library - here you need only Part Number (and it may have Part Name, Part Label as well). The CL View - Part tab shows the Part Data from the central library (Part Number) and the mapping between this Part Number and the symbol and footprint (the slot - which is the mapping to the pins). The symbol view shows just the symbol - it is dumb, it has no packaging information. You could place a part from the Part Tab and it will package but it probably won't have all of the information you want on the symbol - this is where you use a parametric database and annotate the properties you are interested in from here, it will allow you to add as much or as little information you require.I would suggest you don't go over the top with this, otherwise verification becomes more difficult. The reason for this is that the central library originated in the Xpedition flow which didn't have Databook and so the central library drove most of the data, when we acquired Databook it gave us more capability than the original central library flow but wasand still is not compulsory to use in the tools.
Is this current set up ideal? No it isn't and we are looking at ways to better integrate this to make it less of a barrier to users.
I was aware about the other database. But, considering that my company use a small amount of electronics components, we decided to avoid the parametric database.
So in this case, I am forced to put and define every property on the CL side, is this correct?
So, basically the way I used since now should be the only one.
Infact, every time I create a part I manually set up all the properties in the Symbol Editor and then I place it directly from Parts Tab of the DataBook.
I don't even see a "CL or a search view" in the DataBook, maybe because we never set up the parametric database.
Now, with your last post, the stuff is more clear.