Can Altium designer save symbols and footprints in it's projects for portability?
Yes AD does this by default, similar to how Eagle does it (pre Fusion Electronics).
I've taken over a number of different client projects over the years that were created in Altium but was never provided the original libraries. I have always been able to export all the component symbols and footprints into my own libraries, and then fix all the designs to then refer to those.
I only have experience of Altium SE99, and Summer 09 thru AD19, so I don't know if anything has changed in AD20/AD21.
does that include vault library parts used assuming that vault is actually a thing.
This command exists:
Make Schematic Library
That's basically all you need to know.
Tim
This command exists:
Make Schematic Library
That's basically all you need to know.
Tim
Well that is all the uncooperative subcontractor needs to know.
This command exists:
Make Schematic Library
That's basically all you need to know.
Tim
And an equivalent command exists in the PCB editor, good for rescuing footprints when the library has gone missing (which seems to be the case 99% of the time, at least with projects by Altium novices).
Simon, make sure your guy consolidates the libraries for you, it’ll save lots of headaches in the future.
does that include vault library parts used assuming that vault is actually a thing.
FWIW, you can use the Manufacturer Part Search to find the vault item, then use the Download command to save it locally.
If I use my expired CS licence I won't have access to the vault which is why I want to make sure it's not a case of here are the files but you need the vault to make it work, or course you have the vault don't you?
Yuppo. You can include a SCH/PCB library in the project, also you can extract the SCH symbols & PCB footprints from a given project to make into a new library
Does the Vault stop giving access once a license has expired? I am sure I was getting access even not renewing my support. It was a while back though so maybe things changed.
The project files store everything. unlike other cad tools ( hello orcrap ! ) that require access to the library.
The reason behind it is simple : version control. you can open a 20 year old design and be guaranteed to still have all data. you can run a check to see if anything has gone outdated but it will not "break" the design.
I mean, sorta? Open a project you don’t have libraries for and try to update the PCB and suddenly it’s “footprint not found” all over the place.
I have since figured out that one should be able to export the footprints from the PCB file into a new library (correct me if I’m wrong) and then use that “new” library to update the PCB.
I'd use kicad anyway if 6 really can do it. It's just a case of are all the required bits of information there.
Can Altium designer save symbols and footprints in it's projects for portability?
Yes and no. The symbols and footprints are stored within the files themselves. However, a sane designer will use a component database which has all the metadata (like manufacturer, order number, supplier order number, etc). That information may not end up in the project file (or could be outdated). So besides the project files you will also want to have a bill of materials that is generated using the information from the database. Or better: the component database itself but that is usually not something that gets handed over that easely.
Can Altium designer save symbols and footprints in it's projects for portability?
Yes and no. The symbols and footprints are stored within the files themselves. However, a sane designer will use a component database which has all the metadata (like manufacturer, order number, supplier order number, etc). That information may not end up in the project file (or could be outdated). So besides the project files you will also want to have a bill of materials that is generated using the information from the database. Or better: the component database itself but that is usually not something that gets handed over that easely.
I already have the manufacturing data, the issues would be the lack of design data that has been paid for. I just want to make sure that the excuse of libraries, is just that!
Google for 'Altium create integrated library'
It is a bit cumbersome process in itself. There are tutorials how to do it. You can create both schematic and footprint integrated libraries specific to the project.
I just don't want the project to fall apart when I open it in CS or KiCad to make mods.
Not sure if Kicad can read Altium's integrated libraries
I just don't want the project to fall apart when I open it in CS or KiCad to make mods.
Typically you'll need to have the Altium files written (exported) in ASCII format in order to import them in other programs. But even then importing projects from one PCB package to another is not something I would recommend. It is very likely that the definition of how elements are built are incompatible. So you end up with something that looks the same but isn't. Take a pad surrounded by a polygon (copper pour) for example. In CAD package A the clearance around the pad could be defined by the clearance in the polygon definition where in package B the clearance could be defined by the thermal relief setting of the pad. To make matters worse: these can also depend on a global setting of the design which may not exist when going from one CAD package to the other. This is next to impossible to translate automatically. And then there are things like constraints for trace widths, distances, matched impedances, trace lengths, differential pair phase matching, etc.
IOW: if you have a design in Altium, then edit it with Altium. Getting a converted design cleaned up properly is likely almost as much work as re-doing it from scratch.