Altium Vault - Lifecycle Management

[DarkPrince]

Hello everyone. It has been a long time since I've had a serious post here. Of course, I've been lurking in the shadows though.

To my point of posting here though. I've been using Altium Designer for the past few years developing boards for the company I work for. We've been bouncing between SchLib libraries and Personal Vault based data storage. After some issues with the Personal Vault, we decided to dive into the full version of the Vault with all the management features. Due to changing requirements/standards I am going to migrate to the new Vault manually, fortunately our Vault library isn't too great and the redundant work is minimal. This on the other hand, offers me the opportunity to set the standards in revisioning and lifecycle schemes. I am curious on if anyone in the community uses these Vault tools and how they use them. Also if I can learn from another persons mistake maybe I can avoid one iteration of this.

What revisioning schemes do you use and why?

Do you use the Vault's lifecycle management tools? If so what scheme do you use?

Second question, why would a lifecycle ever transition backwards in its lifecycle? For example, from “In Production” to “In Prototype”, I feel this is an impossible transition. If something is wrong, a new revision of the item will have to be created anyway, resetting the lifecycle to “New In Design” or what the first state & stage is.

I am hoping to at least use the lifecycle system, as we have a thorough internal review cycle and it would assist the reviewer to be able to flag reviewed/non-reviewed, and I can setup a lifecycle to flag these things.

Thank you.

[free_electron]

Enterprise vault user here. (200 + users / 10.000+ parts / split vault/oracle server).
Since i am the vault master i know pretty good how it works.( i set it up)

Tip 1 : make folders for Components, symbols and footprints.
tip 2 : make subfolders for categories. resistors, capacitors, ic, transistors.
tip 3 : for component folders only : make sub-sub folders. nmos pmos, zener , shottky , analog digital etc ... 0402 0603 0805 ... you get what i mean.

tip 4 : learn to use the templates and create template for each sub category. Set defaults in templates and force requirements of parameters from there
tip 5 : drive parameter visibility from the folders.
tip 6 : do not store anything in the symbols. it is useless. don't tie anything to footprints. Only set designator and description. drive comment field from the component.

tip 7 : when creating pcb parts you will find out that often the description does not get loaded ( depending on how you create the part ) , or you have to enter it again on a secondary screen.
to create new parts make a local library for sch and pcb and link those to an incoming library in the vault. This allows you to avoid this problem. bonus is that any incoming part ends up in an invisible library so end user cannot use it unless it has gone through lifecycle ( new parts always come in 'from desingn' )

tip8 : cloning is your friend. you can clone symbols, parts footprints. when cloning parts : you can clone symbols , footprints inside the parts editor as well. need to add 4 0805 resisots ? clone any 0805 , then simply click 'add' at the bottom to inject 3 more and release all at once. the grid can copy past straight from excel.

tip9 : resitrict the number of people the can edit / create vault parts. you need a librarian. you can allow people to create symbols and footprints but there should be a gatekeeper to take them into the vault and tie it together.

tip10 : when creating templates : use Manufacturer and Manufacturer PartNo as fields. nothing else !. the octopart integration triggers on those keywords. you get full blown integration for free that way.
tip 11 : altium is sensitive to keywords. that means you can use certain keywords as fieldnames. for example 'grouping' will directly trigger to the annotator process. we have a situation where we need to store our internal product code under 3 fields. Reason being that our internal PLM system (enovia) needs a keyword called 'TPN' to find the column. a life modeling tool (sherlock) uses its own field for crosslinking the database. and then we store the 'comment' field so that altium overrides the comment properly for the schematic symbol. inside the vault i simply set the comment field and the two others are set as '=comment'. so altium will interpret this automatically ( like the magic strings '.designator' )

tip 12 . do NOT use slashes in part names. there is currently an issue with the path parser. if you create a diode  BZX87R5V1/198 altium cannot find it. reason being that , if the diode folder is /components/diodes/zeners .. the part ends up in /components/diodes/zeners/BZX87R5V1/198.schlib. the string does not get sanitized properly.

tip13 make sure there is more than one admin account. NEVER login using that account through altium. Web access only ! if altium crashes the sessions can lock up. if admin locks up .... you will have to reboot the server.

as for lifecycle : we use the built in one.
as for the stepping back : that is usefull when an update is done to a a parameter field that has no impact on the board. for example you spot that Vceo was set wrongly for a component. that has no impact on schematics nor pcb's. there is no need to retrigger the lifecycle manager. demote, fix it , promote.

[DarkPrince]

Enterprise vault user here. (200 + users / 10.000+ parts / split vault/oracle server).
Since i am the vault master i know pretty good how it works.( i set it up)

Our electrical department consists of... 4 people. In regard to board design, I am the main designer but we have someone in-training that may help out in the future. One other person usually does the reviews of the designs before we send out for manufacturing. So, not quite the scale you work at.

Tip 1 : make folders for Components, symbols and footprints.
tip 2 : make subfolders for categories. resistors, capacitors, ic, transistors.
tip 3 : for component folders only : make sub-sub folders. nmos pmos, zener , shottky , analog digital etc ... 0402 0603 0805 ... you get what i mean.

See attached image for our current structure which the first level within Manufacturer Components is the manufacturer name. It is <Manufacturer>/<Component Type>[/<Sub Component Type>], Models/(SYM/FTPK) created at the level deemed appropriate.

tip 4 : learn to use the templates and create template for each sub category. Set defaults in templates and force requirements of parameters from there
tip 5 : drive parameter visibility from the folders.
tip 6 : do not store anything in the symbols. it is useless. don't tie anything to footprints. Only set designator and description. drive comment field from the component.

I do plan on diving deep in the templates. Good tip on the parameter visibility, will use. And the dead-simple symbols was the plan, trying to reduce redundant work.

tip 7 : when creating pcb parts you will find out that often the description does not get loaded ( depending on how you create the part ) , or you have to enter it again on a secondary screen.
to create new parts make a local library for sch and pcb and link those to an incoming library in the vault. This allows you to avoid this problem. bonus is that any incoming part ends up in an invisible library so end user cannot use it unless it has gone through lifecycle ( new parts always come in 'from desingn' )

I am not quite sure I know what you mean here. I did a few tests (add to vault from new component file vs. add new from vault (fileless editing)) and both pulled descriptions fine it appeared.

tip8 : cloning is your friend. you can clone symbols, parts footprints. when cloning parts : you can clone symbols , footprints inside the parts editor as well. need to add 4 0805 resisots ? clone any 0805 , then simply click 'add' at the bottom to inject 3 more and release all at once. the grid can copy past straight from excel.

Will look into this. Thanks!

tip9 : resitrict the number of people the can edit / create vault parts. you need a librarian. you can allow people to create symbols and footprints but there should be a gatekeeper to take them into the vault and tie it together.

As stated, our department is small, so I am the board designer... and librarian... and everything else. Actually from what it sounds like you use files to start a new design in the vault rather than the "Create Component" command. Might be related to what you said above.

tip10 : when creating templates : use Manufacturer and Manufacturer PartNo as fields. nothing else !. the octopart integration triggers on those keywords. you get full blown integration for free that way.
tip 11 : altium is sensitive to keywords. that means you can use certain keywords as fieldnames. for example 'grouping' will directly trigger to the annotator process. we have a situation where we need to store our internal product code under 3 fields. Reason being that our internal PLM system (enovia) needs a keyword called 'TPN' to find the column. a life modeling tool (sherlock) uses its own field for crosslinking the database. and then we store the 'comment' field so that altium overrides the comment properly for the schematic symbol. inside the vault i simply set the comment field and the two others are set as '=comment'. so altium will interpret this automatically ( like the magic strings '.designator' )

Great! I just dug up some docs on this. Will take this approach to get the integration.

tip 12 . do NOT use slashes in part names. there is currently an issue with the path parser. if you create a diode  BZX87R5V1/198 altium cannot find it. reason being that , if the diode folder is /components/diodes/zeners .. the part ends up in /components/diodes/zeners/BZX87R5V1/198.schlib. the string does not get sanitized properly.

Good to know and avoided it in the past anyway. Glad to be on the right path here.

tip13 make sure there is more than one admin account. NEVER login using that account through altium. Web access only ! if altium crashes the sessions can lock up. if admin locks up .... you will have to reboot the server.

Thanks for the heads up. Being a small department I am an admin... and actually using it (had to even do licensing and server installation). I'll create a secondary account for Altium use then.

as for lifecycle : we use the built in one.
as for the stepping back : that is usefull when an update is done to a a parameter field that has no impact on the board. for example you spot that Vceo was set wrongly for a component. that has no impact on schematics nor pcb's. there is no need to retrigger the lifecycle manager. demote, fix it , promote.

I might be mis-understanding how Altium works but can you update an item without creating a new revision? From my poking every time a new revision is created it defaults back to New from Design. I feel I am missing something here.

I had this idea that from Pending Approval the design would either get Released (Approved) or Rejected (Rejected), and a new lowest-level revision would have to be created which would reset the lifecycle to Design (or whatever the first is). This way I can create a saved search and get a list of all items that the reviewer reviewed and didn't approve (state == Rejected). I am not sure how to do that with the Altium Lifecycles if their state just goes back to design.

I'll go back and check out the Altium defaults. They document what their examples are but do they document how they should be used?

FYI, I have both AD 16.1.12 and  17.0.11 installed currently (had issues during migration so currently have side-by-side installation).