Easiest way to manage PCB versions/revisions in Altium? - Page 1
Forum section: electronics / general

author: smoothVTer
author_rank: Regular Contributor
timestamp: December 10, 2016, 11:40:27 pm
content: ( Apologies if this has been answered here elsewhere; the words "version" and "revision" appear everywhere in search results on this forum )What is the simplest way to create Altium project versions / PCB revisions?For example, I created a project named myProject_V0.0. I want to do a PCB update where I'll move components around, delete some components, add some other components, and generally improve upon my V0.0 PCB. At first I tried to do what I do in Eagle: copy the entire project folder over and rename it ( myProject_V0.0 --> myProject_V0.1 ) and rename all associated files within the folder structure, but Altium complains then it cannot find the libraries associated with the project ( which are attached to / part of my original project V0.0 )I looked into Altium's built-in SVN system, version control & configurations; my eyes glaze over and my brain becomes numb with excessive complications and dozens of details. The documentation is mind-numbingly deep and seems like Altium's system for doing something like creating another PCB version is targeted for large companies where many engineers share documents, check-in and check-out files; the setup for doing so seems like very, very much overhead.So: Anyone out there care to share what's the quick-and-dirty method for creating V0.1, V0.2 etc of PCB's and schematic documents? The goals are:Start with some existing .PrjPcb project and all associated schematics/PCB and attached librariesCopy everything, but rename it under a different name, different folder namePreserve all library links and project settings such as stack up, design rules, etc.Be able to modify schematic/pcb, add/subtract from it, all without affecting the prior version

author: DerekG
author_rank: Frequent Contributor
timestamp: December 10, 2016, 11:54:10 pm
content: Quote from: smoothVTer on December 10, 2016, 11:40:27 pmJust open your existing schematic & rename it so you now have two schematics in your project. Then do the same with your pcb so you now have two pcbs in your project too.The other way is to avoid projects altogether. Just start your schematic as a "free file" & use this to generate your pcb (also as a "free file").

author: carljrb
author_rank: Contributor
timestamp: December 11, 2016, 04:44:09 am
content: I use SVN to version things, however I use TortoiseSVN for this instead of Altium's built-in tools.

author: technotronix
author_rank: Regular Contributor
timestamp: January 02, 2017, 02:43:56 pm
content: check this out. This may helpful.http://techdocs.altium.com/display/ADOH/Version+Control+and+Altium+Designer

author: IanJ
author_rank: Unknown
timestamp: January 09, 2017, 05:37:50 am
content: I have the same issue with CircuitStudio......I wish there was a 'duplicate and rename' project folder function.My own problem is that I sometimes use a particular project as a basis for a new project that isn't a 'version' necessarily of the one I am duplicating from.Just copying the pcb and sch files is fine but problems with paths start to occur when copying pcblib etc.Am previously a long term Eagle user.......so maybe that's the problem......😯Ian.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: January 09, 2017, 10:34:55 am
content: I don't understand why you would want libraries for each project... surely if you are building a "set" of projects as/for a single entity (your own company, an employer, etc) you want to build up one single library that always is up to date and correct rather than have compoenent libs sitting around everywhere in folders? and since altium sch and pcb files have all the component data anyway, you can always generate libraries for a project if you ever need to...anyway...I keep all design files (sch, pcb, outjob, etc) for a project together, and have them in a git repo. Then as I edit things I can check them in with descriptions of what I did and when, and tag the repo state for releases using a standard format tag..I can also zip up the folder as a "release snapshot" if I want, but git pretty much makes that unnecessary.I don't tend to rename files with version numbers in the filename, as that's really fiddly and unnecessary - but will update revision numbers inside the files. (ie the PCB file has a revision in it, schematic sheets do too)when I do a release, then all the output stuff (gerbers, BOM, schematic prints, pcb fab doc, assembly docs, 3d models, etc) goes into a standard directory structure in a suitably named/versioned folder inside my common "release packs" folder, and I use the outjob file for the project to make sure everything has the relevant version attached in its name. Then I check it all, zip up the folder with the release version in the zipfile name, and send it off..

author: IanJ
author_rank: Unknown
timestamp: January 09, 2017, 08:50:02 pm
content: Quote from: julianhigginson on January 09, 2017, 10:34:55 amI think I started to realize that after my 1st or 2nd project.........as a new user I had initially thought the .pcblib's went with the project and integrated libs were central. Thanks to this thread I think I'll sort that out........Ian.

author: free_electron
author_rank: Super Contributor
timestamp: January 12, 2017, 05:11:01 pm
content: rule 1 : NEVER EVER edit filenames OUTSIDE of altium !that being saidsimply copy the entire folder.rename the copy FOLDERopen the project in altium from the new folder.Save project as (note: save PROJECT as, not the normal 'save as') .give baby new name.done.for exampe a folder name myproject v1.0 inside is myproject v1.0.prjpcb and all the other files related to it.in windows :- copy folder- rename "copy of myproject v1.0" to "myproject v1.1'launch altium.open project : navigate to 'myproject v1.1 folder and open myproject v1.0.prjpcbsave project as myproject v1.1.prjpcbdone.no need for muckeryNEVER EVER alter filenames (apart from the prjpcb file) outside of altium. altium doesn't care what is in the directories. the links are stored in the prjpcb file. alter filenames ouside of altium and you break the links. this is done on purpose so you can store other data in the project directories that altium has no business with.There is no need to have libraries travel with a project. everything that is needed for a schematic or pcb is stored inside the schematic and pcb files.