What is the point of Rooms in Altium (+ updating schematics) - Page 1
Forum section: electronics / general

author: Random Model Maker
author_rank: Regular Contributor
timestamp: June 05, 2018, 09:39:56 am
content: Hello you much wiser people than me,First of all the usual disclaimer, I am sorry if this has been asked before, I could not find it through the search functions (at least in this forum).Now to my question: I am (maybe notthat) new to Altium, but I am a self-taught bumbling idiotwho finds out about all the wonderful features through youtube videos, really as I go along.What I see always pop into existence when I go to start on a new PCB is that the components appear on these Rooms, which particularly annoys me if I add several components to an ongoing design and when I drag them on the bave to change ioard all at once, the already placed components wander off into the rhubarb.After my search I noticed those Rooms must be a feature most likely present on more than just my copy of Altium, and they must have some very important purpose; still I do not get the primary idea, what they are good for, if I need them, or if I have been doing something horribly wrong by instantly deleting them as soon as they appear.Another question: I was just making a new net class what for pin swapping, and when I went to update the schematic, it would not want to take over my class from the PCB back to the schematic and give me the message "check project options". I however could not find the necessary option to allow me updating the schematic, and when I want to import changes to the PCB, it always wants to delete my class. Does anyone know off the top of their head what I would need to change in the options?Many Thanks to all of you

author: Mikekoz13
author_rank: Contributor
timestamp: June 05, 2018, 11:58:44 am
content: Rooms will allow a repeated circuit to be dealt with more quickly and easily. For instance, if you have the same circuit repeated 10 times, and you created your schematic correctly, each circuit will be placed in it's own individual room when you capture the schematic to the PcbDoc. Then you can place and route one of the 10 circuits and once done copy that placement and routing to the other 9 circuits in just moments.As to your newly added components ripping up other components and moving them.... look at your Component Links. They are broken.

author: Random Model Maker
author_rank: Regular Contributor
timestamp: June 05, 2018, 12:11:51 pm
content: That's interesting, could have saved me a lot of time in the past.Now I just need to find out how to design my schematic properly, as you say. I presume copying and pasting to 10 different sheets is not that?Not sure what exactly component links are and how I broke them, but when I move a Room, all components move with it, which happens a lot if you drag select a lot of components. I know that it's a feature, but it gets really annoying if you don't want to.

author: Berni
author_rank: Super Contributor
timestamp: June 05, 2018, 12:19:26 pm
content: Yep copypasting the same layout is the main use for it:Here is how you do it.https://www.altium.com/documentation/18.0/display/ADES/((Multi-Sheet+and+Multi-Channel+Design))_ADBasically when you want to duplicate it you just put it all in a sheet and then bring multiple instances of that sheet into your design using sheet symbols. I tend to use sheet symbols in all designs that span more than one schematic page.EDIT: And yes if you don't need this automatic layout copypasting functionality then turn the rooms off as they have very little use beyond that.

author: Psi
author_rank: Super Contributor
timestamp: June 05, 2018, 12:25:31 pm
content: Rooms are there to annoy you, kill them immediately and turn off the automatic generation.

author: Random Model Maker
author_rank: Regular Contributor
timestamp: June 05, 2018, 12:32:12 pm
content: Quote from: Berni on June 05, 2018, 12:19:26 pmThank you very muchQuote from: Psi on June 05, 2018, 12:25:31 pmMy thinking, but there is always the lingering danger of bumblefuckery over my head.So my main concern, that I cannot correctly design a PCB without the Rooms, is unwarranted then.

author: ajb
author_rank: Super Contributor
timestamp: June 05, 2018, 02:38:35 pm
content: You can also use rooms to drive design rules (for example, creating rules that only apply in a BGA fanout area or something). One thing that makes them slightly less annoying is to change the display to "Draft" under View Options, that removes the fill and makes them just an outline, so they don't obscure everything under them. Do the same thing for 3D bodies as well. But yeah, generally they're more annoying than helpful unless you're doing a multichannel design. You can turn off room generation on a per-sheet basis by going to Project Options -> Class Generation.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 05, 2018, 07:20:52 pm
content: Always amused when I pick up an old design where the rooms have clearly been deleted in anger...The creator didn't know you go to Project Options, Classes and tick them off in there.Tim

author: Psi
author_rank: Super Contributor
timestamp: June 06, 2018, 10:47:04 am
content: Quote from: T3sl4co1l on June 05, 2018, 07:20:52 pmhaha yeah,or when you come across a project where someone has carefully moved all the rooms away from the PCB and you discover them hiding somewhere.

author: Gibson486
author_rank: Frequent Contributor
timestamp: June 11, 2018, 11:59:32 pm
content: I had a design with 18 repeated circuits (double sided too). Rooms was AWESOME! When i found out you could apply rooms to traces as well, my life was complete!

author: Berni
author_rank: Super Contributor
timestamp: June 12, 2018, 05:06:03 am
content: In my early days of Altium i had got rid of rooms so that i set the room to keep components outside and then deleted it. On the next schematic update it would put the room back but it was all the way in the bottom left corner out of the way where its difficult to even select it. Crude but it worked.It would make sense that Altium would only enable rooms by default if it was a multichannel schematic design. There is no reason to have that room if your entire design is a single schematic page. Like literally zero use, if you wanted to apply special rules to part of the board then you would need to manually make a new room anyway.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 12, 2018, 09:11:21 am
content: I suppose there might be some regional settings you could use for layout objects, whereas InComponentClass only affects components.You can also make polygonal rooms, which would allow you to apply such settings in regions much like the old timey boards where each functional block is demarcated and labeled, and some potentially have different rules.You'd still have to set net classes and rules specifically for things like clearance and width. I'm not sure how much good this can actually do.Hmm, I've used regional exceptions on rare occasion -- example, making an exception for adjacent or NC pins in a fine-pitch device that handles high voltages -- I wonder if these can be done by room instead. And also that the custom room used isn't going to be removed on update.Tim

author: julianhigginson
author_rank: Frequent Contributor
timestamp: June 12, 2018, 11:50:01 am
content: I like rooms, but have to admit my normal treatment of the room for a project's base schematic is to set it to "all components outside" and shove it down the bottom left of the PCB area... This is because normally my base schematic contains all the board's connectors and user-level parts, and works as a kind of top level overview of the design. So as a result the base schematic sheet has parts that are placed all over the board... And if a room covers everything, it may as well cover nothing.It'd be less necessary to get rid of the base room if the rooms feature was a bit more polished though. particularly around being able to select different rooms that are overlapped on the same layer.

author: Random Model Maker
author_rank: Regular Contributor
timestamp: June 12, 2018, 01:58:41 pm
content: Quick question, if I wanted to pass an entire bus from one schematic to another, no hierarchy, just a flat design, is that possible and how would it be done? (AD16 btw).There is no multi channel thing going on, just a way crowded schematic.Do I have to name the nets going into the bus consecutively (ie net1, net2...) or can I name them the way I want?So far I have used buses with non-consecutive names with great success, as well as ports, power ports etc. to link my schematics.My obviously dumb approach of plugging a bus into a port did not work (worth a try though)

author: ajb
author_rank: Super Contributor
timestamp: June 12, 2018, 07:58:31 pm
content: Wow, are there that many people just shoving the rooms off to the side of their PCBs?Project -> Project Options -> Class Generation tab -> Uncheck "Generate Rooms"(I'll admit that I'll often delete the same rooms over and over again, but every time I think "I need to turn those rooms off--I'll do that right after I just..." and then I forget all about it until the next sch->PCB push)Even on multichannel designs I tend to eventually delete the rooms once I'm 90-95% done the layout, since it makes it easier to do the final layout tweaks.Quote from: T3sl4co1l on June 12, 2018, 09:11:21 amThis is the problem I couldn't get around when I experimented with this a while ago. It seems that you basically have to create a sheet specifically for the sake of generating the room, which forces you to organize your schematic so that only the parts that should be placed within the special rule area are in that sheet. In my case, I was trying to use a room to create rules for fanning out a QFN, so I had a room with just that IC and it's handful of supporting passives, which was kind of pointless. For a big FPGA or something it would probably make more sense, but once I got it to work it still wasn't worth the trouble of dealing with a room for my experiment. I haven't tried using regions for rules, that seems like a better idea since it decouples the rule area from the structure of the schematics.

author: D3f1ant
author_rank: Frequent Contributor
timestamp: June 14, 2018, 08:06:27 pm
content: Project -> Project Options -> Class Generation tab -> Uncheck "Generate Rooms"This is the correct way to disbable room generation when it's not required. If we all email AD support maybe they will turn it off by default, and automatically turn it on only when required.

author: Psi
author_rank: Super Contributor
timestamp: June 15, 2018, 12:40:42 pm
content: Quote from: D3f1ant on June 14, 2018, 08:06:27 pmhaha, they'd probably remove the option to disable it.

author: Gerhard_dk4xp
author_rank: Frequent Contributor
timestamp: June 15, 2018, 01:58:44 pm
content: Rooms can be extremely helpful.<https://www.flickr.com/photos/137684711@N07/41004659340/in/dateposted-public/><https://www.flickr.com/photos/137684711@N07/40883730542/in/album-72157662535945536/><https://www.flickr.com/photos/137684711@N07/26052800387/in/album-72157662535945536/>(amplifier with 20 parallel input stages for lower voltage noise)regards, Gerhard

author: free_electron
author_rank: Super Contributor
timestamp: June 15, 2018, 02:38:30 pm
content: rooms are used to partition your layout and group blocks.the default mode is to create a room per page.but you can control your own room creation as well through blankets and directives.i typically do the layout of a block , size the room to contain everything. that makes it easy if i need to move that block later on. everything is contained in it.

author: DutchGert
author_rank: Frequent Contributor
timestamp: June 28, 2018, 08:02:02 pm
content: The standard rooms generated per page are anoying so usually i turn those off but I do use rooms to enforce specific design rules in certain parts of the board.for example: a room called "BGA" under your bga's so you can set your track or polygon clearance under the BGA just a bit tighter then the rest of the board.