Copying PCBs in Eagle - Page 1
Forum section: electronics / general

author: ocset
author_rank: Super Contributor
timestamp: March 24, 2018, 11:45:40 am
content: Hello,I have a product which comprises many different PCBs. I am laying them all out in the same windoww (.brd file). One of the PCBs must be duplicated. However, when i copy it and try to paste it back into the .brd file, it just tells me it cant be done, and says error message "cant back annotate..."Do you know how i can duplicate it and have it in the same .brd file?It saves me from laying out the board all over again.

author: ataradov
author_rank: Super Contributor
timestamp: March 24, 2018, 06:15:13 pm
content: You can't do this. This will create a situation where you have multiple components with the same reference designator. None of the internal Eagle structures support this.

author: Mattylad
author_rank: Regular Contributor
timestamp: March 24, 2018, 07:37:32 pm
content: Why?Why are you trying to copy it?Why are you doing all these in the same design file?

author: jpanhalt
author_rank: Super Contributor
timestamp: March 24, 2018, 07:49:21 pm
content: Not sure exactly what you are doing. Two possibilities for solving it:1) Copy the PCB you need and paste to anew file, blank .brd. Of course you may get the message about forward/backward compatibility, because there is no schematic to match it. Device names will change from whatever they were to start at "1." For example, R10 may become R1 and so forth.2) Eagle has a panelize function that lets you put multiple instances of a PCB on a single PCBwithoutrenumbering.Above comments apply to versions <8.0

author: KL27x
author_rank: Super Contributor
timestamp: March 25, 2018, 02:52:32 am
content: Jpanhalt seems to know Eagle better than I. But there is another way you can do this, where you simply "break annotation." So this is only to be done if you want to panelize a Gerber, for instance. And this is what it sounds like you want to do.Breaking annotation is as easy as closing the schematic window. A banner will appear in the PCB view window saying "ANNOTATION BROKEN!" Then you can copy and paste all you want. But you will no longer have a schematic linked to this board, and YOU CANNOT UNDO THIS AFAIK. (I'm surprised more people haven't done this accidentally at some point, and learned this the hard way). So make sure you save this to a new .brd file. If you need to make anything but minor tweaks in the future (or debug a problem with the board), you have to go back to the original .brd and do the work there, and copy and paste, again. Without a schematic, you can't do signal routing for instance. Or ERC check. Etc.

author: jpanhalt
author_rank: Super Contributor
timestamp: March 25, 2018, 09:35:56 am
content: @KL27xAh yes, closing the schematic is always an option. That is a little like amputating something to prevent cancer. It works, but can be very hard to reverse.It is my method of choice when I want to get rid of a pesky via -- the one you add to the board but can't delete. You get the message to do it on the schematic, but look as you may, they are hard to find. Closing the schematic eliminates that problem. Then when you re-open the schematic all is well, unless you were so overjoyed with that success that you changed a component or something.

author: westfw
author_rank: Super Contributor
timestamp: March 25, 2018, 09:52:59 am
content: Pesky vias should be "ripped up" rather than deleted.

author: KL27x
author_rank: Super Contributor
timestamp: March 26, 2018, 08:48:45 am
content: ^yep.QuoteYou do not have to put vias in your schematic, at all. To stitch up planes, you can drop a via into the PCB and then rename the net to connect it to your pours/polygons. Then you can even copypasta this via and sprinkle it wherever you want. For connecting signals, you can let signal-routing create them by changing from top copper to bottom copper or vice-versa while routing, et voila, the via appears. And they will not clutter up your schematic. Perhaps you have created some this way (and perhaps you should start creating all of them this way!), and that's why you can't find them. Once a via is created in these ways (and connected by renaming the nets, in the former example), it is essentially considered a piece of routed trace. When you try to delete it, and it refers you to delete it in the schematic, it thinks you are trying to delete this signal, entirely. The via is not in your schematic; you would have to delete/break the signal/connection wire in the schematic to remove the via (along with the rest of the traces you have routed for that signal), when what you really want to do is "rip up" just the via in the PCB window, same as you would a trace.I can imagine how badly you wish you knew this, before.

author: jpanhalt
author_rank: Super Contributor
timestamp: March 26, 2018, 11:45:10 am
content: I knew vias are not on the schematic (usually). I was being tongue in cheek, which was related to the Eagle message. And yes, I know they can be removed with ripup. It is often easier for me to do it by closing the schematic. No harm, no foul and often quicker.

author: KL27x
author_rank: Super Contributor
timestamp: March 27, 2018, 12:12:04 am
content: ^ Oh.That is interesting. I'll have to play around with it to see if it can be useful. So far, deleting one via while the schematic is closed, then opening it, again and rerouting that signal caused 3 ERC errors.QuoteThe only issue I can guess is when ripping up a via, it always rips up another section of trace, too. Logically, I suppose this is because eliminating just the via leaves nowhere to show this break in the trace, since we view the unrouted signals in only the X and Y axis.I can afford to save a lot more time with Eagle. I suck. Maybe one day I'll learn where to use this trick. Thanks.

author: westfw
author_rank: Super Contributor
timestamp: March 27, 2018, 08:07:03 am
content: QuoteNo it doesn't. If you're careful to select just the via (possibly using right-click), then only the via is removed. It'll leave a big "X" at the spot if the bottom and top layers are connected by a zero-length airwire:

author: KL27x
author_rank: Super Contributor
timestamp: March 27, 2018, 08:22:34 pm
content: Thanks for the correction.I had just done the delete thing. I suppose this is an issue with deleting a via. when you delete it and reopen the schematic, you can't necessarily see the break in the trace. There's no X on there.But OTOH, my memory is nagging at me and has convinced me there are some instances where ripping up a via unintentionally removes routed traces. I seem to recall getting into such situations and end up resorting to rerouting a section of trace, redundantly.

author: westfw
author_rank: Super Contributor
timestamp: March 28, 2018, 01:24:04 am
content: QuoteIt IS pretty easy to accidentally rip up a trace when you're aiming for a via (or another segment of a trace.) And if you rip up part of a trace and mean to rip up the via next, but accidentally hit the airwire, it will rip up the entire signal up to the next pad.This is one of the cases where it pays to have "undo" mapped to ctrl-Z (or whatever.) EAGLE's "undo/redo" is very handy!

author: ocset
author_rank: Super Contributor
timestamp: March 29, 2018, 05:08:54 am
content: Thanks all, Eagle is the best, i hope i dont loose my version 7 licence as i hear you have to pay yearly to use Eagle now its owned by Autodesk. If i do have to buy it new again, i hope Autodesk dont change Eagle.I mean, i think "the_other_package_thats_widely_regarded_as_the_best_-you_know_the_one_i_mean" is great but you have to almost have the intellect of a computer hacker (or know the right people), to be able to use all its wonderful features.

author: westfw
author_rank: Super Contributor
timestamp: March 29, 2018, 06:18:16 am
content: QuoteYeah; they've gone to a "subscription model." It's actually not too awful; the same price you would have paid for for a particular version will get you several years worth of subscription, and they seem open to doing things like converting people from "hobbyist" to "pro" for the short duration of a commercial product...

author: ocset
author_rank: Super Contributor
timestamp: March 30, 2018, 06:54:38 pm
content: Thanks, but i think its a disaster, as i hear you cant use it unless your online..........try being online on any British Train.

author: jpanhalt
author_rank: Super Contributor
timestamp: March 30, 2018, 07:59:14 pm
content: @FlybackDownload an earlier free version. On-line not needed. I use 7.2 and 7.7 roughly interchangeably. Been using it since 3.x. A few quirks, maybe yes. But for being free of hassles, not having to be on-line, and very powerful, it does the job.My recommendations, posted well earlier, should still work with 8.x.

author: ebastler
author_rank: Super Contributor
timestamp: March 30, 2018, 08:16:56 pm
content: Quote from: treez on March 30, 2018, 06:54:38 pmYoucanuse Eagle without being online. It wants to phone home at least once a month, I believe, to check that your subscription is still valid.If you have to spend more than one month on end on board of a train (British or elsewhere), you probably have other problems than Eagle connectivity...

author: ar__systems
author_rank: Frequent Contributor
timestamp: April 03, 2018, 11:54:18 am
content: Yes, you can do this. However you need to copy-paste board and schematics independently. In other words:1. Open the source PCB.2. Copy the board. It is better to copy entire board. You can remove unneeded elements later.3. Open the target PCB file. Make sure to close target SCH file.4. Paste the board into target.5. Open source sch6. copy the schematics. Again - entire schematics7 open target sch. close target .brd8 paste the schematicsNow you can open the BRD and check for consistency. If you did everything correctly, you should end up with a consistent board now.

author: ocset
author_rank: Super Contributor
timestamp: April 21, 2018, 09:45:20 am
content: QuoteThanks but i cant seem to do it.Well, i ended up doing it , but ended up with the board and schem not being consistent.The attached are the concerned Eagle files.We want the pcb of file "two" to be pasted into file "one"

author: jpanhalt
author_rank: Super Contributor
timestamp: April 21, 2018, 10:33:32 am
content: It is not that hard. When you do a copy/cut and paste, do you have all layers shown? Have you practiced on something a little less complex? After you paste the second schematic, do you do an ERC?

author: ocset
author_rank: Super Contributor
timestamp: April 21, 2018, 11:15:17 am
content: Thanks, yes i had all layers shown...it fails the ERC.I am beginning to think this cannot be possible, because how would equivalence between scm and brd be maintained if a section of circuitry suddenly comes into the brd file.

author: jpanhalt
author_rank: Super Contributor
timestamp: April 21, 2018, 11:19:20 am
content: Hi Treez,Had a little bit of time to waste, so I made the attached file. That should include the single board and schematic and the combined. It is a very old design of mine for which I made a DIY board and did not pay particular attention to overlaps and other messages. Nevertheless, the combined schematic and board are consistent.One added detail, when you paste, nets such as VDD and GND will receive new names like VDD1 and GND1 on the pasted schematic. You will probably want to go to the combined schematic and rename them the same. That will create the appropriate airwires on the board that you can then route or ignore at your pleasure.John

author: jpanhalt
author_rank: Super Contributor
timestamp: April 22, 2018, 09:55:58 am
content: @treezAny update?

author: ocset
author_rank: Super Contributor
timestamp: April 22, 2018, 11:59:11 am
content: Hello John,Wow!Thankyou very much indeed!Great of you to do this.This is fantastic, just what was needed!Kind Regards,Andy

author: westfw
author_rank: Super Contributor
timestamp: April 22, 2018, 09:05:44 pm
content: The new versions of eagle seem to have some features aimed at doing this. "Design blocks"?