Eagle newbie, please review - Page 1
Forum section: electronics / general

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 03, 2014, 07:15:56 pm
content: Rather than try to layout my own board from scratch (which I have never done before), I decided to modify an existing through-hole (open source hardware) design from blinkstick.com and try to get a compact SMT board. The goal is as tiny a board as possible, which will mimic a standard USB connector once covered with a few layers of heatshrink sleeve.I am pretty happy with what I have now, but Eagle is complaining about various clearance issues. Could a kind soul please help improve the design so that it can be submitted for prototype production?1) Are the clearance issues really an issue in practice (production) or the default clearance rules simply too strict?2) I have been advised to do a ground flood fill, but I am not sure how to do that?!3) Are vias under components going to be a problem, or is this common practice?4) How do I pack as many as possible on a board (say 5cm x 5cm on seedstudio.com) and make it easy to cut them out?5) I've seen part sourcing and board prototying done through Eagle/element14, is that any good? I was considering sourcing myself and ordering boards from seedstudio.com.Any comments/feedback appreciated.

author: Mr.B
author_rank: Unknown
timestamp: December 03, 2014, 07:51:18 pm
content: First up... Are you validating against SeeedStudios design rules if you intend to use SeeedStudio?From their site, download SeeedStudio_DRU_no_angle_20130527.dru or the latest version.In the section of your PCB shown below, there is plenty of room to move that via to get more clearance.There are a bunch of such examples on your board that are easily solved.To try to answer your questions:1. Yes it is an issue. The PCB manufacturer can only achieve certain tolerances. You need to download or create the Design Rules file for the particular manufacturer.2.http://dangerousprototypes.com/2012/07/18/eagle-polygons/3. No problems.4. SeeedStudio recently introduced an option for "panellising". They will be able to lay up multiple on one board. You will need to tell them how far apart you want them... i.e. the width of your scroll saw.5. I have only ever sourced myself and then had the PCBs done at SeeedStudio. I think the whole Source and Build process offered by Element14 and even Seeed are only any use when you have a decent volume, so it depends upon how many you intend to make. You will need to calculate out the economics yourself.

author: Mr.B
author_rank: Unknown
timestamp: December 03, 2014, 08:44:10 pm
content: My 5 minute improvement attached.Could do with a bit more of a tidy up though...

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 03, 2014, 08:44:59 pm
content: Thanks for the feedback Mr. B. I definitely want to validate against SeedStudio, thanks for that tip!Can I assume the SeedStudio rules are these I found on GitHub:https://github.com/lpatiny/legoino/blob/master/eagle/other/Fusion%20eagle/SeeedStudio_DRU_no_angle_20130527.dru

author: Mr.B
author_rank: Unknown
timestamp: December 03, 2014, 08:49:54 pm
content: Their latest one attached...

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 03, 2014, 08:51:11 pm
content: Quote from: Mr.B on December 03, 2014, 08:44:10 pmAwesome... except for one tiny detail, my Eagle (light) complaints about layer 2 and 15 not being available. I believe only layer 1 and 16 are available in the light edition?!

author: Mr.B
author_rank: Unknown
timestamp: December 03, 2014, 09:04:12 pm
content: Oops, sorry.I am not 100% sure about this because I don't have the light version to test it, but try this...Open the brd file in a text editor.Line 12 should be: <layer number="2" name="Route2" color="1" fill="3" visible="no" active="yes"/>Line 25 should be: <layer number="15" name="Route15" color="4" fill="6" visible="no" active="yes"/>In both cases change active="yes" to be active="no"As I say, untested.However I have manually manipulated other items in these files before without problems.

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 03, 2014, 09:24:37 pm
content: Yeah that worked.I applied the design rules you linked to, and running DRC now results in "9 approved errors"... clearance errors. I assume since this is not flagged as errors, an "approved error" is to be taken as a warning? I guess I will try to submit it to SeeedStudio soon. Thanks for the assistance.

author: Mr.B
author_rank: Unknown
timestamp: December 03, 2014, 09:30:14 pm
content: I approved those errors.One is the track at the top of the board that is too close to the edge, but it should be OK.The others are the footprint of the USB connector:Mounting holes too close to the edge of the board, but they should be OK.The D+ and D- pads are too close together according to the rules, but they should be OK as well.Also, make sure you use SeeedStudios CAM file to create your gerber files.Double check, no, triple check your gerbers... Once it goes to SeeedStudio it is too late.I use GerbView to check mine but there are numerous gerber viewers out there.Cheers

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 04, 2014, 06:39:23 am
content: I think I may have successfully generated the gerbers, although I am not sure about the drill holes which are not visible in Gerbv when I check it. Apparently this is a common newbie mistake (http://liudr.wordpress.com/2012/12/22/ordering-pcb-from-seeedstudio/) but all I can verify is that the .txt file indeed do have some drill data in it. Does everything look ok for PCB manufacturing? I realize there WILL be mistakes/tweaks to be done to any first production, but just trying to avoid rookie mistakes here.

author: Mr.B
author_rank: Unknown
timestamp: December 04, 2014, 07:13:20 pm
content: There is something very wrong with your drill file. (txt).The holesarevisible in Gerbv... It is just that they are not on your board.Have you used the latest "Seeed Gerber Generator" file?On this page:http://support.seeedstudio.com/knowledgebase/articles/422482-fusion-pcb-order-submission-guidelines

author: H.O
author_rank: Frequent Contributor
timestamp: December 05, 2014, 06:49:21 am
content: Hi,If you've used their CAM file for Eagle then you should be fine - and human eyes will look at the file(s) before it goes to production so if there's something seriously wrong with it it's highly likely it'll get picked up.As for why it doesn't display correctly in Gerbv.....I don't know that software (and honestly not that much about Gerber formats) but make sure that the format of the CAM output file matches what Gerbv is set to. I use Viewplot to verify my Gerbers and I need to change the expected format (number of decimal places) of the drill file to make it display correct, if I don't I get similar results to what is seen in the previous screenshot.

author: casper.bang
author_rank: Frequent Contributor
timestamp: December 09, 2014, 07:01:22 am
content: Ok a final thanks you guys for valuable help to this newbie. Pretty sure I succeeded in fixing that last drill file issue, caused by Eagle NOT using "GERBER_RS274X" as Output Device for the very first DrillsHoles pane (all other panes were using this Output Device). Now Gerbv displays the board more correctly. I've sent the order to SeeedStudio, not really expecting perfection to come back, but at $10 it's a cheap way to get some practical experiences.

author: Armadillo
author_rank: Super Contributor
timestamp: January 05, 2015, 01:53:55 am
content: Quote from: Mr.B on December 03, 2014, 09:30:14 pmThere are bugs in the SeeedStudio cam file [Seeed_Gerber_Generater_2-layer dated 27 March 2013], be careful with it because it treats layer 51  as Top layer traces creating shorted connections. At the moment, it would be best to use the sparkfun cam file.Cheers..

author: kizzap
author_rank: Unknown
timestamp: January 05, 2015, 02:19:17 am
content: Quote from: Armadillo on January 05, 2015, 01:53:55 amNot a hard fix really...go to the top copper tab in the cam and deselect the layer that is throwing up the fault. Personally I would be checking on all Cams that only the layers you want to be sent out are infact sent out.

author: Mr.B
author_rank: Unknown
timestamp: January 05, 2015, 02:29:00 am
content: Quote from: kizzap on January 05, 2015, 02:19:17 amYip... Always check what you are outputting.And... like I said above... Double check, no, triple check your gerbers.

author: casper.bang
author_rank: Frequent Contributor
timestamp: January 05, 2015, 07:07:21 am
content: Guys, I am of course all for checking... double-checking... and triple-checking. The thing is, unless you know the pitfalls and what exactly to CHECK FOR, it doesn't matter how many times I review the output in some arbitrary rendering utility. The PCB's have been produced and delivered, whether or not they stand up to the test of performing correctly after having components soldered on is the next step.