Elecrow covers vias with solder mask?! - Page 1
Forum section: electronics / general

author: MagicSmoker
author_rank: Super Contributor
timestamp: October 29, 2016, 11:59:46 am
content: So I finally gave in to the dark side and ordered a 2-layer board of a known-good design from Elecrow. I used their recommended EAGLE cam file to create the Gerbers, sent them off and about a week later received the boards. The board quality looked decent on initial inspection, so I assembled one and proceeded with testing. It worked fine, so no shorted or opened traces, but I was having a difficult time scoping signals from vias that do double-duty as scope probe test points on my boards. Upon closer inspection I saw that the vias were covered with solder mask?!? That's a first for me... I hope this is an error/defect on their part, and not something they do by default because otherwise the board quality and service was good.EDIT: just for reference, square vias go to common/ground on my boards while round with a silkscreened circle around them are for signals/power rails.

author: zapta
author_rank: Super Contributor
timestamp: October 29, 2016, 12:14:03 pm
content: It's depends on the eagle design that you used. If it has covered vias that electro will cover them.IIRC, there is in eagle's settings a 'limit' value that control via covering. If you set it for example to 20 mils, vias with drill less/equals 20 mils will be covered with mask and larger one will not. I presume that if you set it to 0 eagle will generate non covered vias for you.Edit: this is the settinghttps://farm3.staticflickr.com/2906/14238175172_7e68aa337e_z.jpg

author: wraper
author_rank: Unknown
timestamp: October 29, 2016, 12:33:21 pm
content: Have you checked your gerbers if vias aren't covered there?http://www.gerber-viewer.com/

author: DerekG
author_rank: Frequent Contributor
timestamp: October 29, 2016, 01:06:45 pm
content: Quote from: MagicSmoker on October 29, 2016, 11:59:46 amI have had a similar experience with PCBWAY. The prototypes came back with the vias open as expected, whereas the production quantity came back with solder mask covering the vias.I prefer open vias as it makes it easier to fault find the boards plus the holes (0.8mm in my case) usually fill OK when wave soldered. This adds to the current carrying capacity of the vias themselves which is handy if the plating is too thin.If you cover the top side of the via with solder mask, an air trap forms which prevents the wave soldering from properly filling the via.

author: Andreas
author_rank: Super Contributor
timestamp: October 29, 2016, 02:49:10 pm
content: Hello,I think it depends on the hole size.My vias with 32 mils for the hole are all open on the PCB.Although in stop mask they are closed.I also think it would give a mess if they would paint the large holes.The small holes are probably no issue if they are painted.Some manufacturers use a dry film for the stop mask.In this case they can close the large holes.With best regardsAndreas

author: MagicSmoker
author_rank: Super Contributor
timestamp: October 29, 2016, 03:14:29 pm
content: Quote from: zapta on October 29, 2016, 12:14:03 pmThis was it. The Elecrow design rule file changes the minimum drill size to get an opening in the solder mask to 100mils! The same setting in my design rule file is 20 mils.So I guess they made the board correctly, it just isn't what I wanted. I changed the setting and will re-order the board; if the vias are still getting covered THEN I will go medieval on them.

author: matseng
author_rank: Frequent Contributor
timestamp: October 29, 2016, 04:34:21 pm
content: You're not checking the gerbers with a gerber viewer after generating them?I would never dream of sending for pcbs without spending a minute or two making sure that the gerbers seems reasonable. Either with the plain old gerbv or with one of new new cool 3d-viewers. I've more than once discovered (minor) issues that I've corrected before actually sending them off for manufacturing.

author: MagicSmoker
author_rank: Super Contributor
timestamp: October 29, 2016, 06:18:12 pm
content: Quote from: matseng on October 29, 2016, 04:34:21 pmYes, I checked the Gerbers* and did not notice anything was wrong. Probably for the same reason that authors still need editors to proofread what they wrote.Let's not be too quick to judge here.* - EDIT- I use ViewMate to check Gerber files, even though I don't much like it.

author: zapta
author_rank: Super Contributor
timestamp: October 29, 2016, 07:12:04 pm
content: Quote from: MagicSmoker on October 29, 2016, 06:18:12 pmYou can use oshpark as an eagle pcb design viewer. Just upload the .brd file and it will show you how the various layer will look.

author: matseng
author_rank: Frequent Contributor
timestamp: October 30, 2016, 06:43:04 am
content: Quote from: zapta on October 29, 2016, 07:12:04 pmThat's really not a good idea - since then some .cam and .dru files will be applied by them at a later stage and you won't be in control of how you want the pcb to end up. Always generate the gerbers yourself, check the gerbers with a local or online viewer, zip them and upload to the boardhouse. Or else you have "outsourced" too much of the process.

author: zapta
author_rank: Super Contributor
timestamp: October 30, 2016, 02:05:48 pm
content: Quote from: matseng on October 30, 2016, 06:43:04 amI always order from oshpark using .brd files and never had a problem. Same with oshstencils.Is your concern based on actual bad experience with oshpark?

author: Farley
author_rank: Regular Contributor
timestamp: October 30, 2016, 02:34:44 pm
content: I don't believe matseng is deriding OSH Park or OSH Stencils (I've had excellent service from both places, btw). I think he is pointing out that giving any third party control over your output files might lead to unexpected results.Once I generate Gerbers and drill files, and check them in a viewer (I use gerbv), I then have a definite expectation of the results I should get when I receive the PCBs.

author: matseng
author_rank: Frequent Contributor
timestamp: October 30, 2016, 03:31:31 pm
content: Exactly... I don't have any experience at all with OSH Park. It was just a general observation that if you want to know what is actually is do be manufactured then you should generate the Gerber's yourself - and check them.It's not hard to generate Gerber's, and if you care about your work and the end product I'd say it's a required step in the process of going from idea to pcb.

author: zapta
author_rank: Super Contributor
timestamp: October 30, 2016, 03:55:13 pm
content: Quote from: matseng on October 30, 2016, 03:31:31 pmOk, thanks for clarifying, since your answer was in the context of oshpark.If you will try to upload .brd files to oshpark or oshstencils you will realize that they allow you to review their interpretation of that .brd file before you place the order. This is even safer than uploading gerbers blindly and not being able to see the vendor's interpretation of those gerbers.

author: matseng
author_rank: Frequent Contributor
timestamp: October 30, 2016, 04:30:20 pm
content: Well, you can hope that they will use exactly the same cam/dru files in both the viewer and the real generator. And they probably are, but by no means this is for 100% certain for all times.Giving them Gerber's on the other hand is almost 100% certain since no conversation or interpretation of rules is ever necessary since this is the standardized format all fabs are actually using.If you say that sending a brd file is safer than sending Gerber's then you're simply wrong....

author: zapta
author_rank: Super Contributor
timestamp: October 30, 2016, 04:57:14 pm
content: Quote from: matseng on October 30, 2016, 04:30:20 pmSending the .brd files and reviewing the vendor interpretation of the files using the vendor tools vs. reviewing gerbers file with a third party tool and not seeing the vendor's interoperation of the files. Yes, in this scenario .brd is safer.

author: timb
author_rank: Super Contributor
timestamp: October 30, 2016, 09:25:47 pm
content: Quote from: zapta on October 30, 2016, 04:57:14 pmOr, you could review the Gerbers with a viewer, then upload them to OSHPark and review them there as well... That seems *even safer* to me.The way OSHPark generates previews (from Eagle, KiCad *or* Gerbers/NC Drill files) *is* nice, yes. However, the images are generally low resolution and can't be zoomed into, so you lose a lot of the detail. On a bigger (or denser) board, it's certainly not enough to check for a lot of clearance issues.Their previews are designed for you to verify they were able to read the files you upload (that is, the various layers are--at a minimum--present). Beyond that, it's up to you to verify the Gerbers exported from your tool correctly using a Gerber viewer!So, you're always better off exporting your own Gerbers, checking them in a viewer, then uploading them (where, if applicable, another basic visual verification can be performed).Period.

author: zapta
author_rank: Super Contributor
timestamp: November 01, 2016, 04:27:10 am
content: Quote from: timb on October 30, 2016, 09:25:47 pmQuestion mark at most.