OSH Park !Sucks, my design sucks! - Page 1
Forum section: electronics / projects

author: blueskull
author_rank: Unknown
timestamp: January 09, 2015, 12:55:49 am
content: I laid out a board using Altium Designer 14.3, and I exported all gerber and NC files. I then uploaded all files to OSH Park as a zip file, and I got the following render image.When I got the actual boards, they don't appear exactly like the render image.Firstly, the internal cutouts are not as flat and sharp as a quality fab's product. The cut out looks like rounded rectangle, rather than a real rectangle.Secondly, all vias I used was treated as pads, which have NO solder mask at all. This is really a pain in the ass, because I have some vias in close vicinity of SMD pads, and having no solder mask can lead to solder leaking into vias, then leading to unreliable and faulty solder joints.Other than that, I will say, frankly, OSH Park is really a good fab, especially for budget makers like me.

author: c4757p
author_rank: Super Contributor
timestamp: January 09, 2015, 12:59:23 am
content: Quote from: blueskull on January 09, 2015, 12:55:49 amThe routing bits aren't infinitely narrow? Oh no!Did youaskwhat size they were? Or did you just assume they'd be perfect for your application without specifying?Edit:Ten seconds on Googlesays 100mil diameter - those look about right for that.QuoteThe render shows this, you ninny. You screwed it up when you exported the Gerbers. They don't change that.QuoteBut they "Suck!", right?

author: Nerull
author_rank: Frequent Contributor
timestamp: January 09, 2015, 01:01:45 am
content: Quote from: blueskull on January 09, 2015, 12:55:49 amSince many other OSHPark boards have solder mask over vias and your rendered image does not show solder mask over vias it seems like the problem was with your gerbers. They made what youaskedthem to make, which is not necessarily what youwantedthem to make, but that's manufacturing for you.

author: poorchava
author_rank: Super Contributor
timestamp: January 09, 2015, 01:06:09 am
content: When you need to fit rectangular objects into milled slots, then you have to account for the endmill radius and add a properly size overcut - that's a common knowledge in pcb manufacturing (or any milling at all).It's not possible to mill perfectly square inside corners when milling from the top- that's a fact. Only way to do so on a millling machine is to set the pcb vertically on the edge, bolted to some right-angle vertical surface serving as vertical support, but that's not something a dedicated pcb factory router can do.Or if it's less than a hundred PCB get yourself a beer and grab a file

author: Nerull
author_rank: Frequent Contributor
timestamp: January 09, 2015, 01:20:26 am
content: If you want to cover all vias, do this:QuoteIf you need to define individual vias you can select 'force tenting' in their properties.

author: nuno
author_rank: Frequent Contributor
timestamp: January 09, 2015, 01:30:49 am
content: I only use KiCAD, and it has an option on the via to say what layers it affects, maybe there's something similar on your CAD package.Your problems are not OSHP's fault as you've been told already, but I find 3 "annoyancies" about OSHPark:1) The render's PCB color and copper color on the renders are so similar that it's very difficult to distinguish both.2) I find the silkscreen's positioning tolerance a bit too "big"; I have to say I have no experience with similarly small silkscreens on other manufacturers.3) The PCBs are shipped loose inside a bubble bag, with sharp FR4 points from hand broken (separated) PCBs.Still I use their service sometimes, for prototypes (let's say it's for their free rendering service). So far I haven't find relevant differences (for the better) from futurlec which is the other manufacturer I've orded boards from (they actually pack them well for shipping); being in Europe it is the same for me to order from OSHP or futurlec, same shipping time, similar quality and price, but better shipping conditions for futurlec and a free renderer for OSHP.

author: free_electron
author_rank: Super Contributor
timestamp: January 09, 2015, 03:11:55 am
content: There is a much better way to do this.Yes, you can fidget with selecting the vias and playing with the tenting. But, if you make aan edit by adding kne via and you forget to run tat command youwill screw it up again.Write a design rul that sets the soldermask for vias to negative their diameter. Done.Whatever via you place will be tented.If a via is to be used for a testpoint you simp,y alter the ruleIsvia and (not (assemblytestpoint.))That will tent the vias that are not marked as assembly trstpoints.Design rule sets are your friends. You can automate almost anything with the design rules.

author: zapta
author_rank: Super Contributor
timestamp: January 09, 2015, 03:32:47 am
content: OSHPark are spec'ed as 0.1" milling tool diameter. If they suck it's because they try to up sale on checkout a non OSH MCU board or a local buddy. ;-)http://support.oshpark.com/support/articles/134889-internal-cutouts-and-slots

author: rx8pilot
author_rank: Super Contributor
timestamp: January 09, 2015, 06:58:33 am
content: Geez....declaring the fab company sucks because YOU made a number of mistakes? Learn the process before you bash someones livelihood.How many PCB's have you designed expecting internal corners to be sharp?

author: zapta
author_rank: Super Contributor
timestamp: January 09, 2015, 07:43:05 am
content: Quote from: nuno on January 09, 2015, 01:30:49 amYou don't have to order from oshpark to use the renderer. The renderer has poor resolution but is still very useful. I upload eagle files directly instead of Gerber's.

author: Corporate666
author_rank: Unknown
timestamp: January 09, 2015, 10:55:53 am
content: Quote from: rx8pilot on January 09, 2015, 06:58:33 am+1These are real people working hard to make a living. Bashing them for something they didn't do is beyond poor form.blueskull,You really need to modify your thread title, or if you can't, then request a moderator to do it for you. This kind of stuff will show up in Google searches.

author: zapta
author_rank: Super Contributor
timestamp: January 09, 2015, 01:49:10 pm
content: Quote from: 3roomlab on January 09, 2015, 11:00:54 amFor 2 layers $5 per square inch per three boards. For PCB prices check pcbshopper.com.

author: nuno
author_rank: Frequent Contributor
timestamp: January 09, 2015, 02:50:58 pm
content: Quote from: zapta on January 09, 2015, 07:43:05 amI know and I do it too (I always use Gerbers). What I meant is that I order from them as a "payment" for the free renderer I use, since some of the PCBs I do, fit their service, and for the most is its roughly the same "service level" I get from my other manufacturer.

author: zapta
author_rank: Super Contributor
timestamp: January 09, 2015, 07:47:26 pm
content: Will having a small drill near each of the corners before the milling improve the corner radius?

author: wraper
author_rank: Unknown
timestamp: January 09, 2015, 08:03:54 pm
content: Quote from: blueskull on January 09, 2015, 07:40:47 pmCompletely flat no, but you can choose PCB service which offers routing with smaller mill bit. For example, Smart Prototyping do 0.8 mm slots and plated slots for free.

author: free_electron
author_rank: Super Contributor
timestamp: January 09, 2015, 08:20:37 pm
content: slots and plated slots are different from routing ! slots are done using a special slot drilling bit ( both drills and mills ) during the main drill step.cutouts are milled during depanelisation.All you can do is have 4 drill strokes at the corners and then overlap the mill.

author: wraper
author_rank: Unknown
timestamp: January 09, 2015, 08:27:04 pm
content: Quote from: free_electron on January 09, 2015, 08:20:37 pmI said about plated slots because I see them on this PCB too. Of course they are different things.

author: kizzap
author_rank: Unknown
timestamp: January 10, 2015, 02:41:23 am
content: In future, if you definitely need the corners to be cleared for a square whatever, I think the easiest way to go about it is to do something like the image I have attached.

author: rx8pilot
author_rank: Super Contributor
timestamp: January 10, 2015, 04:13:40 am
content: Quote from: zapta on January 09, 2015, 07:47:26 pmNot really. You end up with overlapping radii and its messy. It also creates an interrupted cut for the router bit which can crack the carbide. The best solution is to draw in the overshoot in the corners so that no drill is needed. Most houses use a center-cutting router, if you can have a continuous line to follow with radii slightly larger than the "normal "tool" for the fab house - you will be golden.I owned and operated a CNC machine shop for years - this is how its done the easy way. There are broaching tools and laser cutters that can make internal corners, but that is not normally part of a PCB fabrication line. All things can happen with enough time and money ;-)Look at these two PCB outlines I have done recently. All inside corners have a >.063 radius that easily passes a .100" tool. Making the radius equal to the tool will cause it to chatter when it turns the corner. The one with arrows shows an over cut corner that has to seat a USB connector that has sharp corners. The profile requires no special work for the fabricator and I get no surprises when they show up.

author: marshallh
author_rank: Unknown
timestamp: January 10, 2015, 06:55:25 am
content: Same here, just route out the internal corner

author: steve_w
author_rank: Regular Contributor
timestamp: January 10, 2015, 08:42:06 am
content: Hey Wrapper,Where did you get the graphic, is it a standard or just "best practice." I want to learn PCB manufacture but find it very confusing, there is no one stop shop.Any reference to good PCB design tips would be appreciated.Steve W

author: Monkeh
author_rank: Super Contributor
timestamp: January 10, 2015, 11:22:05 am
content: Quote from: 3roomlab on January 10, 2015, 09:42:42 amIt's all included.You could just visit their site and see.

author: wraper
author_rank: Unknown
timestamp: January 10, 2015, 03:48:13 pm
content: Quote from: steve_w on January 10, 2015, 08:42:06 amThis picture is from smart prototyping website. Every PCB service have their design rules/capabilities. In this particular case IMO it is better to change PCB fab which can use finer tool. 32 mil vs 100 mil is a big difference. Dave made a video about PCB manufacturing stuff, few years ago I think.

author: SteveyG
author_rank: Unknown
timestamp: January 10, 2015, 06:06:23 pm
content: Quote from: Corporate666 on January 09, 2015, 10:55:53 amWhat's more impressive is someone has more than $7000 to spend on Altium Designer, but clearly has little experience!

author: zapta
author_rank: Super Contributor
timestamp: January 10, 2015, 09:33:35 pm
content: Quote from: blueskull on January 10, 2015, 08:08:25 pmI noticed this as well with orders from China, they improved my design (e.g stencil cut outs) without asking me and so far it was for the good.

author: LukeW
author_rank: Frequent Contributor
timestamp: January 11, 2015, 02:21:29 am
content: Quote from: SteveyG on January 10, 2015, 06:06:23 pmCould be a university etc. license for Altium.