[sdiy] PCB / Panel Manufacture

Sarah Thompson plodger at gmail.com
Fri Feb 7 11:53:30 CET 2020


OSHPark manufacture in the US and are cheap and fast. I used them a lot
when I worked at NASA for prototypes. They can work with EAGLE easily. I've
also used them for front panels by designing the panel as a PCB -- this
works pretty well. One peculiarity is that all their boards are purple,
which you may or may not like! :-)

On Fri, Feb 7, 2020 at 7:56 AM <rsdio at audiobanshee.com> wrote:

> Hi Shawn,
>
> Eagle will work fine. Basically all of the fab houses accept Eagle files,
> and certainly all of them support Gerber files produced by Eagle. Eagle has
> all of the features you need to make professional boards. It will take you
> a long time to learn everything, but everything can be done in Eagle. There
> are some commands and key combinations that are esoteric, but nearly all
> CAD software is like that, except for some of the newer programs (but those
> are less than fully professional). Your best bet is to find the online
> support forum for Eagle, read the documentation, and ask questions if you
> can’t find answers to your questions in the archives of the forum. I
> purchased Eagle before it became subscription based, so my license has no
> limitations. I don’t know whether your license is size-limited,
> layer-limited, page-limited, or otherwise limited. So, unless you run into
> limits, I recommend treating Eagle like a new synth that you dive into and
> learn absolutely everything you can about it.
>
> Keep in mind the size constraints of Eurorack. You don’t want breakaway
> tabs on your PCB interfering with modules next to yours. Same thing with
> face plates, although Dieter covers this on the doepfer.de site.
>
> I order all of my PCB designs from USA-based fabrication houses. Prototron
> is near me in Redmond, WA. They’re probably the most expensive I’ve ever
> used, but they’ll make a deal for quantity. Sunstone Circuits in Oregon has
> some bargains, but it really depends upon your size. Advanced Circuits,
> a.k.a. 4PCB, have some decent deals on prototypes, and their quality is way
> above the cheaper places. I can literally see the quality different with
> the naked eye when comparing an Advanced Circuits PCB with my exact same
> design files made by a cheaper fab house. OSH Park probably has the best
> prices in the USA, but you’ll wait longer than anywhere else. Their quality
> is really good - probably all you’ll ever need - but they’re not top
> quality.
>
> Once nice thing about 4PCB is their FreeDFM site that will check your
> Gerber files and report errors. There’s no charge to use the site, but
> you’ll get one email asking if you want to buy the boards. I’ve never
> received more than one advertising email, though, so I often use them to
> check a design even when I order somewhere else. This is a good way -
> especially when you’re just starting out - to get an idea of whether your
> PCB is following standard design rule
>
> Speaking of fab houses and Eagle, make sure you find and download a DRU
> (Design Rules) file for each of the sites that you want quotes from. OSH
> Park and Sunstone Circuit actually have the files on their web sites.
> Advanced Circuits describes all the constraints textually, and if you study
> how to edit the data in Eagle then you can create your own DRU for Advanced
> Circuits orders. Before ordering any new PCB design, make sure you change
> the DRU selection to point to the file describing the specific fab house
> that you want to order from, and run the “dru" command to check for
> violations. You might have to change trace sizes or move things around to
> fit the capabilities. Sometimes, the minimum drill size makes your vias
> larger, and then everything has to be spaced further apart. FreeDFM will
> catch this, but you can catch almost all of the same issues inside Eagle
> before you upload anything. Eagle remembers which DRU file you’ve selected
> for each PCB project board file, so you can order from different places.
>
> Some people think PCB fab options are as simple as: China is cheap, and
> USA is expensive. Some people even think that all PCBs are made in China
> even when you order from a USA company. Sometimes this is true, but not
> always, and there are other factors. For one thing, TSA can randomly hold
> up your PCB order at the border, and then you’ll be waiting longer than OSH
> Park (OSH Park is my benchmark for “long wait times"). I had one customer
> order from the cheapest Chinese PCB shop, and then screamed bloody murder
> when TSA held all of the boards for weeks, maybe months - delaying their
> product manufacturing. You might pay more in USA most of the time, but it
> might also really be worth it to you when you consider everything like
> time-to-market.
>
>
> I’ve made several panels, both for 19” rack electronics and for Eurorack.
> I’ve ordered everything from Front Panel Express in Seattle. They’re
> somewhat expensive, but if you pay attention you can keep the price
> reasonable. For one thing, it seems really expensive to add paint in etched
> lettering, and so I’ve never paid for that. However, if you just spend a
> few cents extra for anodized aluminum, especially black, then etched
> lettering will reveal the bare aluminum color behind the anodized surface,
> and then you don’t need to pay for paint to make the letters visible via
> contrast. Front Panel Express will also screen print any image, but I’ve
> only used that for projects where I have the extra budget - it’s not cheap,
> either.
>
> Front Panel Express has a free application that you use to design the
> panels. It’s probably a really bad idea, because I don’t know whether you
> can import or export designs from other design tools. Since I’m only doing
> prototypes, I don’t worry too much that all of my designs are in a
> proprietary format. However, it is really convenient that you can get price
> quotes within the app, and they’re even itemized so you can see what
> determines the cost and sometimes even delete or change features that are
> too expensive. Sometimes it’s a slow process to quote all of the variations
> appropriate for a given design, but if you’re cost conscious then it’s
> probably worth the time to research.
>
> One cool thing about Front Panel Express is that if you screw up a panel
> in a way that you can fix it by cutting more away, then you can save money
> by sending back the original panel for them to cut changes. That ends up
> being cheaper that ordering a second panel from scratch, but you really
> have to work extra hard to create a design that includes just the
> differences between the old mistakes and the new desired panel. I realize
> this is probably only a practical option when you live close enough to
> drive by, drop off the old panel, and pick up the new one later. They have
> free shipping for large orders, but when you’re saving money you have to
> think about the cost of shipping when your total is below their free
> shipping minimum. Obviously, though, you can’t fix a panel after you’ve cut
> too much away - there’s not a drill that can add aluminum back on the face
> plate.
>
>
> For both PCB and panel designs, you want to make careful measurements of
> all mechanical parts, particularly screw holes, screw placements, and drill
> sizes. Not only do you have to align the components with the boards and
> panels, but you have to align the boards and panels with each other.
>
> In Eagle, I tend to create extra layers, or use Documentation or Reference
> layers to draw the mechanical parts that are not actually part of the PCB.
> This helps me get an idea of how things will fit together later. Of course,
> there are work flows that allow you to create 3D data for your PCB design.
> Eagle is compatible with that, and I know people doing it, but I haven’t
> taken the time to learn. Besides, you still need to create 3D models for
> the face plate and other mechanical components, and that seems like a lot
> of work unless you’re using the exact same parts as everyone else.
>
> You have to get used to the fact that some parts are measured in metrics
> units, and others are measured in English units. Within Eagle, I frequently
> switch my measurements between Inches, Mils, and millimeters. It’s a pain,
> because I don’t know how to change the units after calling up the editor
> for a component placement, so I just cancel the dialog, switch units, and
> then open the dialog again. Once I get all parts that touch other parts
> aligned properly, I use the Eagle “lock” tool to prevent those parts from
> being moved accidentally. Components that only mount on the PCB and nothing
> else are left movable.
>
> Meanwhile, FrontDesign.app also allows English and metric units, and again
> is a bit of a pain because I find that you always need to mix both in the
> same design. Eurorack is a bizarre mix of English units and metric. Even
> though the numbers are almost always reported in millimeters, it’s fairly
> obvious that 1 HP is 0.2” (1/5”), so I often check placements on a 0.2”
> grid.
>
> There are lots of things to learn, but these days we have the internet. I
> recently had to figure out what size hole to drill to guarantee the
> standard amount of room for an M3 screw and an M6 pot shaft. Sometimes the
> data sheets for the electronics components will tell you these things.
> Other times, you just have to ask the industry what’s a standard drill size
> for an M3 screw.
>
> Personally, I prefer solid aluminum to a PCB for front panels. Granted,
> you can order a multilayer PCB and dedicate a solid copper layer to shield
> your electronics from emissions, but it seems a lot easier to keep out
> noise with a solid metal enclosure. For Eurorack, that means a metal case
> and metal face plates. But there’s nothing wrong with using Eagle to design
> cool face plates.
>
> You can even change the colors of the layers in Eagle to get a rough idea
> of how the finished product will look. I designed a product where the
> internal boards have black screen print on clear solder mask, and the raw
> copper and FR4 material shows though. OSH Park has an option now with black
> PCB material, white screen, and clear solder mask that looks crazy - you
> really have to think about how it will look before you order.
>
>
> One weird thing about Eagle is that Devices seem to require all Symbols
> and Packages to come from the same library file. So, you can make your own,
> but if you want to borrow an existing Package for your Device, you’ll have
> to copy that Package into your library. I recommend building your own Eagle
> parts library, and back it up regularly. I actually use revision control,
> just like I do for source code when doing computer software design, to keep
> track of my own Eagle library files. That way, I can recover an old
> version, and can work on multiple computers and know that I have the latest.
>
> There are Eagle libraries available for free, and they’re sometimes a
> time-saving starting point, but never trust that they’re correct. Whether
> you create the packages yourself, download them from the Eagle community,
> or mix and match, you always want to study the data sheets for the
> electronics parts, direct from the manufacturer, and make sure all
> measurements are correct. Here is where you learn that you can’t make the
> drill size the same as the through-hole lead size, because it will be too
> tight once the copper plating, board finishing and tinning are completed
> and the hole gets smaller.
>
> Regarding data sheets, I recommend that you *always* go directly to the
> part manufacturer’s web site, search for the exact part you’re using, and
> download the latest data sheets for the stuff you’re using. Trusting Mouser
> to have the latest information, or some internet aggregator that wants to
> sell you knockoff chips, is not the way to get your design right. It takes
> almost exactly the same amount of time to download the data sheet from the
> wrong source as it does to download it from the right source. Once you do,
> keep a backup of those files for future reference, and keep the files
> organized so you know what you have. On that note, I currently have
> approximately 2,838 data sheets from 218 different manufacturers under
> ~/Documents, and I have a few backups of those.
>
> Most of them have recommendations somewhere for PCB design for their
> parts, but a lot do not have any hints. That’s partly because the proper
> way to design is highly dependent upon the process used by your particular
> PCB fab, and when you change fab houses you might need to actually change
> your PCB design to accommodate.
>
> Some companies like Analog Devices and Texas Instruments also have
> Application Notes and even electronics design articles from excellent
> engineers who will explain many of the things you need to know to design a
> PCB. You have to start by reading the entire data sheet for the parts
> you’re using, and follow every link in that data sheet to the other
> documentation from the manufacturer on related information that you might
> need.
>
> As for whether you need 2 oz copper, or super wide traces, there are
> probably plenty of articles online that will discuss that.
>
> Brian Willoughby
> Sound Consulting
>
>
> On Feb 6, 2020, at 7:31 PM, Shawn Rakestraw <shawnrakestraw at gmail.com>
> wrote:
> > Hey All! I'm new to the list and this is my first question.
> >
> > I want to dip into making some PCBs and possibly front panels. I am into
> eurorack, so that is what I will be aiming toward. I have been learning how
> to use Eagle to make my schematic into a board.
> >
> > Currently, I have been working on a power supply PCB that would mount
> inside of a case, so I don't have any major size constraints or precision.
> I will probably make a simple bus board next to distribute the power. Then
> I want to move on to an actual module. Something simple at first.
> >
> > I should also mention that I am in USA, although that probably doesn't
> matter that much anymore. I do prefer to order things in the US when I can
> though.
> >
> > I am asking for any advice at all really. My question begins with who /
> where to order from, but after that I am a bit in the dark about what to
> even ask. I don't know if copper trace thickness should be a concern.
> Obviously with power PCBs and distribution boards you want wide traces and
> I have done some research to try to learn how wide for certain amp loads.
> Really, any advice will be good for me - anything that you wish you had
> known before your first order could be helpful.
> >
> > Has anyone made panels and if so, what is the beginning process for
> that? Can you design them in Eagle using Nets or something? I don't know
> how people even design them.
> >
> > Thanks in advance, I look forward to your replies!
> >
> > - Shawn
>
> _______________________________________________
> Synth-diy mailing list
> Synth-diy at synth-diy.org
> http://synth-diy.org/mailman/listinfo/synth-diy
>


-- 
[s]
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://synth-diy.org/pipermail/synth-diy/attachments/20200207/d3c041f1/attachment.htm>


More information about the Synth-diy mailing list