[sdiy] PCB / Panel Manufacture

[john slee]

Not anymore! They now have a black substrate/transparent soldermask option.
I used it to make a PCB panel recently, with a copper flood-fill on the top
layer, and (I think) it looks absolutely lovely

Hopefully this image attachment thing will actually work...

John


On Fri, 7 Feb 2020 at 21:55, Sarah Thompson <plodger at gmail.com> wrote:

> 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]
> _______________________________________________
> Synth-diy mailing list
> Synth-diy at synth-diy.org
> http://synth-diy.org/mailman/listinfo/synth-diy
>
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://synth-diy.org/pipermail/synth-diy/attachments/20200207/b1255072/attachment.htm>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: E4772D2B-FDFF-4D57-A6DB-DC62E721969F.jpeg
Type: image/jpeg
Size: 103108 bytes
Desc: not available
URL: <http://synth-diy.org/pipermail/synth-diy/attachments/20200207/b1255072/attachment.jpeg>