[sdiy] PCB / Panel Manufacture

rsdio at audiobanshee.com rsdio at audiobanshee.com
Fri Feb 7 07:55:21 CET 2020

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

More information about the Synth-diy mailing list