PCB design in Eagle

Anyone here uses Eagle? I am used to Altium and Eagle feels SO oldschool, but it is hard to beat the fully free Easel for personal projects.

Why is so difficult to drag, and click on stuff? any hint how to get used to that?

i.e. dragging pins is a pain in the ass! the software has no feedback on what is selected on what is a hot “spot”, it feels like the graphical editors I remember doing in a week in Uni

I use Eagle. It’s very … conservative in terms of CAD conventions where they expect you to do most everything using either keystrokes or scripts though there is usually a non-intuitive way to use the mouse.

Lol I’ve had the click and drag problems as well, it’s not always obvious where the handle to click is for each component as it could be obscured by any of the number of layers in the footprint. This is made worse when you start downloading random libraries from different places online as there isn’t a set convention on where the handle should be (you could always edit parts though and set handle to center or corner if you’d like). An easier way is to use the lasso mode so you just draw a shape roughly around what you want to move and it’ll select all handles inside the shape. Alternatively if the board isn’t too densely packed you can click and drag over to box select. Not great and yes it’s a pita but it does technically work.

The upside of eagle I find is there’s a library for just about everything, sch and brd linking is painless, doesn’t do that weird stitched line poly thing a lot of other pcb editors do with planes (making changes is so much easier when it’s one button click to re-render filled planes that act like polygons with vertices rather than a bunch of line segments that make up a poly), and erc/drc/cam process flow works very well.

What ticks me off is Autodesk moving Eagle over to cloud licensing, severely restricting free functionatlity, and year over year drastic price hiking the paid plans out of hobby price points.

1 Like

Thanks! Altium (CircuitMaker) seems a lot more polished, but they have restrictions like layers and the libraries are a horrible deal in that cloud version.

They are moving everything to Fusion 360. It is like an IFRAME with Eagle. Feels very buggy for now.

Yeah dragging sucks in eagle pretty bad.

The way it works if you haven’t figured it out if an object is all on it’s own it will drag it straight away on the first left mouse button click.

The problem is that if there is anything remotely close to where you are click (which is common) it will actually “highlight” the component or trace first, and if what you are trying to get to isn’t highlighted you have to cycle through different selection choices with the right mouse button.

Once you’ve finally highlighted the correct component then you left click again to begin dragging.

It’s a giant pain in the ass because you kinda don’t know whether it will grab it on the first try or not. Sometimes if you expect to have to do the highlight first thing, but then it drags it on the first try you’ll end up moving it a tiny bit then dropping it.

Also when you are cycling through selections you’ll zoom past what you want and have to keep going.

If you’ve got more than 2 layers or very densely populated areas this becomes a real pain.

Altium is great horrendously expensive. I think most people will agree that KiCad is the way to go.

But you are right, eagle does have a lot of libraries out there, and both adafruit and sparkfun do stuff in eagle. But actually I’m to the point I almost always make my own footprints for stuff anyways, because many times it’s faster than finding just the right part and it confirms the pinout is correct from the datasheet.

That said, www.snapeda.com is super awesome if it has your part in it. And it can give footprints for all the major packages, and sometimes even has the 3d model along with it so if you are linking it to fusion360 or another cad package it will work.

1 Like

Thanks for the feedback, quite helpful!

I mean I feel that Eagle is super mature, doing the tracing is very pleasant, and the output is very clean. With CircuitMaker I had to fiddle a lot with details. The link between sch and pcb also very smooth.

One last question for the more seasoned: to make a weird CNC cut in the middle of a PCB, is it ok with lines on layer 46? I cannot get it working on the online gerber viewers

Yes the milling layer (46) will work fine, or I’ve naughtily even just used the dimension outline layer (20) before to do inner routes with a note specifying how I want it milled out (jlcpcb accepted the gerbers and manufactured without issue but as always ymmv).

1 Like

Generally I go for using a 0 width line for the exterior and internal cutouts.

Almost all gerber viewers will render this “not exactly”. For example if you read through OSHpark documents they say that it will show the dimension line but won’t actually “blank” out the negative space. Basically their script isn’t advanced enough to know what is internal or external.

When using other gerberviewers like from PCBway or JLCpcb both of them in general have lots of glitches even on a normal dimension.

I find that OSHpark is generally the “best” for determining what you are actually going to get.

And the advantage of using 0 width traces for dimension is that it allows the board house to use whatever size milling tool is appropriate for the cut. If you define a width then they might try to use something that doesn’t make any sense or reduce the options they have to mill it out.

In general, I try to only use the milling layer for plated slots, that way it’s more obvious to the operator what’s going on.


But how do they know it is internal cut for example?

The operator that runs the machine has to figure it out, generally this isn’t an issue but if you have a complex design you can write “CUTOUT” in the parts you want gone. This is talked about in the design rules for virtually every board house, its good reading.



1 Like

Also probably worth noting, board houses kind of “don’t like” internal cutouts because it creates little bits that get left behind when they take the panel out, or it falls down to the bottom of the milling machine.

It’s not like they won’t do them, but if you look at PCBs that are used in products you vary rarely see actual cutouts in them. If you go high enough volume where they are actually calculating how much time and effort your PCBs take instead of just giving you a rack rate, having internal cutouts will increase the cost because of the cleanup time between panels. But at that volume you’re also counting how many vias and other drills you are placing to calculate cost.

1 Like

Thanks! I have almost 0 experience ordering boards but I remember that a quite convoluted design in Altium was cut perfectly for 5 USD the 10 units in elecrow (not internal) so I am hoping the do the same with this.

I was trying to make the open source pcb for your “arduboy” nano clone, but there is no way I pay for altium just to joke around because the 2 layer limit on circuitmaker.

A cut is a cut, so long as the toolpath doesn’t do anything wacky causing damage most pcb manufacturers will give you the freedom to hang yourself with a design that may not work. I don’t think it practically matters to the machine whether it’s an interior or exterior cut, but the cad department may change a corner or a bit of a side of your interior cut to a mousebite which they can poke out after manufacture just to alleviate floating bits of pcb from messing things up with their machine if they think it’s necessary.

At the risk of going off topic; have you considered using KiCad? Many open source developers are turned off by Eagle’s current licensing terms (and lack of Linux support).


Honestly KiCad is probably the best way to go. If you don’t want to pay for eagle, the free version is just going to lock you into learning something that has limited functionality, also isn’t being developed very heavily any more.

KiCad is getting new features all the time and so if you learn it then you’re with a big community of people.

There are some things KiCad still can’t do like curved traces, it just recently added beveled corners though.

The push+pull routing that KiCad has is probably worth it on it’s own although I believe the latest versions of Eagle also do this? Unknown, I’m stuck on the last offline version of 7.7.0 after that you need to have a subscription… which pisses me off because I paid a lot of money for my license.

1 Like

I tried but it just feels like gimp in the early 2000s, which break the joy for me. I hope it continues improving (audacity made me forget audition, blender is awesome, etc)

In this case, that subscription model is slightly more convenient for my purposes. I.e. build personal/open stuff and when I need the license for a business 60 USD isn’t steep for a month

It is and it isn’t. I would have got 2 and a half years of subscription for what I paid, and I suppose I’ve got more out of it than that by now. And when you consider it also includes all the other cad applications with it, maybe it’s ok.

But yeah eagles selection process is a pain in the butt I scream at my computer sometimes after trying to move something like 4 times in a row.

I guess my biggest pet peeve actually is the fact you can’t leave options menus open. I’ve got tons of screen real estate and it would be SO MUCH better if I could leave a window open to select from active layers instead of having to use a drop down menu each time.

1 Like

I feel your pain. I found this helpful

Are you familiar with the ASSIGN command or the Options → Assign… menu?

These allow you to set up custom shortcuts which run EAGLE commands, including scripts and ULP if needs be.

So what you could could do is set up a shortcut key to do say:
DISPLAY NONE; DISPLAY 1 20 21 23 25 29 31

This would first clear all the selected layers and then enable the Top (1), Dimension (20), tPlace (21), tOrigins (23), tNames (25), tStop (29), and tCream (31) layers.

You can create similar ones for the bottom and internal layers.

You can also do things like add “rat; rip @;” to a shortcut so you can quickly run ratsnest and clear all the polygon fills in case they are obscuring visibility on things.

An even better way is to set up your layers you want to view and them save them by right clicking the layer button and naming it using “New”

Screen Shot 04-10-17 at 10.46 AM

Then it is as simple as assigning a keyboard shortcut that inputs “DISPLAY (layer_group_name)” to switch to that group of layers.

It’s by no means a way to have the layer menu open all the time but I find it does save a lot of time.


Bro this is life changing. Yeah still not as good as if I could keep the layers open but “rat; rip @” is awesome. I get into the habit of not adding my polygons until after EVERYTHING is done, then just having to squint if I need to make changes… or if I open the document as new just never touch the ratsnest button.

Yes the ripup shortcut is super handy! I also have stayed with Eagle 7.7. It does what I need it to do and I have a metric ton of custom part footprints that I would have a redo if I ever moved to another system. I’ve tried and Kicad just isn’t for me.