Routing Anxiety

Archive BatchPCB
1

“R.A.” has had me sitting on my hands for the past month or two afraid of completing my first PCB and submitting it for a test run. I got the nerve to get into it a little bit today though.

Can anyone help me out? I am crippled by incompetence right now.

First a couple basic questions: What is the command format that I can type into Eagle, so I can line up the parts to specific absolute locations? I tried the move command but it seemed to be relative positioning. And is there a way to get a count of via’s on the PCB? I’ve tried Googling to no avail !??!

Back to routing. I’m afraid to even try manual routing because I have the idea that it will take hours, and if I move parts I would have to start all over again.

Autorouting seems to work pretty well but it looks incredibly ugly, and I’d like to avoid the ugliness. And, I admit, I’ve pretty much ignored adjusting Autorouter setup and DRC rules. The only thing I’ve been careful to do is create a class to thicken the 12 volt wires appropriately.

It’d be nice if I had a friend to work with on this project right now because there are so many things cummulating at once that I feel like one brain just isn’t enough!!! :shock:

Also, is this normal? When I do an ERC is get the error:

“SUPPLY Pin +5V overwritten with VDD”

Is +5V generally the same as VDD when using a PIC, or did I make a mistake somehwere?

And after a DRC check, I get a “Width” error pointing to the bottom line of my 12V ground plane polygon. What does that mean???

Sorry about all the questions. I’m just feeling sort of overwhelmed.

2

If you actually care about the PCB - don’t autoroute. Autorouting can be useful to give suggestions as to possible routes for especially hard to route signals - but you will always get better results routing by hand. You might try moving parts to one position, autorouting to see how it looks, and then move them to another position and try autorouting again. It will help you to visualize how the traces need to flow - but I still think you should rip them all up and do it by hand.

To align your parts to your grid - use the move command as you normally would, but when picking up objects ctrl-click on them instead of just clicking on them. It will align them to the grid.

The warning about VDD should be safe to ignore.

The width error is probably due to you making the polygon with a really fine line.

3

Thanks, I have read all the warnings against autorouting. It’s just that since I’ve never manually routed before it’s intimidating.

I suppose once I am entirely sure about the placement of my components I will be more prepared to start manual routing.

One question I still have is whether I can type the position of a component into the command line? I think that would be easier than dragging them on the grid in my situation.

4

I never use the autorouter and I always use the mouse to position. My boards come out pretty good.

On using drag to position, select a grid that works for you. I usually set the alternate grid to be 1/4 the regular grid. That way I can press the alt key and tweak to the alt-grid.

I would play around with hand routing a small board 1-2 ICs and a handfull of other components. Then work up to more complex. It took me maybe 5 boards to get comfortable with routing.

There are several things you can do to make it easier:

  • put a polygon on one entire side of the board and name it gnd. This is a gnd plane and will get rid of most of your gnd airwires. this will make it a lot cleaner.

  • lay out the ICs and other components. try to minimize the number of crossing airwires. play with the layout a lot.

  • route power next. a loop around the board might work well for you.

  • then start hooking up signal wires.

there are different strategies for routing the signal wires. Some people use one side for vertical and the other for horizontal. a lot depends on the board.

by this time you are probably well on your way.

5

djohnson:
Is +5V generally the same as VDD when using a PIC

Yeah, VDD is the more-positive supply in a CMOS circuit — the one connected to the drain (the D in VDD stands for drain) where electrons leave the transistor.

For a TTL or other bipolar device, the more positive supply is VCC, since it’s connected to the collectors of most of the transistors.

The more-negative supply on a CMOS device is usually called VSS (since it’s connected to the “source” terminal of the transistor, where the electrons enter the channel) but the more-negative supply of a TTL device is typically just called “ground”. :slight_smile:

6

djohnson:
Thanks, I have read all the warnings against autorouting. It’s just that since I’ve never manually routed before it’s intimidating.

I suppose once I am entirely sure about the placement of my components I will be more prepared to start manual routing.

One question I still have is whether I can type the position of a component into the command line? I think that would be easier than dragging them on the grid in my situation.

So far I’ve done all my routing myself, and eagle has kept me from ever making a mistake.

The best thing you can do to ensure success it to make absolutely sure your schematic is correct. Check that every wire is connected where it’s supposed to be, and not to anything it shouldn’t. The EC will almost always catch this stuff. Also, make sure the library components you are using are made correctly. Make sure the pins in the symbol match up with the pads on the package. Package dimensions and footprints are important too. If you’re using standard parts that can be found in general eagle libraries, there should be no problem, as long as you’re sure the part in the library is indeed the part you use. If you use custom components, you need to be careful. But that’s beside the point, because the autorouter can’t tell if your component is made wrong or not.

If you’re schematic is perfect, then it’s very difficult to mess up the PCB, since Eagle is very good at detecting inconsistencies. When you think you’re done, turn off all layers except unrouted and make sure all the routes are connected.

So I say go for it. As long as you’re not lazy, it should turn out fine. I’ve found the autorouter to be pretty much useless for high density stuff.

7

Just as a warning - some eagle footprints are not correct. I’ve been bitten once by this, and after that, I always checked it on paper first.

Cheers,

–David Carne

8

djohnson:
“R.A.” has had me sitting on my hands for the past month or two afraid of completing my first PCB and submitting it for a test run. I got the nerve to get into it a little bit today though.

Can anyone help me out? I am crippled by incompetence right now.

Greetings djohnson,

I see that you have some good suggestions from others to your plea for help. How complex is the PCB that you’d like to make? (Size, number of components, SMT or TH, Analog, Digital, uC, or mixed-signal?).

The first step is to know that you have correctly captured the schematic in EAGLE and that it passes ERC with no errors. There will always be warnings, and this should be examined carefully and mentally ignored once you know why they are reported. (For example, most devices use letters for the power and ground (GND, VCC, VDD, VSS, etc.) which you, as designer, connect to your power and ground buses (of which you must have at least two, sometimes more).

Next, check that each of your library parts are the right physical package, and that the device signals are on the right pins. Assume that inherited library parts from CADSOFT are probably okay but a 100% check is a good idea. Any that you borrowed from other sources are suspect.

Now you are ready to start a PCB design!

But, wait. There a lot riding on this step. You could be stuck in a do-loop for tens (if not hundreds) of hours. Why not make a trial PCB first?

That’s what I did with EAGLE and BatchPCB. I placed a few parts on a five square inch PCB, challenged myself to fit it on a specific footprint (a ready made plastic enclosure) and added mechanically challenging parts (such as a PCB mounted switch) that was not in the supplied EAGLE library.

The resulting PCB was very good, but not perfect. I doubt I personally can ever made a perfect PCB - there’s literally hundreds of ‘gotchas’ waiting to trip anyone up.

For many, a PCB is just a place to stick parts, they don’t care about geometry, symmetry, aestetics, or style. As long as the parts are connected electrically and don’t bump into each other, they’re happy! They see the autorouter as a time saver, and let it do the work.

On the other hand, some of us go nuts getting the PCB to be perfect. We never use the autorouter, but we always mitre the trace corners, size the vias to the trace width, isolate high voltages (I typically bring AC120V on the PCB and use a PC mounted transofromer), provide spacing between the part outlines, spell check the silk layers, add a copyright and title block, label the connectors and test points, etc. etc.

In my own projects I’m finding that mechanical (rather than electrical) issues take more of my time. I’ve done projects through Batch PCB where two PCBs plug together and ones where the PCB mounted switches pass through the panels (another CAD design tool and using a machine shop to make the parts). Once of the best tools I purchased was a digital caliper - it measures physical objects with a 1mil resolution.

Either way, a very wise move is to run the DRC before compiling the job to make Gerbers. Run it again with the check angle and check grid switches on. It’s not easy to get that “DRC:no errors” confirmation that your EAGLE PCB design is perfect. I think it’s worth the extra effort before sending the project out for fab.

If you’d like a virtual tutor, via PM or email, let me know. Glad to help, I actually like doing this stuff in my spare time!

Comments Welcome!

9

All these replies are so helpful I can’t think of any single one to reply to for thanks, but just know I really appreciate a place where people can do this kind of complex work. You all deserve to be millionaires for the kind of work you do. I’m a little happier when I’m programming but I’m sure that if I make time to start routing a lot more it will be fun too, with the help of your advice. Thanks again.

10

busonerd:
Just as a warning - some eagle footprints are not correct. I’ve been bitten once by this, and after that, I always checked it on paper first.

Cheers,

–David Carne

The only Eagle libraries I actually trust are the RCL and pinhead libraries. Everything else I just make myself. People are so afraid of making new parts - but once you know how to do it you discover that it's quite easy.
11

Useful strategies when routing are to route the critical tracks first, like the supplies and clocks. Route the shortest nets first and work up to the longest nets.

Leon

12

NleahciM:

busonerd:
Just as a warning - some eagle footprints are not correct. I’ve been bitten once by this, and after that, I always checked it on paper first.

Cheers,

–David Carne

The only Eagle libraries I actually trust are the RCL and pinhead libraries. Everything else I just make myself. People are so afraid of making new parts - but once you know how to do it you discover that it's quite easy.

I make lots myself but it’s just as easy to verify an existing one. Most library entries are correct however, there are some glaring errors. like the normal and wide versions of a package being switched. They used the standard package footprints so I got complacent and stupidly didn’t verify. I used the normal version and got the wide one instead. I was able to use it but only because I had routed just one trace in the middle. After that I ALWAYS paper test my boards (print it out and lay the parts on the paper).

I second the comment about making your own. It really is pretty easy. Worth the effort to learn as you will, most certainly, wind up having to make your own parts.

13

Another warning regarding the RCL library. The footprint for 0402 resistors in it is fine for hand soldering, but no good at all for reflow. At a previous workplace, we ran a board with the default 0402’s and they tombstoned all over the place.

Cheers,

–David Carne

14

busonerd:
tombstoned

lol, so that’s what they call it?

So what do you do, make the footprints smaller?

15

Yes, the tombstoning is caused by surface tension in the molten solder. With smaller pads there is less solder and tombstoning is less likely.

Leon