Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

EAGLE Autoroute problem

Status
Not open for further replies.

transistance

New Member
OwnModel1.sch -> Pspice Model
PCB.sch-> Eagle Model

Eagle can not autoroute my design. Is it not possible to finish this on a double sided? Does it have to be multiple layered?

Am I doing something wrong? My does indeed look like a rat's nest in eagle.

I am very very new to Eagle and PCB fabrication.

thanks in advance,
 

Attachments

  • PCB.zip
    27.6 KB · Views: 283
The Eagle autoroute is not up to the task. This is not a big deal because most people I know prefer to route by hand. There are too many things the router does not know about. Even if it could come up with a layout you might not like it.

I suggest you go to the Eagle site and work through their tutorials on routing. It is not an intuitive process.

You can do a lot on two layers. More as your experience grows.

The airwires will look like a rats nest. Finding a component placement that untangles this as much as possible is the first step. Moving and rotating parts to get the least tangle.

I have not idea how complicated your circuit is so it is difficult to say much more.


OwnModel1.sch -> Pspice Model
PCB.sch-> Eagle Model

Eagle can not autoroute my design. Is it not possible to finish this on a double sided? Does it have to be multiple layered?

Am I doing something wrong? My does indeed look like a rat's nest in eagle.

I am very very new to Eagle and PCB fabrication.

thanks in advance,
 
is it easier just to look at your protoboard and route from there rather than your pspice schematic? makes a better visual image imo. or even better, look at your protoboard hand-draw a draft on paper with a pencil then draw the pcb on file?

if i want to draw the pcb from scratch is it possible? or do i have to draw schematic first then convert it to pcb visual and then move them around?
 
Last edited:
Schematic capture is when you draw the schematic and the program generates the airwires/rubber bands (the rat nets in layout) for you. This ensures that your PCB matches your schematic. It also allows you to do ERC electrical rule checks and DRC design rule checks.

If you do not want to use schematic capture do not use eagle. I suggest sprint layout but others will work. Might be a good idea for you in that I am getting the feeling that you just want to get it done.

In the long run eagle will save time with the schematic capture feature but the package takes longer to learn the non schematic capture software.

The layout on your protoboard may or may not be the best choice for the PCB. Depends on how you arranged the parts, just as on the PCB layout program.

is it easier just to look at your protoboard and route from there rather than your pspice schematic? makes a better visual image imo. or even better, look at your protoboard draw a draft with a pencil and paper in hand then draw he pcb on file?

if i want to draw the pcb from scratch is it possible? or do i have to draw schematic first then convert it to pcb visual and then move them around?
 
Last edited:
I always wanna just get things done, have a really impatient personality thus screw up often..
I just expected the software to be a little smarter, apparently it does not really reduce the work load that much.. If the right thing to is to capture schematics then I will.. Is eagle more commonly used and "smarter" then Orcad Capture?
 
I always wanna just get things done, have a really impatient personality thus screw up often..
I just expected the software to be a little smarter, apparently it does not really reduce the work load that much.. If the right thing to is to capture schematics then I will.. Is eagle more commonly used and "smarter" then Orcad Capture?

Schematic capture saves time in that if you get the schematic righ the board wll be too. You do not have to compare the two. That is the work it does for you. The ERC rules help you ensure that you at least connected pins and the DRC rules can make the difference between a board that is easy to soldeer and etch and a pig. But you have to know how to use all of that.

Eagle light is free. Orcad cost a lot.
Even with orcad some (not sure what %) of boards are routed by hand. A lot of route the first trace by hand and have the system mimic it with the other 7 sort of thing.
 
I use OrCAD Capture because I like the interface, I use Sprint Layout because I like its interface. I manually route traces as autorouters never seem to get things quite right IMO.
 
Autorouting is one of those problems that a Computer Science jockey (capital "C", capital "S") would consider a "hard" problem. That means not just "Golly, chief, that's tough!", but rather that nobody has solved the fundamental problems behind it, so algorithms to do it boil down to brute force.

Classic examples of this class of problem are the Knight's Tour and the Travelling Salesman.

Anyway, don't be so impatient that you shoot yourself in the foot by moving past Eagle too fast. There is no software which is going to save you the trouble of using your brain. It's the most powerful computer you have.

Sure, Eagle has a somewhat Byzantine interface which is mired solidly in 1991, but it will save you time in the end--as 3v0 said, the ERC and DRC alone are worth it. Use the schematic capture, make sure everything checks out, and then route by hand. Sometimes using the autorouter can show you things you didn't see in the design, too.


Torben
 
Something I do in Eagle, and used to do also in Orcad, is let autoroute do the "heavy lifting". By this I mean, set your design rules, let it route whatever it can, then look at what it can't do, then try and deduce why. Many times moving even one part will solve a dozen problems. This way you can use your brain to solve one or two problems, and maybe only hand route a couple traces. Also, when you are manually routing, sometimes when you rip-up a trace and start rerouting, the software will "re-snap" a new route or simplify a current one, fixing even more for you.

Always do a cleanup using the software via the rats nest function if you move parts, this simplifying will sometimes ease many routing problems.

I always try to layout the parts physically in logical groups close to what they will connect to. This makes the biggest difference in the routing. I have had boards with the max part count in the free version of Eagle, and only used 3 Vias, and they could have been removed if I had used existing resistors as jumpers, but I wanted all the parts in straight rows.

It's an Art, it is also a skill you develope, the more you do the better you get. Soon you will bee thinking so far ahead in your routing you won't be able to keep up with your thoughts.
 
Zevon8 nailed it. Autorouting is not the answer but it can be a useful tool to get you partway there.

I also agree that routing in general is as much an art as anything else. I always feel my spirits sink when I first look at the board with all the airwires and components sitting beside the board area, waiting. Once I get started, though, it's actually quite fun. Small changes can drastically simplify things, too. Ratsnest is invaluable.

Sometimes the hard part is knowing when to stop, since you can always come back to a board and see "just one more thing" which could be better. ;)


Torben
 
Something I do in Eagle, and used to do also in Orcad, is let autoroute do the "heavy lifting". By this I mean, set your design rules, let it route whatever it can, then look at what it can't do, then try and deduce why. Many times moving even one part will solve a dozen problems. This way you can use your brain to solve one or two problems, and maybe only hand route a couple traces. Also, when you are manually routing, sometimes when you rip-up a trace and start rerouting, the software will "re-snap" a new route or simplify a current one, fixing even more for you.

Always do a cleanup using the software via the rats nest function if you move parts, this simplifying will sometimes ease many routing problems.

I always try to layout the parts physically in logical groups close to what they will connect to. This makes the biggest difference in the routing. I have had boards with the max part count in the free version of Eagle, and only used 3 Vias, and they could have been removed if I had used existing resistors as jumpers, but I wanted all the parts in straight rows.

It's an Art, it is also a skill you develope, the more you do the better you get. Soon you will bee thinking so far ahead in your routing you won't be able to keep up with your thoughts.

Very well stated!

In addition to this, and Torbin's comments, when I am satisfied with my first attempt, I will also rename this board (with both the board and schematic closed) then after re-opening the schematic, click on switch to board, which gives me another board. I try to see if I can do it better on a second attempt. Usually I can, but if not, I go back to the first one.
 
Eagle routing

Hi transistance,

impatience is something Turks have to live with. They are just created that way.

Going to electronic design you must defeat your impatience. The program can not do the mental work for you. A board design, no matter how many components are used, is always artwork. The program however doesn't know of any art.

Here is a good advise to design circuit boards without lots of stress and confusion (because of the heavy load of airwires): This is an easy step-by-step-method.

Draw a part of the schematic, say 10 components and connect them. Then create a board, just typing "board;".

You should also already have considered what the final board should look like, e.g. PCB-connectors and terminals at the outer edge of the board and know the side they should be placed. (You certainly don't want terminals pointing to the front end of a board which also contains indicator LEDs and switches. :D)

Place the few components in a way to reduce intersections and crossings already with the airwires. Then route that part manually. Don't do it too sohpistacated (e.g. using a routing grid size of 1/160inch, 1/20inch will to in many cases), since you will decide to rip up one or another trace for rerouting later.

With those 10 components you know exactly their relation within the circuit and can place them logically and practically.

Then step over to the schematic again and repeat the procedure until you are finished.

You'll see success at the end with a good looking design.

My philosophy about electronic design has always been that: A circuit does not only have to function properly; it must look beautiful too. :)

As already mentioned placing a part somewhere else (not too far from the others connecting to it) or just rotating it might solve many problems. Move or rotate and use "ratsnest" right away.

It is disgusting and frustrating placing parts on a board, working for hours to route them to finally find out that a decoupling capacitor (connected to a voltage regulator IC) was placed at the opposite end of the board, making a good detour to its destination, and being worth - NOTHING.

Hans

P.S. I know a lot about Turkey and its people. I've lived in Turkey for more than five years. Concerning patience there seems to be a "one-way" impatience. Think it over!
 
All auto routers exhibit various degrees of suckage. Real designers hand route anyway, unless pressed for time.
 
Last edited:
I did a really quick job using the auto router, usually I like to hand place stuff but I did this so that you could see the kind of layout possible. You can take this and edit it by hand to slowly shrink it down.

Note that R13 seems to be unconnected on one leg ?

This was all done by placing / rotating components untill the wires didn't seem to cross much, then hitting autoroute with the default settings.

Hope it helps.
 

Attachments

  • PCB.zip
    6.4 KB · Views: 235
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top