Electronic – ny PCB design software/extension that can do automatic components placement

The Eagle autorouter is a decent tool, and I use it a lot. However, like any tool, you have to know how to use it well and understand its limitations. If you are just expecting to throw everything at the autorouter, you will be dissappointed. No current auto router, and probably for a number of years to come, can do that for anything beyond contrived or toy problems.

You say there are settings in the Eagle autorouter you don't understand and never mess with. This is a bad attitude, and probably a good part of your problem. There is no set of control parameters that works on all boards. Even within 2 layer boards there are various tradeoffs. You absolutely have to read the manual and adjust the parameters for your particular situation.

For two layers boards, I often try to keep most of the bottom layer a ground plane. I therefore use the top layer for interconnects as much as possible, and the bottom layer for short "jumpers" to make the routing topology work out. In this case, I set a high cost for routing in the bottom layer.

Before autorouting, you have to look at the board and think about the critical areas that you can't explain to a autorouter. For example, you want to keep the loop currents of a switching power supply local and off the main ground plane. The same holds true for high frequency currents local to a digital chip, like bypass caps and crystal with its caps. If you are using the pseudo ground plane layer as I described above, then you want to manually connect every ground connection immediately to the ground plane with its own via. That leaves maximum room on the top layer for routing everything else.

The process of routing a board even when letting the auto router do most of the grunt work looks like this:

1. Manually route the critical paths, as I mentioned above.

2. Do basic housekeeping pre-auto routing. This includes connecting all the ground pins directly to the ground plane for example.

3. Look for problem areas where you can see the autorouter might get itself into trouble. If there are short connections in dense areas you might want to make some of them. This takes some experience and intuition, so if you're new to the particular autorouter, skip this step for now.

4. Save a copy of the board, then run the auto router. If this is the first thru here, just have it do the minimum to find a solution. The purpose of the first few times is to see where the problem areas are so you can adjust the layout and your manual pre-route accordingly.

5. Look carefully at the resulting route. See where the problem areas are. Revert back to the saved copy from step 4 and adjust your layout and manual pre-route according to what the auto router did. Repeat back to step 4 until the result looks reasonable. As you do more iterations thru here, you crank up the autorouter optimizations and other parameters to make a more final route. In the beginning you are just trying to see if it can find a solution and what the large problems are. In later passes you converge on a real route. I start out with no optimization passes, and use 8 for final routes. I also configure early passes to find a solution, then later passes to optimize it.

6. Do manual cleanup on the route. In the case of a two layer board with mostly ground on the bottom, you want to minimize the maximum dimensions of islands in the ground plane. It is better to have a large number of small islands than fewer large islands. Sometimes you can see ways of rearranging signals locally to minimize the jumpers on the bottom layer. In this stage, the big picture has already been taken care of and you are focusing on manually optimizing small areas. This is similar to a peephole optimizer of compilers.

Here is a Eagle autorouter control file I used on a two layer project with the bottom layer a ground plane to the extent possible:

; EAGLE Autorouter Control File

[Default]

  RoutingGrid     = 4mil

  ; Trace Parameters:

  tpViaShape      = Round

  ; Preferred Directions:

  PrefDir.1       = *
  PrefDir.2       = 0
  PrefDir.3       = 0
  PrefDir.4       = 0
  PrefDir.5       = 0
  PrefDir.6       = 0
  PrefDir.7       = 0
  PrefDir.8       = 0
  PrefDir.9       = 0
  PrefDir.10      = 0
  PrefDir.11      = 0
  PrefDir.12      = 0
  PrefDir.13      = 0
  PrefDir.14      = 0
  PrefDir.15      = 0
  PrefDir.16      = *

  Active          =    1
  ; Cost Factors:

  cfVia           =   50
  cfNonPref       =    5
  cfChangeDir     =    2
  cfOrthStep      =    2
  cfDiagStep      =    3
  cfExtdStep      =    0
  cfBonusStep     =    1
  cfMalusStep     =    1
  cfPadImpact     =    4
  cfSmdImpact     =    4
  cfBusImpact     =    0
  cfHugging       =    3
  cfAvoid         =    4
  cfPolygon       =   10

  cfBase.1        =    0
  cfBase.2        =    1
  cfBase.3        =    1
  cfBase.4        =    1
  cfBase.5        =    1
  cfBase.6        =    1
  cfBase.7        =    1
  cfBase.8        =    1
  cfBase.9        =    1
  cfBase.10       =    1
  cfBase.11       =    1
  cfBase.12       =    1
  cfBase.13       =    1
  cfBase.14       =    1
  cfBase.15       =    1
  cfBase.16       =    5

  ; Maximum Number of...:

  mnVias          =   20
  mnSegments      = 9999
  mnExtdSteps     = 9999
  mnRipupLevel    =   50
  mnRipupSteps    =  300
  mnRipupTotal    =  500

[Busses]

  @Route

  Active          =    1
  cfVia           =   10
  cfChangeDir     =    5
  cfBusImpact     =    4
  cfPolygon       =   25
  cfBase.16       =   10
  mnVias          =    0
  mnRipupLevel    =   10
  mnRipupSteps    =  100
  mnRipupTotal    =  100

[Route]

  @Default

  Active          =    1

[Optimize1]

  @Route

  Active          =    1
  cfVia           =   99
  cfNonPref       =    4
  cfChangeDir     =    4
  cfExtdStep      =    1
  cfHugging       =    1
  cfPolygon       =   30
  cfBase.16       =   10
  mnExtdSteps     =   20
  mnRipupLevel    =    0
  mnRipupSteps    =  100
  mnRipupTotal    =  100

[Optimize2]

  @Optimize1

  Active          =    1
  cfNonPref       =    3
  cfChangeDir     =    3
  cfBonusStep     =    2
  cfMalusStep     =    2
  cfPadImpact     =    2
  cfSmdImpact     =    2
  cfHugging       =    0
  cfPolygon       =   40
  mnExtdSteps     =   15

[Optimize3]

  @Optimize2

  Active          =    1
  cfVia           =   80
  cfNonPref       =    2
  cfChangeDir     =    2
  cfPadImpact     =    0
  cfSmdImpact     =    0
  cfPolygon       =   50
  mnExtdSteps     =   10

[Optimize4]

  @Optimize3

  Active          =    1
  cfVia           =   60
  cfNonPref       =    1
  cfPolygon       =   60
  cfBase.16       =   12

[Optimize5]

  @Optimize4

  Active          =    1
  cfVia           =   40
  cfNonPref       =    0
  cfPolygon       =   70
  cfBase.16       =   14
  mnExtdSteps     =    5

[Optimize6]

  @Optimize5

  Active          =    1
  cfVia           =   20
  cfBase.16       =   16

[Optimize7]

  @Optimize6

  Active          =    1
  cfBase.16       =   18

[Optimize8]

  @Optimize7

  Active          =    1
  cfBase.16       =   20

I have been designing some PCBs recently and I would suggest you NOT to use auto-placer or auto-router for your final product. (Proteus has auto placer.)

First of all - Your software is as intelligent as an earthworm when it comes to auto placement or auto routing. In other words, it's dumb as a potato.

Auto routing would not know which placement will get you a better trace pattern which will enable you not only to make an efficient design but also to minimize noise in the circuit. Similarly auto routing doesn't know that shifting a component slightly to the left or right would enable you to route a track in a better way. These tools will just give you a design which is correct according to the circuit. But when it comes to real world performance, things are different.
For example:

• Decoupling capacitors should be physically close to the IC.
• There should be loops of least enclosed area.
• Ground plane should be as solid as possible.
• No interfering signals should be close to your crystal oscillator etc.

Your software won't respect these concepts because these are not mentioned in your schematic. You will know only when you have got the PCB manufactured and it doesn't work as expected all the time. I am not saying it won't work. It might work, for 90% of times but you have to take that 10% into consideration too.

My suggestions is that you should learn some PCB designing concepts and try placing and routing on your own. You can always post your schematic and board layout in forums and experts will give you their opinion/suggestions.