New to PCB design - why doesn't auto placing components exist?

Question

The circuit design software I have seen has the ability to automatically route traces etc. on a PCB.
But why doesn't this software have the ability to automatically place components on a PCB say to minimise total board size?
Is this just too complicated to be automated?

Answer 1

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.

Answer 2

One thing you're not considering is that a schematic does not contain enough information to lay out a board properly.

Basically, the PCB layout requires consideration and accommodation for a few dozen layout requirements per part, none of which are codified in the schematic. Consider just the bypass capacitors. To have an automated system properly place the bypass capacitor for each component, you'd need to have some additional directives on the schematic that dictate to the autorouter that the trace between the two nodes must be below a certain length.
Presumably, you'd then need further directives to encode the priority of length minimization for various nets, something to dictate differential pairs/controlled impedance, guard traces (if needed), etc...
Basically, there are a lot of additional variables that drive the placement that are usually not encoded at all in schematic/ratsnest documents.

Furthermore, even if you assume that you have all of the above design constraints, the sheer size of the problem space for a common layout is enormous. It's the equivalent of trying to solve a equation with thousands of inputs, where every input has a different, non-linear effect on all the others. Effectively, the problem is completely intractable from a brute-force perspective. Any solution must therefore involve some sort of heuristic mechanism, which has it's own complexities.

---

Realistically, the primary reason there aren't at least better autorouters is that there's just no market. The EDA market is comparatively small in comparison to many other niche, special purpose software markets, and even the best autorouter ever won't even approach a real layout by an actual human.

When in the midst of a particularly boring layout, I usually have some fantasies of trying to design my own autorouter, by doing something with vector fields and simulated annealing, but even that would only approach a local optimum, rather then a general optimum layout.

Answer 3

My router has a placer and support for "rooms". That let's you draw areas and assign parts to "rooms" from the schematic. The auto placer will group them together in the room the part is assigned to. Pretty sure it has support for this connector should go to this location too. There's also a tool that can do automatic decoupling placement and part selection/optimization based on simulation results. It's not cheap though :) but it does work.

The auto placer can save you a little time by placing everything together like that. But I still prefer cross probing the schematic to the layout in place mode.

Just like the auto router you get out what you put in in terms of constraints and how well you can use it. If you just try to use your auto router without constraining it properly it just routes everywhere. When set up properly we use it to correctly route large matched length DDR sections. On much larger and denser boards it's almost a necessity, and certainly a requirement for a layout services shop that needs the speed. However these things might not be worth it for someone doing only a few small boards a year.

Answer 4

Back in 1974-1975 I worked in the Design Automation department at Honeywell. The problem hasn't changed since then:

1. It's not computationally feasible to optimize. Like most global optimization problems, it's NP-Complete, meaning the complexity of the computation grows horribly quickly. Since you can't wait around for a trillion years (or worse), we can regard the optimal solution as being impossible to find.
2. It's unclear to the program just what you want to optimize. Logical grouping according to your model of the circuit organization? Trace length? Board area? Parasitic coupling? Propagation delay? Thermal dissipation (max temp)? Thermal bleed from higher-power sections to temperature-sensitive components? RF emission? Noise? Mechanical properties (for example, placing more massive components near the mechanical supports? Service characteristics, like not putting on-board connectors closer together than human fingers can manage? External constraints, like connector locations, or fitting within the available space (no conflicts with cases, fans, etc.)

There are AI-based approaches to dealing with problems like this. However, at some point, it is easier for the designer to just try things, and get feedback from the software as to the design criteria he's interested in. Telling AI software everything you know can be an endless, thankless task. Ultimately, the software has to satisfy you, the designer, and your set of tradeoffs.

The best way for this to work, then, is to view it as a collaboration between designer and software, with the designer making the final decisions. The software can provide information about the properties, and can suggest ways to improve a property of interest, and help explore the consequences of a change.

But I predict we will never, ever, see fully-automated layout -- so long as we have humans looking at and caring about the result.

Answer 5

My software has a placer. I ran it one time just to see what would happen. It went rip roaring through the board, and got all of the components on it. When I looked at it, parts were EVERYWHERE. The IC was in one corner, and its decoupling cap was in the other. The critical path zig-zagged back and forth across the board.

My point here is placement is hardest part of the layout to get right. First there are the mechanical constraints. The ME/industrial designer wants your connector/switch/pot/LED/whatever other external interfacing component to come off the board at a certain spot. Some components may be too tall to be in certain areas inside the enclosure. There may be parts of the circuit that need to keep a certain clearance for isolation.

Software can be configured to deal with some of these factors, but it will never do as good a job, or be able to visually see problems the way a human can. In a perfect world, if you get placement right, do power, ground, and critical path routing, a quick pass of the autorouter should be able to finish the layout off.

Answer 6

I have used auto-placers before, and they are indeed as dumb as a pile of rocks. About the only thing you can sanely use them for is for untangling a pile of footprints that all were imported into your board at the same place on it; anything else is simply too much to ask.