Which PCB Packages Offer Circuit Testing / Emulation?

[thermionic]

Hi,

I recently read here that Eagle now imports PSpice files. Good, but is there a package which carries the circuit emulation through to the PCB layout itself?

Obviously, circuit emulation itself is no substitute for building the real thing (none of the designers I know rely on emulation - they're invariably quite scathing about it and start telling you to knuckle down and make a breadboard). It might be a little too much to ask for a package to analyse potential for parasitics and x-talk (although not unreasonable?) etc, but what about one that simply checks the PCB is a faithful transcription of the schematic? One that makes sure -ve is connected to -ve - and that you haven't flipped phase on one channel etc..

Having spent many hours with scalpel and iron, debugging faults on PCBs due to human error, such a piece of software would be revolutionary to me. Which package does it? Is it relatively affordable?

Thanks in advance. 

 

[gemini86]

Kicad has a DRC check that makes sure the layout matches the schem perfectly, shows the missing connection, also shows how many connections are yet to be made.

Other than that, I don't think anything like that exists that's cheap. There are some autorouting software that know all the important layout and routing rules and can layout a PCB better than the average engineer, in less time. Those are usually thousands on thousands of dollars, making it only really feasible for, say, computer component design.

 

[Andy Peters]

Hi,

I recently read here that Eagle now imports PSpice files. Good, but is there a package which carries the circuit emulation through to the PCB layout itself?

Obviously, circuit emulation itself is no substitute for building the real thing (none of the designers I know rely on emulation - they're invariably quite scathing about it and start telling you to knuckle down and make a breadboard). It might be a little too much to ask for a package to analyse potential for parasitics and x-talk (although not unreasonable?) etc, but what about one that simply checks the PCB is a faithful transcription of the schematic? One that makes sure -ve is connected to -ve - and that you haven't flipped phase on one channel etc..

Having spent many hours with scalpel and iron, debugging faults on PCBs due to human error, such a piece of software would be revolutionary to me. Which package does it? Is it relatively affordable?

Thanks in advance.

You're asking for a tool to do several different checks.

Standard DRC can handle testing to make sure outputs don't connect to outputs and the like.

Pretty much any non-toy package "checks [that] the PCB is a faithful transcription of the schematic" because you start with a schematic and generate the netlist for layout from that schematic. As long as you don't do anything dumb like modify the netlist in the PCB and not back-annotate it to the schematic, it'll be correct. You should get into the habit of giving each and every signal a proper net name rather than rely on the tools to generate them for you; this way, making mistakes connecting different nets together becomes quite difficult as the DRC will complain.

Of course you need to add design rules for things like trace widths and spacing.

"Checking to see if you've flipped phase on one channel?" Well, the schematic has no knowledge of polarity or phase, but many packages support multichannel hierarchical designs where you draw a schematic for one channel and it gets replicated for as many as you need. So there's no way to have one channel wrong.

As for checking for parasitics and crosstalk, you need an IBIS signal-integrity simulation tool and models of your various parts. Altium Designer does that quite handily, actually, and Hyperlynx can read other vendors' PCB layouts and do signal-integrity simulation on them. Not free, and I haven't seen a low-cost signal-integrity simulation tool. (And I haven't seen IBIS models of the usual things we see in audio circuits, anyway.)

-a

 

[abbey road d enfer]

Hi,

I recently read here that Eagle now imports PSpice files. Good, but is there a package which carries the circuit emulation through to the PCB layout itself?

If I understand correctly, you want a simulator that works from the same netlist as your PCB package. Importing a netlist from a Spice program won't help you because your PCB software wants to know in what package your components are. Many editors offer a complete PCB/sim package but they are much more expensive than the Eagle/LTspice combo. Unfortunately Eagle netlists are not usable by LTspice (you may prefer LISA). The penalty is that you have to do two schemos, one for eagle and one for LTSpice, and sure, there are risks of errors.

Obviously, circuit emulation itself is no substitute for building the real thing (none of the designers I know rely on emulation - they're invariably quite scathing about it and start telling you to knuckle down and make a breadboard). It might be a little too much to ask for a package to analyse potential for parasitics and x-talk (although not unreasonable?) etc, but what about one that simply checks the PCB is a faithful transcription of the schematic? One that makes sure -ve is connected to -ve - and that you haven't flipped phase on one channel etc..

Eagle does it well, it has a DRC that checks consistency between schemo and layout.
It won't tell you the bandwidth and distortion (LTspice takes care of that) but only a specialised software will be capable of dealing with parasitics, unless you back-annotate your simulation with all the stray capacitances of the PCB.  :'(

Having spent many hours with scalpel and iron, debugging faults on PCBs due to human error, such a piece of software would be revolutionary to me. Which package does it? Is it relatively affordable?

If you mean layout errors, like non-connected pins, wrongly-connected pins, overlaid tracks, the DRC takes care of that. Even the basic version of Eagle has it.
Your layout cannot "more correct" than your schemo, though.

 

[ramshackles]

You can get stuff like this:

http://www.mentor.com/pcb/

which will do DRC's and also EM, thermal and signal integrity analysis to help you create the 'best' layout...

Probably not cheap though. Clearly too expensive for them to say how much online...

 

[abbey road d enfer]

You can get stuff like this:

http://www.mentor.com/pcb/

which will do DRC's and also EM, thermal and signal integrity analysis to help you create the 'best' layout...

Probably not cheap though. Clearly too expensive for them to say how much online...

You can also expect a VERY steep learning curve.

 

[ruffrecords]

You can get stuff like this:

http://www.mentor.com/pcb/

which will do DRC's and also EM, thermal and signal integrity analysis to help you create the 'best' layout...

Probably not cheap though. Clearly too expensive for them to say how much online...

You can also expect a VERY steep learning curve.

And expect to spend a lot of time there when you reach the top. Mentor systems are the sort that need a full time employee to get the most out of them.

Cheers

Ian

 

[Matador]

Parasitic extraction tools are common in the high power (a.k.a. high cost) layout realms, especially at the chip level.  I know of no hobby-grade tools to do this.

But as with everything, you need to think about/know which nodes are sensitive to this stuff.  When I was doing my C12 layout, I knew that frequency response involving high-impedance nets could be clobbered by parasitic capacitances of even a few pF.  If you know the trace width/thickness, PCB material (which gives the dielectric constant) and thickness, etc, you can use many free online calculators to give you a rough indication of the parasitic capacitances.  You can then add these elements into your simulation.  I think you'll find that for most things audio (the frequencies and impedance we typically work with), <handwavey>these effects are mostly negligible</handwavey>.  I would hazard to say investing the same effort in ground routing will pay back many more dividends than extracting and manually adding 2pF stray caps into an API312 design.

However most of these online tools assume an infinite ground plane and no fringing effects, etc.  But it's a good / free place to start.

 

[thermionic]

Thanks to all of you. Much food for thought!

 

[pucho812]

Check out Proteus by labcenter. It does drc, it does spice simulation on most of the parts and does easy incorporation of the captured schematic to PCB layout. worth looking at for sure.