Cheap Schematic Capture

Not at $60 and hour it wouldn't, since I would already have done the work. Can I have some sensible answers please.

Dirk

Do you need a PADS schematic, or just a PADS netlist?

gschem has a PADS netlister if you just need a netlist, and gschem (part of gEDA) is free (beer-wise and speech-wise). (and no, it won't force you to distribute your schematics)

Thanks Not sure which one I need - I'll have to talk with the layout guy. However, it's got to be Windows. That's all we have here. I've tried using Linux in the past but its a real pain.

Dirk

So use gschem under windows.

I've not used PADS, but have used Protel almost daily for the last 8 years, and OrCAD before that. If PADS works in a similar fashion, then you won't really be helping.

I've also had people generate schematics for me in Protel thinking they were saving me time. It doesn't. Not unless you have my libraries. Regardless of how pretty the schematic is, I will always have to completely redraw it to work with my existing libraries which are usually not drawn is the same way as the client would have. Since the library part defines the footprint it'll always need redone. Incidentally, I can import schematics from several other CAD packages, but would never use it for anything other than a template to help redraw the schematic. Imported schematics never seem to work in the same way as a natively drawn one.

Seriously, just give him what you have and let him do his part without the constraints of a crappy imported schematic.

Chris

Dirk, There is a lot of truth in what Chris says. If you do it, nothing says that your schematic symbols will match up properly with the designer's footprint library. When there is a error, who's fault is it? So the designer either has you sign-off with a warning of his fears and the unknown nature of the interface between the two realms (schematic/pcb), or the designer has to trouble shoot and delve into each and every part in your schematic to make sure there are no hidden gotchas hiding just below the surface.

-- Sincerely, Brad Velander.

You really need the schematic program that he's using, along with the libraries. Otherwise the components almost certainly won't match up, and he'll have to spend a lot of time converting them. It's a real pest that there's practically zero interoperability between different CADs, and one place where a European directive would be useful, if they could be trusted not to screw it up.

"Dirk Bruere at NeoPax" a écrit dans le message de news: snipped-for-privacy@q77g2000hsh.googlegroups.com...

It's not free but it's not expensive : we currently use Labcenter's proteus suite

for schematics and simulation, and then export the netlist in a standard Tango format when we don't to the routing ourselves under Proteus. Our industrial partner has no problem to import them in PADS but as someone said they have then to manually remap each component to the corresponding footprint in PADS libraries.

Hopes that helps, Robert

Paul, I wouldn't concur with your statement of needing the same program. For many years I used OrCAD schematic with PADs, then Protel for Windows replaced the OrCAD, still with PADs. Many years ago I used OrCAD with Maxi-PC. You do need a progam that will export a simple compatible netlist of one form or another. The more critical part is the synergy between the schematic symbols and the PCB footprints. That synergy is buitl itno the symbols simply by exchange of information and the standards used for pin numbering on any devices not already covered by an accepted standard. (i.e. SOT-23s, DPaks, SOT-223s, etc. The parts where some pin numberings differ.) For the OP to learn the package he obtains, apply all the standards correctly, get matching symbols and a compatible netlost output would be a tall order. Not impossible but surely a lot slower and riskier process than just having the PCB designer do it. The PCB designer is undoubtedly familiar with his own tools bringing much more sped and value to the process.

--
Sincerely,
Brad Velander.

"Paul Burke"  wrote in message 
news:61flubF1v425sU1@mid.individual.net...
> Dirk Bruere at NeoPax wrote:
>> Hi
>>
>> I\'m looking for a cheap (or free!) schematic capture package that can
>> output in PADS format. I\'m not the layout guy but it will certainly
>> save him time compared with me drawing out the circuit in a normal CAD
>> package. Pin count around 1000 at present.
>
>
> You really need the schematic program that he\'s using, along with the 
> libraries. Otherwise the components almost certainly won\'t match up, and 
> he\'ll have to spend a lot of time converting them. It\'s a real pest that 
> there\'s practically zero interoperability between different CADs, and one 
> place where a European directive would be useful, if they could be trusted 
> not to screw it up.
>

"Dirk Bruere at NeoPax" a écrit dans le message de news: snipped-for-privacy@q77g2000hsh.googlegroups.com...

Hi Brad,

OrCAD/PADS seems to be a popular combination, at least on the west coast here.

Let me add to your informative post: While it certainly is viable to use a different schematic capture and PCB package, what you normally lose includes:

-- The ability to "trivially" (quickly) swap equivalent gates within a package or equivalent pins within a gate. Most PCB/schematic capture packages can do this with "is/was" files *and the PCB guy having knowledge of what the allowable swaps are* (this information is in the schematic library files but not a PCB netlist), but this makes it somewhat klunkier (slower) to get done.

-- The ability to apply various layout rules based on net class. E.g., your have your clock net class, your differential pair net class, your power net class, etc. and the PCB package automatically sets the right defaults (clocks might need to be routed point to point rather than in a home-run topology, power nets are far, diff. traces have matched lengths, etc.) This can sometimes be overcome with 3rd-party software -- for OrCAD/PADS Prescience

seems to be the well-known, get-out-your-checkbook-and-weep solution. For small designs going around and defining a bunch of net classes usually isn't that big of a deal since the PCB guy can just go around and do the same thing in his tool... for big designs schematic capture and PCB layout are potentially far enough removed that you'd really prefer to have the schematic "drive" the layout with such rules.

---Joel

On Thu, 14 Feb 2008 04:23:39 GMT, "Brad Velander" wrote: [Fixed top posting]

I agree with Brad. Most PCB packages can also export a netlist based on the actual routed tracks. This netlist can then be compared with the orignal netlist exported from the schematic package. If a suitable netlist format is chosen, then it does not take too long to manually compare the netlists and hence ensure that the PCB represents the schematic.

Regards Anton Erasmus

Joel, Your points are valid but I think it is far exceeding the OP needs/knowledge. Would you really think that he is going to do even a quarter of all that? And the PCB designer can swap gates manually and then ink ammend the schematics if the OP does the schematics.

But addressing some of your actual comments, yes OrCAD was very popular as a front-end for PADs. That is because back in it's day the PADs Logic was a horrible clunky program. As a matter of fact it still is today but now Mentor charges $1500 for it when PADs couldn't give it away free back in the

90s. Actually they did give it away free, but typically nobody would use it.

The part swapping is most dependant on the schematic packages ability to read it back in. OrCAD could read back the PADs Was/Is file.

-- Sincerely, Brad Velander.

Hi Brad,

I expect the O.P. actually would make great use of fast & easy gate/pin swapping if available in the program he's using, and there's a decent chance he'd set up at least a few rudimentary net classes ("Power" & "Signal" are always favorites), but other than that, no, he won't likely be using many of those high-end features. My post was more just to provide some of the "bigger picture" for his own edification.

(My experience with gate/pin swapping is that pretty much everyone does it if the layout program has the knowledge of the various legal swaps -- or has a feature to try to optimize the rat's nest by automatically performing these swaps, as Pulsonix and some other programs can -- whereas if you have to manually tell the layout package "swap pin 2 and 3" or "swap pins 1, 2, and 3 with 7, 6, and 5" a lot of people won't bother since it's more effort than just making a slightly "messy" route instead.)

---Joel

Joel, Your impression of the OP was obviously greater than mine. I sensed that he was at best a hobbiest but since he didn't already have a tool, I surmised that most tools and functions would simply bog him down. Not to say that he may not be very intelligent, I just know how the average person gets bogged down learning the nuances of a CAD program and most don't do get it right when they do get through it.

As for pin/gate swapping, I never use the automatic features because they don't intelligently apply any details about the routing, just simple manhattan distance minimizations. Which are usually definitely not routing optimized and no software can do that that I have seen.

-- Sincerely, Brad Velander.

Hi Brad,

Agreed, although I often find that Manhattan-distance optimized pin/gate swapping is *closer* to "routing optimized" than just whatever happens to pop out from the schematic in the first place.

I have a great deal of respect for really good PCB layout guys (of which I'm not one :-) )... it's amazing what they can "see" just by looking at a rat's nest relative to most people.

---Joel

Try

then :p

Anyway both KiCad and gEDA/gschem is available in both win32 & Linux