Re: gEDA-user: pcb: Track routing strategies and tips
The schematic should be as readable as possible. Clearly you do not work where I do :) (or as some folks say "there you go, making sense again") > Preferred signal direction is left to right, top to bottom. Me too, whenever possible. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
Stephan Boettcher wrote: > My schematics usually look almost like the layout. The pins of the > symbols are placed like on the package. When in doubt, my design works the other way. The schematic should be as readable as possible. Preferred signal direction is left to right, top to bottom. If no other constraints are imposed, my layout look roughly like the schematic. This is convenient when debugging. ---<)kaimartin(>--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmk&op=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
Colin D Bennett wrote: > (It would be fantastic if pcb could adjust traces > dynamically as components are moved.) One of my favorite daydreams during manual routing: A plugin that handles all all tracks like tensioned rubber band. Then let go of the components and TWANG! --> The board area shrinks to minimum dimensions. :-) ---<)kaimartin(>--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmk&op=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
Colin D Bennett writes: > As a rather inexperienced PCB designer, I find that I have to throw > away two or three layouts until I get one that is usable--and still > not entirely satisfactory. I always end up with such a mess of traces > that I know I need better organization and a method to the madness. > But I am a newb with little knowledge so I fall back on trial-and-error. > > Does anyone have any tips on how to plan a layout for easy and clean > track routing? In particular for 2-layer boards. My schematics usually look almost like the layout. The pins of the symbols are placed like on the package. People on this list argue that the schematic should document the function, not the physical implementation, but in my circuit the function is all inside the FPGA and the processor, while the details of the layout in low noise mixed signal or high-speed applications are very important, so I use the schematic entry as a first opportunity to preview the place and route. > One strategy that I have seen and recently tried is to use the top > layer for all horizontal trace runs and the bottom layer for all > vertical trace runs, or vice-versa. This is a good for (slow) digital designs. These typically benefit from good functional schematics for review and documentation, so my physical style of schematics is not appropriate. OTOH, when it needs to fit on two layers, and the logic is not too complicated, a little physical planing on the schematic level may help later with the placement and save a few backannotation cycles for swapped pins and slots. > Do you ever use the pcb autorouter or do you always route by hand? I never tried an autorouter. But for that kind of Manhattan routing I probably would try. > Do you ever study other people's PCB designs to learn from them? I > think you could find both good and bad examples: things to emulate and > things to avoid yourself. Yes. -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
On Tue, 10 May 2011 21:58:57 -0400
gene glick wrote:
> Kai-Martin posted that placement is more important than routing. I'd
> say they are equally important. The best layout guy in the world
> can't fix a lousy placement. Bogus layout guys throw more layers at
> the problem. So yeah, take the time to plan it out before routing.
One problem I have with placement is guessing how far apart to place
components. If I do the routing and then realize I could shrink the
board, it is really painful to do so since all the traces (lines) will
not scale or move usefully with the components. So basically if I move
a component I need to then re-route a significant part of all the traces
connected to it. (It would be fantastic if pcb could adjust traces
dynamically as components are moved.)
> > Does anyone have any tips on how to plan a layout for easy and clean
> > track routing? In particular for 2-layer boards.
>
> No substitute for experience here. But, partitioning the design by
> type may help : analog, digital, low-speed, high-speed. Try to think
> beyond blindly connecting the parts. Sometimes swapping gates,
> adding parts or other strategies become clear as you route. This is
> a huge benefit when you route your own board. Layout guys just
> connect the pieces together.
Rather than a strict two-step process of (1) schematic capture and
(2) PCB layout, I have recently found an iterative-design process loop
of "do { edit_schematic(); edit_pcb(); } while (!satisfied);" to be very
helpful, for instance when there is a choice of connector pinout or
microcontroller I/O pin usage. I often find that if I switch the MCU
I/O pins used for a connection it really cleans up part of the layout.
> > One strategy that I have seen and recently tried is to use the top
> > layer for all horizontal trace runs and the bottom layer for all
> > vertical trace runs, or vice-versa.
>
> 2-layer is tough. You also have to account for power and ground.
> The parts themselves also crowd routing area. 2-layer is not
> particularly suitable for high-speed anything. Seems good for power
> supply design, and some audio work (I've seen a lot of audio ref
> boards on 2 layer). You can make good designs with 2-layer, just is
> more work. Cost difference to 4-layer is not bad.
At least for DorkbotPDX/pcb.laen.org, 4-layer is double the cost of
2-layer per unit area. However I guess you could do the board in a
smaller area with 4-layer so the final cost would actually be less than
double that of the 2-layer design.
> > Do you ever study other people's PCB designs to learn from them?
> Yeah, a lot. You will find good and bad. There's a whole world of
> opinion out there - and you know what they say about opinions :)
> SI-LIST is a great place to exchange ideas on layout. Several
> industry experts frequently post.
I am checking out SI-LIST now. Sounds interesting.
Regards,
Colin
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
On Wed, 11 May 2011 02:26:43 +0200 Kai-Martin Knaak wrote: > Colin D Bennett wrote: > > > Does anyone have any tips on how to plan a layout for easy and clean > > track routing? In particular for 2-layer boards. > > Put extra care into component placement. IMHO, placement is more > critical to the design than routing. I have heard this advice often. > > Do you ever study other people's PCB designs to learn from them? > > Sometimes I look with awe at computer motherboards ;-) I originally commented in my message at this point about how I found it interesting to examine computer motherboards (but decided to delete it). There is so much to those boards! Some of the vias are nearly microscopic (laser-drilled, I guess). One thing I recently discovered was the trace length matching in the SDRAM signals. Some beautiful PCB design. I've practiced my hot air rework skills with some old motherboards and studied their design while at the same time salvaging some nice connectors, inductors, etc. Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
I start off with schematics. People underestimate the need for a clear schematic. On the schematics, I tend to place components approximately where they will appear on the PCB. This gives me an idea of how traces are to be routed. I divide my schematics into virtual blocks - not actually marked on the schematic. For example one block would be a 3.3V buck powrer supply; another might be a 9DOF sensor area (mag/acc/gyro.) When it comes to a layout, I place major components first and attempt to fit the smaller blocks into the free space as long as traces are kept short. I rarely if ever use the autorouter, even on complex designs. No autorouter, no matter how good, can work as well as routing by hand, in my honest opinion. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
On Wed, May 11, 2011 at 02:26:43AM +0200, Kai-Martin Knaak wrote: > Colin D Bennett wrote: > > > Does anyone have any tips on how to plan a layout for easy and clean > > track routing? In particular for 2-layer boards. > > Put extra care into component placement. IMHO, placement is more > critical to the design than routing. Indeed. I've been told y a professional (her job is to lay out PCB with expensive commercial tools) that she has never seen a good or even acceptable automatic placer. However she claims that automatic routers are now reasonably good, far from perfect, but the help. I have very similar problems in FPGAs: I often can only reach the performance I want when helping by fixing the location of the large blocks (mostly RAM and DSP). > > > > One strategy that I have seen and recently tried is to use the top > > layer for all horizontal trace runs and the bottom layer for all > > vertical trace runs, or vice-versa. > > Yep. This is a good default. It avoids road blocks by tracks on > both sides. It's called Manhattan routing. It's a good starting point, but you should at least perform some via reduction run at some later stage. > > > > Do you ever use the pcb autorouter > > Rarely. Basically only for fun... > > > > or do you always route by hand? > > Mostly. Always in practice, but that's because my circuits are simple but almost invariably involve microstrip and/or coplanar line for the most important signals (and mechanical design of the enclosure is as critical as the PCB layout). I'm in the process of designing a much more complex board with FPGA, DDS and no real high frequency signal (highest frequency being the 400MHz DDS clock). But the layout is going to be done by the person mentioned above (using CadStar at the moment). BTW, there is no gschem->CadStar netlister, or did I miss it? Gabriel ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
On Tue, May 10, 2011 at 04:26:06PM -0700, Colin D Bennett wrote: > As a rather inexperienced PCB designer, I find that I have to throw > away two or three layouts until I get one that is usable--and still > not entirely satisfactory. I always end up with such a mess of traces > that I know I need better organization and a method to the madness. > But I am a newb with little knowledge so I fall back on trial-and-error. > > Does anyone have any tips on how to plan a layout for easy and clean > track routing? In particular for 2-layer boards. > As a hobbyist, I work mainly with 2-layer boards, since those are what I can make at home. This means that I also minimize the number of vias I use, which presents its own challenges. My latest pcb is here: http://wpsoftware.net/andrew/stereo_bike.pcb This was also interesting because I was space-constrained (the board needs to fit into a small cast iron box on my bicycle) and since this is a high-powered audio application, I needed large power traces and a lot of heat sink. As has been said, experience is a huge factor in laying out boards. Don't be afraid to rotate things 180 and try odd ways of connecting components. Using source control on PCBs is a good idea. Do things locally (in my case, the power supply, main amp and guitar pre-amp were all laid out separately) and worry about connecting them later. Figure out how to avoid intersections before spacing things out. If you get stuck, it can help to decide ``I'll just use a jumper wire here'' and move on. Often problems are easier to solve once more of the board is in place. > One strategy that I have seen and recently tried is to use the top > layer for all horizontal trace runs and the bottom layer for all > vertical trace runs, or vice-versa. > > Do you ever use the pcb autorouter or do you always route by hand? > The autorouter uses too much space in my experience and isn't good at deciding what trace widths to use. > Do you ever study other people's PCB designs to learn from them? I > think you could find both good and bad examples: things to emulate and > things to avoid yourself. > Yes :) fortunately, in my line of work I am also often able to ask the designers of said boards what they were thinking. > Thanks for any suggestions. There are some incredibly experienced and > talented electronic designers on the list and I'd love to learn > anything I can from you all. > -- Andrew Poelstra Email: asp11 at sfu.ca OR apoelstra at wpsoftware.net Web: http://www.wpsoftware.net/andrew/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
Colin D Bennett wrote: As a rather inexperienced PCB designer, I find that I have to throw away two or three layouts until I get one that is usable--and still not entirely satisfactory. I always end up with such a mess of traces that I know I need better organization and a method to the madness. But I am a newb with little knowledge so I fall back on trial-and-error. I am also new to routing my own stuff but have a bunch of experience telling others how to do it for me (day job ;) On a prior job, the layout house did all auto-routes. They'd start several jobs with different router restrictions, allow them to route for a while, then pick one, and optimize it - probably by hand. Yes, starting over is common. Kai-Martin posted that placement is more important than routing. I'd say they are equally important. The best layout guy in the world can't fix a lousy placement. Bogus layout guys throw more layers at the problem. So yeah, take the time to plan it out before routing. Does anyone have any tips on how to plan a layout for easy and clean track routing? In particular for 2-layer boards. No substitute for experience here. But, partitioning the design by type may help : analog, digital, low-speed, high-speed. Try to think beyond blindly connecting the parts. Sometimes swapping gates, adding parts or other strategies become clear as you route. This is a huge benefit when you route your own board. Layout guys just connect the pieces together. One strategy that I have seen and recently tried is to use the top layer for all horizontal trace runs and the bottom layer for all vertical trace runs, or vice-versa. 2-layer is tough. You also have to account for power and ground. The parts themselves also crowd routing area. 2-layer is not particularly suitable for high-speed anything. Seems good for power supply design, and some audio work (I've seen a lot of audio ref boards on 2 layer). You can make good designs with 2-layer, just is more work. Cost difference to 4-layer is not bad. Yes X-Y routing is the way to go to avoid blocking. Works great for digital stuff. Do you ever use the pcb autorouter or do you always route by hand? I have yet to make the auto router work - but haven't really tried very hard. Hand routing is my preference but it takes longer. Do you ever study other people's PCB designs to learn from them? Yeah, a lot. You will find good and bad. There's a whole world of opinion out there - and you know what they say about opinions :) SI-LIST is a great place to exchange ideas on layout. Several industry experts frequently post. gene ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb: Track routing strategies and tips
Colin D Bennett wrote: > Does anyone have any tips on how to plan a layout for easy and clean > track routing? In particular for 2-layer boards. Put extra care into component placement. IMHO, placement is more critical to the design than routing. > One strategy that I have seen and recently tried is to use the top > layer for all horizontal trace runs and the bottom layer for all > vertical trace runs, or vice-versa. Yep. This is a good default. It avoids road blocks by tracks on both sides. > Do you ever use the pcb autorouter Rarely. > or do you always route by hand? Mostly. > Do you ever study other people's PCB designs to learn from them? Sometimes I look with awe at computer motherboards ;-) ---<)kaimartin(>--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: pcb: Track routing strategies and tips
As a rather inexperienced PCB designer, I find that I have to throw away two or three layouts until I get one that is usable--and still not entirely satisfactory. I always end up with such a mess of traces that I know I need better organization and a method to the madness. But I am a newb with little knowledge so I fall back on trial-and-error. Does anyone have any tips on how to plan a layout for easy and clean track routing? In particular for 2-layer boards. One strategy that I have seen and recently tried is to use the top layer for all horizontal trace runs and the bottom layer for all vertical trace runs, or vice-versa. Do you ever use the pcb autorouter or do you always route by hand? Do you ever study other people's PCB designs to learn from them? I think you could find both good and bad examples: things to emulate and things to avoid yourself. Thanks for any suggestions. There are some incredibly experienced and talented electronic designers on the list and I'd love to learn anything I can from you all. Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
