Re: gEDA-user: DRC/rat quirks
On Tue, Feb 13, 2007 at 04:06:34PM -0800, Harry Eaton wrote: which doesn't work for me even with snap to pad. That's pretty hard to believe. The connectivity is checked by a rigurous intersection test, no particular points are required, any touching will do. Ok, I saw contrary documentation, so I was assuming I was hitting a bug where nets had to end exactly on a pad. Originally it took a fair amount of compute resources to trace the connectivity - it still can with very large boards so updating the whole rats nest automatically was never really considered. You only need to update the ones for the net that's being routed... This sounds like a bug. Send me a test case and I will solve it. Do the source and target turn green when you start the trace? No... Come to think of it this coupled with your rats nest failure above strongly suggests your layers aren't assigned the way you think they are. I think that's it. I just built from CVS and I notice that I can repro my problem if I route on the wrong side. If I route on on the other side, things are much more sane. -- Ben Jackson AD7GD [EMAIL PROTECTED] http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
On Tue, Feb 13, 2007 at 11:28:16AM -0700, Andy Peters wrote: On Feb 13, 2007, at 8:37 AM, DJ Delorie wrote: Ben Jackson wrote: but I would like the ratsnesting to work in a sane fashion and I'd like auto DRC to let me actually draw traces to pads in the same net... Please be specific about which version and what bugs One bug/annoyance I can think of is when moving a footprint, with rats-nest enabled, the rats-nest lines don't move smoothly with the footprint. After you drop the part in the new location, you have to zoom in or out to clean up the rats-nest. That's one. Another is that the rats for a net don't go away unless you can get your line to end exactly the right place, which doesn't work for me even with snap to pad. Also, the rat wire should give visual feedback as you route a net -- rats to routed pads should disappear as you place tracks that complete segments. As for the DRC, I've played with a few boards. Each time I end up with at least one rat wire going between two pads which I can't route because the auto-DRC won't let me onto the second pad. This might be related to the fact that my wire didn't start at the right place, despite it starting on the snap point that caused the new line to exactly cover the rat... There's another thread going on where someone is concerned about trusting a new feature in PCB when fabbing a board. Well, it's all new to me, and I don't know if I trust it yet. Maybe it has fabulous internals and a quirky interface, or maybe the internals are just as quirky... I'm on PCB version 20060822 (the latest in fink) on OS X 10.4.8 on Intel. I'm on PCB version 20060822 (latest freebsd ports) on FreeBSD 4.9 on Intel, displaying to X.org. -- Ben Jackson AD7GD [EMAIL PROTECTED] http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
That's one. Another is that the rats for a net don't go away unless you can get your line to end exactly the right place, which doesn't work for me even with snap to pad. I'd like to see a test case for this. Also, the rat wire should give visual feedback as you route a net -- rats to routed pads should disappear as you place tracks that complete segments. With the lesstif HID, you could call the rats-optimize action on each mouse button release ;-) As for the DRC, I've played with a few boards. Each time I end up with at least one rat wire going between two pads which I can't route because the auto-DRC won't let me onto the second pad. It's also sensitive to which side you started on. Start on the pad that's already wired in, and connect to the one that isn't. Also check your netlist. Still, a test case would help. Me, I don't use auto-drc. I use the 'o' key to tell me when I screwed up, plus the 'f' key to highlight what I'm *supposed* to be routing to. There's another thread going on where someone is concerned about trusting a new feature in PCB when fabbing a board. Because the postscript and pdf prints, on screen, have faint lines between slices, and I didn't know if the DRCbots were going to complain about them. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
Ben Jackson wrote: There's another thread going on where someone is concerned about trusting a new feature in PCB when fabbing a board. Well, it's all new to me, and I don't know if I trust it yet. Maybe it has fabulous internals and a quirky interface, or maybe the internals are just as quirky... The output from PCB is very predictable. I've always gotten accurate results from either my laser printer or the fab house. Never a problem. If you feel like the interface is odd, it is. It is raw. Because of this maybe there's a case for trusting it _more_? Phil Taylor ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
- That's one. Another is that the rats for a net don't go away unless you can get your line to end exactly the right place, which doesn't work for me even with snap to pad. That's pretty hard to believe. The connectivity is checked by a rigurous intersection test, no particular points are required, any touching will do. Implied in your statment is that after making a connection and optimizing the rats nest (o key), a rat line suggests the connection you just made is not making connection. I'd really like to see a test case because I've never seen this behavior ever. Also, the rat wire should give visual feedback as you route a net -- rats to routed pads should disappear as you place tracks that complete segments. Originally it took a fair amount of compute resources to trace the connectivity - it still can with very large boards so updating the whole rats nest automatically was never really considered. I think that most computers are fast enough now that its a viable idea to add an optional setting to optimize the rats nest after every move, track addition, track deletion etc. That would make the rat disappear as soon as the connection was made. As for the DRC, I've played with a few boards. Each time I end up with at least one rat wire going between two pads which I can't route because the auto-DRC won't let me onto the second pad. This might be related to the fact that my wire didn't start at the right place, despite it starting on the snap point that caused the new line to exactly cover the rat... This sounds like a bug. Send me a test case and I will solve it. Do the source and target turn green when you start the trace? Come to think of it this coupled with your rats nest failure above strongly suggests your layers aren't assigned the way you think they are. There was a release where some default layer names (which are nothing more than names and could well be foo and bar) were something like component and solder while they were actually grouped to the opposite side. Check your layer groupings. There's another thread going on where someone is concerned about trusting a new feature in PCB when fabbing a board. Well, it's all new to me, and I don't know if I trust it yet. Maybe it has fabulous internals and a quirky interface, or maybe the internals are just as quirky... pcb has a long history. For many years it was very stable and very reliable. This past year we have made so many sweeping changes including completely replacing all of the user interfaces and major changes to much of the code internals too. Some level of skeptisism is warranted because of this. With that said I think the latest snapshot release should be pretty stable. Any questions? Get answers on any topic at www.Answers.yahoo.com. Try it now. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
Because the postscript and pdf prints, on screen, have faint lines between slices, and I didn't know if the DRCbots were going to complain about them. Strange. I'm sure the postscript is drawing those faint lines but they shouldn't be visible since they are on top of or beneath a solid fill. (The slices share a common edge where the line appears.) Does your printed postscript show those lines (or worse gaps)? Don't pick lemons. See all the new 2007 cars at Yahoo! Autos. http://autos.yahoo.com/new_cars.html ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
Strange. I'm sure the postscript is drawing those faint lines but they shouldn't be visible since they are on top of or beneath a solid fill. (The slices share a common edge where the line appears.) Does your printed postscript show those lines (or worse gaps)? The prints appear OK. Both ghostview and acroread have faint white lines between the slices, and not always - it depends on the zoom factor. I suspect it's due to the antialiasing since it only happens when antialiasing is on, but it makes me wonder if these edges shouldn't be overlapped by a bit (1/100 thou?) or not. I also don't know what the fab's DRC/DFM would do with the thin slices or just-touching edges. gerbv seems to draw it OK too. I wouldn't have been too concerned about it except that these are internal layers on my board, so I can't visually inspect the results from the fab. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: DRC/rat quirks
For instance, you must turn it off if you are placing a via to connect traces to finish off a rats nest, even if the rats are displayed properly. Ok, I can reproduce this. PCB expects you to do something else. What it wants is for you to draw the line off the first pin, change layers, and continue drawing lines. It puts in the vias for you whenever you change layers. You should be able to connect to vias that are already connected to the net through other lines, though. It's just totally unconnected vias it's blocking. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
