once i generate the netlist and start to do routing and lets say after some time may be i have had completed 50% routing if i add/change some simple circuit in my schematics i must regenerate the netlist which means do i need to do the routing from the beginning again. or is there a way to append to my old routing/pcb design.
is there any standard to be followed like what must be via diameter,via drill uvia diameter,uvia drill, track width for different type of signals, and clearance can some one please help me on this one.
Just export a new netlist from schematic and import it into the layout. As long as footprint references don’t change the they will stay where they are. Routed nets will stay too as long as such net exists in the netlist. You can even keep footprints and track that are not in the netlist anymore.
i just do not want to see the wire running from the components to components is there a option to disable the wires/netlist in pcbnew tool once i separate all the components then it would be easy for me to see all component then i can enable the netlist/wire running from one device to another
Hehe… click on the “Mode Footprint” button in the top tool bar in pcbnew (activate it, white IC with green pins).
Then right click on an empty spot and select “Global Spread and Place”.
Chose one of the spread options.
When done, deactivate the “Mode Footprint” afterwards.
I think this is/will not be needed anymore in some future version of the prog.
Yes, the place that fabricates your boards sets limits on some of these factors. And, like @davidsrsb points out, there is typically little to be gained by asking your vendor to operate right on the edge of his capabilities when he makes your boards - so build in a little margin between what you ask for and his advertised capabilities.
But there are other practical reasons for designing with larger feature sizes. One such reason is ergonomics. If a real live person of the homo sapiens persuasion must interact with your board during soldering, troubleshooting, modification, or repair then larger traces, spacing, and pads, should be considered. (When you read the following list of my opinions, remember that 10 mils (0.25 mm) is approximately the thickness of a business card, or the thickness of 3 sheets of common printer paper.)
Hand-soldering SMT components can be done more reliably if the pads are enlarged to expose more copper beyond the component body. And while you’re at it, don’t pack them in so tightly that you can’t get a soldering iron onto the pad.
The same idea applies to test equipment probes, even if the board is machine-assembled. You may try to anticipate which nodes are likely to be investigated by a 'scope or DMM, and which aren’t, but when things don’t behave quite as you expected then the node you want to look at is usually the least-accessible node on the board. Or, you can’t probe it without shorting to adjacent components.
A 10-mil (0.25 mm) annulus on a through-hole pad may be fine for automated soldering processes but taxes the abilities of a manual soldering operator. With so little copper to contact the soldering iron’s tip and conduct heat into the joint, the time needed to complete the joint is longer and the risk of component damage is greater. I use 15 to 20 mil annulus for manually-assembled prototypes, and 30 mils for wire attachment points.
Find out what “standard” hole sizes your board fabricator uses, and limit your hole sizes to exactly those values. In particular, identify his standard value in the range of 0.030" to 0.035" (0.75 to 0.90 mm) and use this size as much as possible - it’ll probably work well for 90% of your through-hole parts.
A 10-mil trace of 1-ounce copper is suitable for a bit less than 1 amp in most applications. Narrower traces are more likely to de-laminate from the fiberglass substrate when components are removed or replaced during prototyping or repair activities.
10 mils is probably the minimum copper-to-copper clearance you should use for hand-soldered boards. (And some production engineers will thank you, perhaps with a serving of your favorite malt beverage, if you stick to 10-mil spacing on machine-assembled boards.) Even at 10 mils you need to watch carefully for solder bridges.
Guys i am unable to see modifications done to a particular footprint it is not reflecting in the Pcbnew after i modify the footprint and build new netlist and read the new netlist in pcbnew the footprint does not change can you please help me on this one ?
make sure the footprint you changed is really the one you’re trying to re-load (been there, done that wrong)
Next, hover over the footprint in question, hit [E] and go to ‘Footprint Properties’ > button [Change Footprints] … new window, set to what you want (just that footprint or similar ones, etc… and hit [Apply].
You can change the footprint either via [List Footprints] or [View Footprints] if you’re not just ‘updating’ from the repo.
Guys How do i just view the front copper components only and hide the back layer components or vice versa i have tried ticking a visible layer option on the right hand side of the tool but that does not help
can i know where i need to mentioned track width and clearance size for internal layers
in the bellow image i have the option to mention only in the external layers
On the left hand side of the image you can see a bunch of components stacked up one on top of the other how can i separate them in just one click or one button press. removing hundreds of components from that heap is just very hard
If any of the ones who usually know this stuff didn’t answer yet it’s either not possible (I suggest searching the bugtracker/wishlist for that particular feature - I won’t do it ) or they didn’t see it attached to the bottom of this thread - then make a new one.
But try the bugtracker/wishlist first as I have a feeling that it’s not possible yet and people asked for it before…?