I need to get a bottom trace between two via's that currently are connected with an airwire.
However, when doing the trace at the bottom, the polygon does not cede to make way for that trace.
Using Eagle v7.6.0
How to solve?
I need to get a bottom trace between two via's that currently are connected with an airwire.
However, when doing the trace at the bottom, the polygon does not cede to make way for that trace.
Using Eagle v7.6.0
How to solve?
The 'issue' with the polygon I solved yesterday. No need to switch off the polygon, just trace the track across the polygon, do a refresh (ratsnest) and the polygon will have cleared a path for the added track.
I am not interested in 3D design features such as for libraries: mine do very well for me. And I do not want having to recreate every library in my folders.
Also, designing new packages never has been a problem for me, no issues with error codes. Eagle, for me, does what I want it to do: create schematics, libraries, and from there pcb tracing, all in a well flowing manner. To me Eagle just is a workhorse to make pcb's. Hundreds of them for over a decade.
The 'issue' with the polygon I solved yesterday. No need to switch off the polygon, just trace the track across the polygon, do a refresh (ratsnest) and the polygon will have cleared a path for the added track.
I am not interested in 3D design features such as for libraries: mine do very well for me. And I do not want having to recreate every library in my folders.
Also, designing new packages never has been a problem for me, no issues with error codes. Eagle, for me, does what I want it to do: create schematics, libraries, and from there pcb tracing, all in a well flowing manner. To me Eagle just is a workhorse to make pcb's. Hundreds of them for over a decade.
"The 'issue' with the polygon I solved yesterday. No need to switch off the polygon, just trace the track across the polygon, do a refresh (ratsnest) and the polygon will have cleared a path for the added track."
Yes, you don't need to switch off. I just suggested it for easier working.
Refreshing the rat's nest works perfectly in Eagle Version 7.6.0, but sometimes corners and edges are visible after refreshing.
This happens when you work in "off-grid" mode, and calculation errors (rounding errors) are visible.
An unfavorable setting of the distances, fine gradation - polygon component - can also cause such rounding errors.
I always check whether I am laying the conductor tracks on the set grid and make sure that these, especially the slanted conductor tracks, are really 45.0 degrees or a multiple of that.
I always set the grid levels to be breakable down to a multiple or divisible so that the components are also placed on a grid.
-> Your autorouter is obviously set to route "off-grid" because it edges and slant the conductor tracks in such a way that it jumps around to the components.
I route mainly manually myself, including multilayer PCBs. That way I have control everywhere. Time is relative...
I also observe high frequency guidelines. Especially where there are clocks or high switched currents/voltages.
I almost never route between the component pads on SMDs, that can be critical unless it is not a problem because the distances are far enough, or the conductor does not carry any frequencies.
I try to use a direct route strategy (in cardinal directions: east-west, north-south, east-north, west-south), with as few vias as possible.
Vias next to the components are better than underneath them.
For SMDs, I make sure that I route on the top side, for through-hole components, I make sure that I route on the bottom side.
Here, the through-hole components are mountet on the bottom side (mirrored), so the tracks are on the top side.
I've all manually routed. North-south, east-west; left top power-in, right top signal-out
--
-> On your board, one of many issues:
the large electrolytic capacitors are connected to the top-layer traces.
This can cause major problems at high temperatures and under physical stress.
-> "cold solder joint", then the capacitor wobbles and you have problems, even where the conductor track breaks across.
-> How do you then repair it?
As well the "high-current" traces are very small, and they are going across the PCB. Your PCB is a power supply that can be very warm, or even hot, containing a µC module.
- So, my suggestion: connect power tracks (if there is no other option, make a power layer, or change the layer, but it is better not to lead them to the components on top) on the bottom layer side, then you have good stability and can also repair the connections better.
I have had to repair many such errors in the past, e.g. TVs, monitors with CRT screens, industrial devices, power supplies, etc...
I had to patch many burned-out holes in PCBs.
I wish you the best with your projects.
Gerald
---
Hi Gerald,
I'm the same, I prefer manual routing; I meant that modern features for guided routing in KiCad are better than the poor auto-router in EAGLE. I don't mean auto-router is better than manual routing (at least, not for the complexity of boards one would be using these particular tools for).
I've not seen what improvements KiCad 9 has made (I don't think they have the rubber-banding feature you mention). In v8, there's a kind of slight approximation, which is the auto-complete. It allows you to move a part, and all connections will turn to air-wires as you mention; however, if you then press Shift-F (with the component highlighted), it will try to auto-fix the connections, i.e. the end result of a rubber-banding sort of operation. Here's a video of it, where I moved a part, and then deleted the traces that I didn't like to remain, and then selected the component and pressed Shift-F. Not as smooth as rubber-banding of course. You can see it missed one trace, but that's easy to fix, by clicking on that trace and pressing Shift-F again.
Personally I don't use this tool in this way (I sometimes use it per track, using just the 'F' key). For general routing, I usually have KiCad set to the 'walk around' mode, and find that very useful minimal guidance while routing (but the other options are very useful too).
The EAGLE imports of libraries is already excellent in v8, however since EAGLE had issues with slotted pads and shaped pads, it is beneficial to either try to clean up those specific footprints, or to recreate them, using the direct KiCad support for those features.
But it would be wise to retain old EAGLE for old projects for sure (even though, again, KiCad support of EAGLE project import is pretty good too).
Personally, I've over time just redone the footprints that I wanted to use, rather than use the EAGLE version (however, I have still imported the EAGLE footprints, so I can easily compare, to reduce the risk of error).
Regarding the 3D models, I now try to always have a 3D model for each new component I add, simply because I've found it reduces errors so much, in two ways:
(1) The obvious way, which is that you can easily see if there are clashes between parts on the board, and optimize the position of parts on board edges, etc.
(2) Not-so-obvious (at least not initially to me!) - it greatly reduces the risk of error in the PCB footprint creation process in the first place, because, if your 3D model doesn't match the pads and outline, then it's immediately clear there is an error in the footprint or the model! This has been immensely useful, because often some dimensions may be vague or missing in the drawings in the datasheets, or I may have introduced some accidental error. The 3D model lets me instantly get a decent amount of additional confidence that the footprint is good.
