Can't route QFN28 4x4mm - Page 1
Forum section: electronics / general

author: JoeyG
author_rank: Regular Contributor
timestamp: October 31, 2024, 10:16:29 pm
content: footprint QFN-28-1EP_4x4mm pad pitch .4mm pad thickness .2mm (from Generic KiCad footprints)I get a DRC error when I place route on QFN28 4x4mm pulled through from schematic footprint settingsWhen trying to place route I get a green pad either side of the pad I am routing as constraint??? . I'm prevented from routing from the pad.HoweverIf I manually place the same footprint on the PCB without any reference to the schematic I can route that footprint pads OK manually.KiCad 8.06If edited the schematic and change footprint to a QFN-28-1EP_7x7mm and then update the PCB I can route OK.So why does it allow me to added a footprint 4x4mm footprint and route OK but if I start with the schmatic and update the PCB with the footprint it doesn't allow routing.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: October 31, 2024, 10:37:23 pm
content: First, add the second dot in KiCad's version number. You are probably working with V8.0.6.For the rest, it is very likely a combination of how your design rules are setup. Te width of your copper tracks plus the clearance all around it has to fit in between the other pads. If your pads have a pitch of 0.4mm, and a width of 0.2mm, then it only leaves a clearance of 0.1mm on either side of the track or pad. KiCad normally draws a thin outline around pads and tracks to show the clearance. This thin line can not overlap with pads or tracks from other nets. And in your case this very likely overlaps.If you just place a footprint on the PCB, then all pads are part of the "no_net" net, and as a result, KiCad does not care whether you violate clearance rules or shorts. For KiCad it's just a single net.

author: JoeyG
author_rank: Regular Contributor
timestamp: October 31, 2024, 11:43:31 pm
content: I've downloaded KiCad and haven't performed any board setup. What board setup do you suggest I config for these pads sizes?

author: Doctorandus_P
author_rank: Super Contributor
timestamp: November 01, 2024, 01:06:02 am
content: You do not change the pad size. Pad size is just part of the footprint size you use.You can set track width and clearance inPCB Editor / File / Board Setup / Design Rules / Net classesBut working with net classes is much more involved then just following a link pointing to it. You really need to do some studying of your own to get familiar with how to use this effectively. Net classes are also a common concept used in (nearly?) any PCB design program.On top of that. With clearances of 0.1mm, you are well outside the production capability of the cheap PCB services. You surely can order PCB's with that resolution, but they definitely will cost more.

author: Swainster
author_rank: Frequent Contributor
timestamp: November 01, 2024, 05:45:11 am
content: I recently found out that JLC can do 0.1mm/0.1mm for 2 layer standard boards. That said, I generally try not to go below 0.2mm trace width.See under "traces":https://jlcpcb.com/capabilities/pcb-capabilities

author: TankSparks
author_rank: Contributor
timestamp: November 07, 2024, 02:25:56 am
content: In my experience 99% of the time if you Can’t route track: Track is too wide use Q command to change track width, The pins on your IC are very close together.

author: phil from seattle
author_rank: Super Contributor
timestamp: November 27, 2024, 12:57:40 am
content: I ran into this a while back with a footprint in a copper zone. The Zone's clearance and min width were too high. But, of course, always first run through board setup - zones inherit from the board rules.