Something seems to be consistently inconsistent. Garbage in > Garbage out.
Is this what you are seeing in the gerber viewer?
The reason is you didnât tick Plot footprint values in the Plot dialog General Options. The 2K for R1 appears because itâs freestanding text you added, and not part of the footprint.
I can confirm that the 2K for R1 does not move when I move the footprint. But the other resistor values do move when I move the footprints.
ButâŚhow did you figure out this diagnosis?
I note that the tracks are unnecessarily thin. 0.2 mm. This makes for easier damage, more ESL and higher DCR. If this were my board I would make the tracks more like 1.5 mm. That is still narrower than the pads.
Here I have made one track 1.5 mm wide. Donât worry about how some of the tracks are not aligned with the footprint pads. As I said, I experimentally moved all 4 resistors. Those are the âpiece de resistance!!â
The other thing I would do is make one layer (probably the back) solid copper ground plane (as much as possible) and put all of the tracks (as much as possible) on the front layer.
1 Like
Simple. I verified that the values were in a silkscreen layer as required to be visible in the final physical product, but I also saw the General Option in the plot dialog which also controls the visibility of the value field. So I tried it with and without that box ticked.
Edit: Besides BobZâs advice, I would also add that unless you are requesting assembly or need a solderpaste stencil, thereâs no need to generate the *.Paste layers.
Are you saying that the SS that didnât show on their drill layer, will be on the PCB?
How do I make a correction to the project?
Thanks
Yes thatâs what I saw from the pcb mfg.
What do I have to do to correct that ?
Stop talking about drill layers, these have nothing to do with drills.
Itâs not enough to put the value in the silkscreen layer, you also have to enable generation from the value field in the plot dialog as already explained here:
Do I have to redraw the wires with a fatter setting or can I just change the trace dimension in the plot settings? Iâm guessing that if I donât change the settings for wire thickness I wonât be able to see if it fits.
I really appreciate you taking the time to explain things to a newbie.
Thanks
Iâll let someone else explain how to use netclasses to influence the track width. Donât call the tracks on the PCB wires. In KiCad terminology wires are the lines in schematics.
Understand that I tend to make wider tracks than most users on this forum. But I think most users would make their tracks for your board wider than the 0.2 mm which you used.
I take an individual approach to tracksâŚI do not rely much on net classes, etc. But I would not attempt to fatten tracks with the gerber plot process.
Open up your pcb file. Make sure that âtracksâ are checked in the selection filter at lower right. Double click on the tracks. It will be very easy to change the track width. I think this might take less than 15 minutes on your board. I do not expect any problems to result but it would be wise to run DRC after doing that.
I did not keep your file. This screen shot was obtained by clicking on a board design of mine:
Hi @vvarady
Firstly, a summary when discussing on the forum:
Schematics have symbols that are connected with wires.
PCBs have footprints that are connected with tracks.
As @retiredfeline hinted:
Set up some track widths. LMB the triangle in the box highlighted by the green arrow. Mine shows 20 mil, yours will show âTrack: use netclass widthâ.
This will take you to âFile > Board Setup > Design Rules > Predefined Sizesâ.
Using the â+â sign (bottom green arrow), type in the various width tracks you may want. The widths you enter will depend on the measuring system you use (imperial or metric). Set your measuring system before opening this chart.
When you have finished loading widths, the top indicator box (top green arrow) will now show your current track width. You can now change widths on the fly with the âWâ and âShift + Wâ hotkeys, as shown in the top illustration.
Also worthy of checking is to hover over the âUâ icon beside the Track width box. A pop-up explaining its use will show.
Finally, File > Board Setup > Design Rules > Netclasses can also be used. This subject is best read about and experimented with, before discussing on the forum. See here.
1 Like