I wouldn’t recommend it…
A single SMD pad on both sides is not allowed.
But 2 pads with the same pin number, one at each side and at the same position, it is allowed.
The double-sided footprint with a different pin position was extracted from https://github.com/MakotoKurauchi/helix/blob/master/Doc/buildguide_jp.md
I guess this might not be the best practice though. What do you think?
It is OK. It only requires more routing.
Great - I’ll use that footprint for now.
For standalone connections, LEDs on each hand are controlled by it’s own Arduino. On both hands the 3PIN 1 and 2 are bridged. JP1 will not be bridged.
For master/slave connection, all LEDs are controlled by a single Arduino. On the master side 3PIN 1 and 2 are bridged. JP 1 is bridged.
On the slave side, 3PIN 2 and 3 are bridged, and JP1 will not be bridged.
Any recommendations? I feel like this can be simplified.
Personally, I would simplify it by doing it as single sided boards instead of the reversible idea. I think you could probably use the same board for both sides, but if not it’s not a big deal to have two different boards.
The GND pads are unconnected.
Is there a way to use trace in FreeRoute, instead of a copper plate? Or are there any other ways to fix this?
I’ve deleted all zones, and run free route.
So, does it make sense to create a board without copper fill like this?
Well first you might need to know why pcb designers use copper fills in the first place.
One reason is that it can reduce the amount of chemicals used to etch the copper.
The far more important reason is that it can help with electro magnetic compatibility (EMC) requirements. If you use a fill for GND it allows low impedance return paths without the designer needing to really think about them. This is especially true if you have a full layer only for GND. (Only possible in very simple two layer boards. Will most likely require at least 4 layers in the design)
If you don’t have a single layer for such a GND plane, then you might need to make use of stitching vias and the trick of restricting one side to mostly horizontal traces and the other side to mostly vertical traces.
This results in orthogonal stripes of copper on top and bottom. By connecting the stripes on the top with the stripes on the bottom you get something similar as a full fill. (But it will of course be worse with regards to EMC then if you have one full fill. It is also more work.)
Even without that trick it might still be possible to get a better result using a split up zone then when using single traces. (But there is no guarantee for it. If the traces are placed carefully it might even result in a better EMC behavior then by forgetting about GND and simply placing a copper pour.)
As you do not design a critical high frequency design, i doubt EMC has a high priority for you. If it would be a priority, you would need to make a specialized board for exactly one purpose with one known configuration.
Thank you! I will try with stitching vias. The orthogonal stripes idea is very interesting too.
Is there a way to auto route or automate the connection of the 2 GND pads in a footprint?
I found that the GND in the front and the back of this footprint are not connected.
So, I found Protip: nicer via stitching
If I use around 24 via stitches in this 110mm*100mm board, is it too much?
Or if I use the via stitching script https://github.com/jsreynaud/kicad-action-scripts , it looks like I can use an array of via stitches in a large amount.
Will there be any problems when I add many via stitches like this?
Should I minimize the use of via stitches?
Some board houses have a limit on holes before they charge more so check with they place you are using.
as @hermit pointed to - this limits / extra charges come from more use/time in drilling all these holes!
and holes are weaker as full material here - so - eventually with this stitching you making it mechanically extremely worse…
if you do some vias in a finer line you could use it to ‘break-away’ parts of the pcb…
sunny greetings
stefan
You can also ask yourself the other question:
Does it have any advantage to put all those via stitches in?
Via stitches are uses for a few different things:
HF shielding (Does not apply here).
Heat conducting (Does not apply here).
Increased current handling (Does not apply here).
Tespoint access: Scope probe’s slide less easily (Does not apply here).
Mechanical strength: Ripoff prevention of traces (Does not apply here).
Mechanical strength of SMD pads for connectors. (Does not apply here).
You may have had some fun placing all those via’s (or wasted your time, depends how you look at it) but I do not see how they add anything to this circuit. And as others have said, it does increase the production cost of the PCB.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.