Hello.
On my 2-Layer PCB I use a few L293D IC. I’m using 1mm Trace Width because L293D Max Output per channel is 600 mA.
My question is: To calculate the Via Size and Via Drill for a 1mm Trace Width, should I use some formula or some standard dimensions?
Best Regards
Kicad includes a calculator that lets you play with the parameters or a via for a given current, from the project screen click on the calculator icon.
Only in 5.99, not in 5.1.
Then there is “Saturn PCB Toolkit” a bit of free software you can use to the same effect.
A very simple rule of thumb is that a Via should have the same amount of copper as a track. Since via’s tend to be round their diameter should be around Trackwidth/pi.
However, because of the way PCB’s are produced, the thickness of the copper in a Via is thinner then on the PCB tracks. I prefer to keep via diameters at least half the track width.
However, the minimum hole diameter for a Via I’m comfortable with is about 0.6mm, which is much wider than most tracks are.
The PCB calculator advises 2.7A for a 1.2mm wide trace, and for such currents I prefer not to trust on a single via.
If you search for via diameter recommendations on the internet you’ll find all kind of stuff, from simple guidelines such as I use to very technical papers with detailed simulations (or even actual measurements) of temperature rise.
Thank you for all the answers.
Yes @paulvdh I was looking for a more simple answer. For instance ended up with some tracks of 1mm width and on those tracks I’ve placed a via with 1.8mm size and 1.2mm drill.
Yes that ok? Really that know, that’s what I was trying to understand. Anyway I did it because it makes sense in my head that it was wider then the track itself.
Also I didn’t know if 1.2mm drill was standard or not.
For a 1mm wide track there really is no need to drill a 1.2mm hole.
As I said before, using half the diameter of the track width is usually plenty.
0.5mm is getting near a very thin drill though. I would simply use the same drill size as is already used for other holes such as DIP IC’s or THT resistors. A long time ago it was good practice to reduce the amount of drill sizes, but nowaday’s the machines are so sophisticated that almost any drill size can be loaded automatically from a magazine.
The typical rule of thumb is 1/2 an amp for a 0.3mm via for a 5C temprise.
This should be backed up by the IPC-2221/2152 as well as the Saturn PCB toolbox.
Likewise it is covered here:
Now an interesting tidbit… based upon that 1/2 amp rule of thumb, you can increase the current capability by adding more via’s OR increasing the diameter of the via. n number of via’s have a current carrying capability comparable to one via with n diameter of the multiple.
ie, a 0.3mm via is good for 1/2 and amp, thus 10-off would be good enough for 5A, or 1off with a diameter of 3mm. Typically I try to balance the diameter to the count as well as minimise the different drill sizes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
