Often times I read comments/recommendations about placing lots of vias for GND in 4-layer designs, as well as a line-up of vias surrounding the board to protect from EMI, etc. I was always under the impression that vias (either tented or not) have a certain impact in the final PCB cost, so I tried to minimize their numbers in my designs. However I might have been wrong and vias are extremely cheap? For instance, in a 4"x4" board, how much would it affect a design cost to have 400 or 200 vias instead of 100? Does the diameter of the via matters? I'm talking about normal all-the-way vias, not buried vias which I know are much more expensive.
\$\begingroup\$
\$\endgroup\$
2
asked Mar 30, 2013 at 23:11
-
\$\begingroup\$ Have you asked your board vendor? PCBs are drilled with computer-controlled equipment, so the vendor's only cost is the machine time. And those machines run fast! Have a look at the Apple device teardowns on iFixit and see how many vias they use on their cost sensitive, yet carefully-engineered designs. Anyway, call the vendor and ask. \$\endgroup\$– markragesCommented Mar 31, 2013 at 4:17
-
\$\begingroup\$ I actually did, but I've got fuzzy responses like "send your design and we'll give you a quote", not something clear cut I could use to direct my design. I suppose I should contact them again and ask for a thorough explanation. \$\endgroup\$– Guillermo PrandiCommented Mar 31, 2013 at 14:03
Add a comment
|
3 Answers
\$\begingroup\$
\$\endgroup\$
Vendors are not good at telling you how costs will vary based on different specifications. They will always ask you for your files and provide a quote to that specific board. They generally can't, or won't, give you a relative answer. In my experience the number of vias is not as important as the size or type. Microvias (definitions may vary from vendor to vendor) are much smaller and will cost more than a standard via. Blind vias (which do not extend through the entire board) will also be more expensive. The price difference between having 200 vias and 100 is probably going to be negligible. Back when holes were drilled manually the cost would have been impacted much more, but nowadays with machines doing all the work, it really doesn't make much of a difference. Keep your via diameters large whenever possible, though. If there's a higher chance of a bit breaking (because it's so small), the board house will charge you more for the fab.
answered Aug 2, 2016 at 12:38
\$\begingroup\$
\$\endgroup\$
1
If I recall correctly, many years ago the local board shops did charge per hole, but I haven't seen hole charges for many years for normal boards. There might be an extra charge for something with an execessive quantity of holes, like a breadboard layout. (This may, of course, vary with the board shop.)
Some of the prototype shops will charge extra if you specify too many different drill sizes, or sizes outside their normal drill set.
answered Mar 30, 2013 at 23:31
-
\$\begingroup\$ Thank you, Peter. I know that much since I've been designing PCBs for some time, now. I was looking for a more thorough response. A PCB with an RF module or some fast MCU with external memory might need a lot of vias for reducing EMI and other reasons (just like breadboards), and I'd like to know how much conservative should I be about them cost-wise. \$\endgroup\$ Commented Mar 31, 2013 at 3:12
\$\begingroup\$
\$\endgroup\$
The NC drill will need more time to drill 400 vias instead of only 100. These machines are expensive and the board manufacturer will charge you in some way for the number of holes. If your smallest drill size is about 0.7 mm, they may drill 3 boards together in a stack, but when smaller drills are used, it is possible to drill only 2 boards in stack or even only one. Drilling 2 boards in stack instead of 3 will need 50 % more time, 1 instead of 3 will be 200 % more time. Using very small drills requires a machine with more revolutions per minute to get clean holes. Very small vias cause problems during the galvanic deposition of copper on the hole walls, the electrolyte liquid exchange may be blocked by dust or air bubles. Dont forget you need a reliable connection of some vias to the inner layers. The board house must clean the hole walls after drilling to ensure a good and relaible connection of the copper on the hole walls to the copper of the inner layers. This process is called etchback. You have to ask your favourate board house for the cost of different number of holes and different drill sizes. Ask if they do an electric test of the connectivity of the boards and compare different board houses.
