Seeed’s Fusion PCB Specification lists for minimum trace spacing / width on FR4-TG130 boards:
For 1oz, 4/4mil, 5/5mil, 6/6mil
Does that mean if I use 6 mil trace width, I have to use 6 mil spacing, for 5 mil width 5 mil spacing, etc.?
If so, then why is spacing correlated with trace width?
I don’t know, but I think that:
Probably the price can depand on technology level. If no track on PCB is smaller then 6mil and no spacing is smaller then 6mil your PCB can be produced in 6/6 standard (probably the chippest).
You can use 6mil track and 5mil spacing, but such PCB will be produced with 5/5 technology.
Thanks, sounds reasonable, although I’ve no clue about PCB manufacturing.
What Seeed calls “spacing” is called “clearance” in KiCad.
Screenshot from Seeed:
There is always a minimum size of features manufacturers can make reliable.
It probably does not matter much if a feature is the width of copper (Can get open circuits if too small) or if a feature is a clearance distance ( Can get shorted if too small).
The size of those features is a sum of worst case production tolerances and may be different with each manufacturer.
Also note that those parameters may depend on weird or non intuitive numbers.
With Seeed for example the clearance between two tracks is different than the clearance between a track and a zone. (And I have no idea why).
I had not seen the 4/4, 5/5, 6/6 notation before, but I have heard about “board classes” before, which are a more universal name for something similar.
KiCad has a table with guidelines in the PCB Calculator for this:
The post by @paulvdh explained the nomenclature. As a first approximation, those two values - the minimum trace width, and the minimum copper-to-copper spacing - correlate to how difficult it is to manufacture the board. When a board fabricator lists several values, like Seeed Studio does, they are probably referring to different pricing levels. You can interpret it as something like,
“Our standard pricing applies to boards that meet 6/6 design rules. For an extra charge we can supply boards designed to 5/5 rules. We can even produce a 4/4 board, but if you must ask how much it’ll cost, you probably can’t afford it.”.
I should add that, at this time (2019), manufacturers specify equal values for trace width and trace spacing. You may even find statements such as “Minimum feature size, 6 mils”, which don’t distinguish between copper “features” and non-copper “features” - the minimum that can be reliably manufactured is 6 mils.
There is no requirement that the narrowest trace on your board, and the closest trace spacing on your board, must have the same values. Since both of these values are specified as MINIMUMS, you are free to use larger values for either one. In fact, most of us usually design a board with wider traces and and greater spacings than what the board fabricator advertises as his minimums. The extra margin gives everybody some room to breathe. I typically set my design rules to 15 or 20 mil trace width, and 10 mil spacing.
Dale
It might also be related to board layers. Either way, 4/4mil isn’t expensive or exotic; JLCPCB specifies 3.5/3.5 on 4 and 6 layer prototype boards, and they’re not expensive. Only relative to 2 layer. I get those made all the time, mostly 4 layer boards. You need 4/4, 5/5, or 6/4 with 0.2/0.45 vias to escape a 0.8mm BGA which makes it a rather mundane spec.
Just in the process of uploading my layout, and there is the answer:
With my current settings, 6/6 mil costs 32.55 USD, 5/5 mil costs 44.53 USD, and 4/4mil costs 85.76 USD.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
