I specify impedance controlled traces by calculating the desired width. Then, I pick a close 3 digit number different from any other trace width. For example, if I calculate that I need a 220 um trace for 50 ohms, I will make all 50 ohm traces 234 um (I do this by assigning a net class for 50 ohm traces so that I can make them all the same by assigning the net class).
Then, in the build notes I specify that all 234 um traces are to be impedance controlled to 50 ohms, and I specify which layer to use as the associated reference plane. Usually they want to know what impedance and allowed variation, and they take care of the rest by including some test coupons with the board fab. They send me the measured impedance of the test coupon, but I donât get the coupons.
There is generally a fee associated with this. I do it because with a multilayer board, the spacing between the impedance controlled trace and the reference plan is usually 125 um or less, so it gets difficult to get good control because the 50 ohm traces start getting pretty narrow and you can end up with a pretty big variation.
If you are doing power RF, you use a bigger dielectric thickness so you can get nice, wide traces to handle the power, and manufacturing tolerances become less of an issue.
This is what I usually do. This is the design part, right?
This is what I want to know better. What are those build notes? How do you use to specify them?
Do you make a word document with this info? I was thinking about having something closer to the design files. Maybe written in the Gerbers would be better, especially if using foreign board manufacturers.
Sure, this is fine. This is the price of the manufacturer⌠it is not the actual scope of the discussion.
I personally havenât use them as my boards tend to be non-complex and I mostly order via online services.
I hope this helps.
EDIT: By the way, KiCad has now the option to add some of this information to your board, as a result, this can be printed in the gerber files if you so decide.
But it all does not seem very useful. I see no specification on which nets are impedance controlled, and neither do I see to what impedance.
The word âImpedanceâ can not be found in the specification of the Gerber X2 format (And this was a bit of a surprise to me)
So the primary path to impedance controlled tracks is to calculate track with from the PCB parameters (track width and dielectric constant) so youâre close, and then combine this with a discussion with your PCB manufacturer, and then probably add a text note on the F.Fab layer, combined with a unique track width for the impedance controlled tracks so they can be easily identified.
Your PCB manufacturer can then fine-tune the track with to get closer to the target impedance. Itâs probably a good idea to make the clearance around impedance controlled tracks a bit wider, so they are still in spec if the PCB manufacturer makes these tracks a bit wider for impedance matching.
Build notes or fab notes are just a file with instructions that we send along with the Gerbers. Itâs a numbered list of instructions about PCB class, tolerances, etc. Itâs mostly boilerplate.
However, we also include additional notes about thing like controlled impedance, which size vias, if any, are via-in-pad-plated-over (VIPPO), etc.
Some people have this as a fab notes sheet in the Gerber, but my present company uses a separate file that we stick in the zip archive. It used to be a text file, now itâs a pdf.
As we get questions from PCB fabricators, if they are common questions that get repeated, we try to answer them in the fab notes so that the number of questions decreases over time (thatâs the theory, anyways).
I am talking about how do you tell PCB Manufactures that tracks X, Y, and Z, have to be impedance checked.
As far as I know Gerbers doe not have labels/wire_names nothing. So you have to write this info somewhere. I can be written in the Gerber files itself somehow, or in another document.
How do you use to do that?
For instance, for me, it would be nice if Kicad could have an option like these Fabrication Drawings, that add text sayingâŚ
These net widths correspond with impedance-controlled tracks.
50 ohms = 0.2 mm
90 ohms = 0.4 mm
100 ohms = 0.5 mm
Something like that, generated by Kicad, as it does for other fabrication drawings
Again (sigh).
I could not find the word impedance in the Gerber X2 specification, which pretty much means it is not standardized, and you are therefore dependent on communication with your PCB manufacturer on how to do it.
I did find it quite surprising this was not specified in the Gerber file format. Maybe itâs time to go harass Ucamco about this.
Ah, I am not talking about having it in the Gerber format itself, I am talking about having it written in the Layout, as the Other Fabrication Drawings are going to appear in the Gerver drawings⌠I am not even considering using Gerber X2 since some PCB Manufactures may not even accept it yet.
Again: Itâs all the same difference, check your PCB manufacturer.
Apparently itâs quite common that they want some text notes written on a gerber layer.
And if some PCB manufacturer does not support X2, then just send him a note that you have send your PCBâs to one of their competitors because of that. X2 has now existed for a quite long time and not supporting is is somewhere between ignorance and stupidity and does not give me much confidence in such a PCB manurefacturerer.
