[SOLVED] why some people's track widths are so small?

Status
Not open for further replies.
L

LandLack

Member level 3
Joined
Aug 8, 2013
Messages
54
Helped
1
Reputation
2
Reaction score
1
Trophy points
8
Activity points
526
(I use microstrip) For what I've understood track width depends mainly from maximum current in the lower frequencies, and on Z0 (characteristic impedance); so when I use the calculators, I have width values of around 1mm, or 1.7mm, etc. But I've found out that some people use tracks of only 6mils (0.15mm) on their pcb!! How is that possible? Was I wrong, or did I forget something?
Please clear me this thing; I have very little practical experience, so please tell me how to behave in the choices, if possible.

Best Regards,
LandLack
 

6 mils of 1oz copper will carry over 0.5 amps, which is way more than digital signals require. When routing very dense boards it would be impossible using 1mm widths. (Forgive me for mixing English and Metric measurements)
 
And also, for fine pitch devices, track widths often go down to much less than 6 mils, but 6 mils is typically about the limit for "average" PCB fabricators (which also means the PCB can be cheaply made)
Necking down the traces overly much to intersect with the pads can create other fabrication issues (acid traps) if not done properly.
 
Regularly do boards with 0.1/0.1mm track and gap (4thou), though better sticking to 0.15/0.15 as mentioned above, though where possible I will use the best track and gap, but rarely go above 0.2mm (8 thou) these days.
I am curious why you say current in the lower frequencies? are you using FFT to determine the square waves spectral content?
As to Zo what type of lines are you calculating this for, high speed? or just general signals.
 

I'm making a RF circuit; the frequencies go from 100MHz to 1.5 GHz; the "line calculator" suggests widths around 1.1 mm if I put the parameters of a FR-4 substrate and 35um copper thickness. These are the carrier frequencies of my signal, which has a useful baseband bandwidth of around 30MHz.

Can I ask you some additional infos?
1) doesn't this 6 mil width generate mismatch between the devices and the traces?
2) What is the frequency of the digital signals that use such low widths?

I'm trying to figure out a general law for all the PCBs and situations.
 

If you need a particular trace impedance, then by all means set your trace width appropriately. What you asked, though, was 'how is it possible' people use 6mils.
 

What impedance are you after as it is this that controls the trace width in conjunction with Er, height between traces and routes. How many layers is your board?
DDR memory interfaces are often done with 0.1mm track gap (4 thou).
 

I need a characteristic impedance Z0 of 50 ohm;
just to know, what is the characteristic impedance of the lines of these digital interfaces?
 

marce said:
HOW MANY LAYERS, dielectric thickness, distance from ground plane for tracks!

https://www.skottanselektronik.com/

For example 6 layer board FR4 50 ohm antenna feed is 0.5mm
Click to expand...

For now I've got only two layers: the first has device + traces, while the second has ground.
The link you've sent me is very useful; for example, for er=4.3, W=1.8mm, t= 0.035mm, h=1mm, we would have Zo=50;
I don't understand the case of the antenna feed: if we see t=0.035mm and w=0.5 mm, we would need a h=0.3mm to obtain the Zo=0. Isn't that "h" value too low (device extremely expensive)?
So these "tight traced digital PCBs" have a low dielectric thickness (h)?
 

I think you should focus on the requirements of your design.

Understanding the design principles of various other boards you see all around might be over your head. Just to mention a few basic points, not all PCBs are using traces with designed impedance, if they do, the nominal impedance isn't necesarily 50 ohms, and not all traces are impedance matched.

I presume the microstrip calculations that you got from the PCB design tools are basically right. With a standard double-sided PCB you don't have the option to vary the substrate height much, but you can use different transmission line geometries if appropriate, e.g. coplanar strip with ground. The other point is that RF circuits can be designed with transmission line segments of different impedance. 50 ohm matching is only a subset of possible solutions.
 
I know, actually I've figured the information about my case; I just wanted to continue this discussion to learn something new. For example, didn't know that some boards (porbably those working with digital signals) had unmatched lines; it would be interesting to find out the limits of this behavior and/or the rule of thumbs about the argument.
 

I just wanted to continue this discussion to learn something new
Click to expand...
I see. The problem is that PCB designs cover a broad range of implemented parameters. 0.15 mm tracks may be either connections of general purpose digital logic without impedance matching on a double-side PCB or traces with well considered impedance on a multi-layer PCB with respective thin substrates. And I guess you didn't even think about impedance of embedded striplines on inner layers.
 

So should the question actually be - Why do people want such wide tracks still? :grin:
 

Mattylad said:
So should the question actually be - Why do people want such wide tracks still? :grin:
Click to expand...

bacause they have to work on frequencies higher than the GHz, I guess.
Thank you very much, guys; in the university they teach you about many things, but sometimes forget to add informations about "quantities", thus it's sometimes hard to understand the priorities...

Best Regards,
Landlack
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…