Continue to Site

# differential pair trace impedance calculations

Status
Not open for further replies.

#### bhushan233k

##### Junior Member level 2
dear friends

I want to route 100 ohm differential pairs of LAN
on two layer pcb ( 1.6mm pcb thickness ) with 8 mil trace width, 8 mil trace spacing , 1.4 mil trace thickness.(dielectric constant Dk=4.3 as fr4 material with 1.6 mm is used)
can anybody help me how to calculate 100 ohm impedance with above data......

I want to route 100 ohm differential pairs of LAN
on two layer pcb ( 1.6mm pcb thickness ) with 8 mil trace width, 8 mil trace spacing , 1.4 mil trace thickness.(dielectric constant Dk=4.3 as fr4 material with 1.6 mm is used)
can anybody help me how to calculate 100 ohm impedance with above data......
With the given parameters, you can only "calculate" that the 100 ohms target is missed (about 130 ohms). Obviously, at least one design parameter must be allowed to vary to achieve 100 ohms.

I presume you are designing a differential microstrip (involving a ground plane), but you didn't tell explicitely.

To achieve 100 ohms with 1.6 mm FR4, the trace width must be increased and/or the separation reduced. If room is limited, it may be helpful to add ground at both sides of the signal lines, making differential surface coplanar strips with ground.

with ground plane I hope... use this tool https://saturnpcb.com/pcb_toolkit.htm

PCB test at factory requires test coupons and adds 10% cost approx in volume. Factory compensates all controlled D codes ( track width) due to dielectric constant variations (large) and plating thickness variations (smaller) to achieve accuracy within 5% or as desired.

8 mil track and gap wont cut it. YOu need higher precision board shop to make this and design with a ground plane to make two 50 Ohm lines with better immunity as your differential current is probably ground return, or not. Some can get better results with tracks on either side that are perfect match, then add ground tracks on either side and thin ground track in between.

If you know TDR test, this is how board shop measures Zo.
I prefer Return loss method on spectrum analyzer, with crosstalk test from adjacent signals.
Best I have achieved is -120dB crosstalk and 40 db Return Loss over entire band up to 1GHz using Getek.(Polyamide type I think)

Reference https://www.multi-circuit-boards.eu/en/pcb-design-aid/layer-buildup/series.html

However if using lower frequencies , you can use std FR4.

Its been 20 yrs , so I am going by memory.

with ground plane I hope...

Why ground plane? Differential pair is perfectly fine without ground plane. By adding a ground plane (=third conductor) you only enable additional modes (i.e. common mode) which is not desirable.

i have used online calculators (plesae refer snap attached)

but i can not reduce spacing less than 8 mils.

so how can i achive 100 ohm differential pair ...

- - - Updated - - -

also no ground plane is used.....

but i can not reduce spacing less than 8 mils.
so how can i achive 100 ohm differential pair ...

As FvM mentioned, you can also increase the trace width for lower impedance.
The relevant impedance value for your case is the differential Z.

You'll need a trace width between 20 to 25 mils.

bhushan233k

### bhushan233k

Points: 2
Any calculators that will work without a reference plane....

Why ground plane? Differential pair is perfectly fine without ground plane. By adding a ground plane (=third conductor) you only enable additional modes (i.e. common mode) which is not desirable.
Having tested designs with ground planes, and many differential DS1 channels in parallel on a distribution box I designed for Avaya ( nee Lucent) they verified my prototype Common Mode Rejection and Crosstalk ( co-channel signals, adjacent tracks) were superlative (-140dB) using ground plane under signals and between channels to absorb any stray crosstalk.

16 Channel 1.54 MHz differential channel including PoE Distribution Box circa 2002

I suspect you are going to learn the hard way.

Without using a fab shop that can verify controlled impedances, you will never get what you expect even with good numbers. All the tolerances are just too high. First define what you expect in tolerances, then determine if design will work.

The site you are using is very accurate but has no tolerances.

1. If a shop is only capable of 8+8mil (track+gap), it means they cannot control the tolerances and quality of anything smaller on a consistent basis.
2. You can expect copper etchback, meaning the edge of the copper etch mask may be etched to within a tolerance of more or less than the thickness of the copper which in this case is 1.4 mil (1oz) which is 17.5% of this minimum gap size of 8mil in your case, which results in a +/-4% change in Zo just from one variable, gap size. Track width increases as gap shrinks from low etchback which increases Zo tolerance again.
This means a cheap shop may give inaccurate Z0 tolerances, so you can expect more reflections and signal distortion depending on line length and rise time
3. A 10% tolerance in dielectric constant can affect Zo by another 4% or so depending on geom.
4. Then add errors in assumptions for dielectric constant due to choices of material epoxy/fiber ratios of supplier tolerance of 10~15% and Polyamide or better Teflon)
5. Chances of achieving a 10% Zo tolerance are slim without experience or paid fab-shop TDR-Zo testing. ( e.g. 100\$) and that's only single ended Zo testing (?)
6. For ANY controlled impedance if you have no experience , you must consider a tolerance stackup of all tolerances or discuss the design with supplier and specify and pay for controlled Zo TDR testing, which is done outside outline of board and then all D codes are corrected if it fails the tolerance criteria after test and rebuilt.
7. Your design ( edge-mode differential microstrip) radiates and EM field between the edges in the gap with some reflected off the ground plane beneath tracks.
8. Controlled impedance, Zo is governed mostly by conductor ratios and to some degree, the dielectric constant and conductor thickness.
9. The gap changes to retain these ratios for different 50 Ohm cables. The outer/inner surface ratio across the gap increases for 75 Ohm Cable for TV.
10. For Ribbon cable, often 100 to 120 Ohm differential, it is the ratio of conductor/gap that matters.
11. Now remember what Characteristic Impedance means as a transmission line.
12. It is the ratio Zo = √(L/ C)
13. For your design "edge-mode differential stripline" , wider tracks give more L but even more capacitance when the board thickness reduced for a give gap. So the critical ratio is the track centre to gap to ground plane.
14. Unfortunately Online Calculators are deceiving unless you actually draw the numbers and understand the ratios and tolerance effects.

Suggested Solution:
for 100 Ohm Differential, use half the board thickness and make the tracks equal to the board thickness. This is an approximate critical ratio.
Normally online calculators are designed for very thin inner layers and not fat double sided low-quality boards using thinner copper 0.5Oz and better shops with more precise process controls for etchback , thus can offer 3 mil track/gaps

- - - Updated - - -

See the geometric ratios and remember for 100 Ohm differential, to draw an imaginary equilateral triangle from track centres to the ground below the gap. dielectric thickness as an approximation with 8 mil gap.
Here are 3 good examples and 1 bad example for Zo=100

Points: 2

### bhushan233k

Points: 2

You can also try with Si8000 Controled Impedance Calculator from Polar Instruments, it's more complete and I think more accurate than these online calculators.

i got much help from your post......

Status
Not open for further replies.