Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

50 ohm track is so wide for a 0.3mm pin ???

Status
Not open for further replies.
actra

actra

Member level 5
Joined
Nov 9, 2004
Messages
90
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Location
cairo [EGYPT]
Activity points
851
rfic pin pcb trace

im using FR-4 ....50 ohm microstrip = 1.407 mm track width
i use an RF IC that has 8 pins ... every pin of 0.3 - 0.4 mm wide only ? how can i connect the microstrip to it with out much mismatching ?
 

rfic pin rf pcb trace

It depends on freq. Generally if you have PCB object are smaller than 1/10 wavelenght you don't have to worry about mismatch cause by PCB. In that case more dangerous are parasitic capacitances (from PCB to GDN) and inductances.
In higher freq I don't know.
 

track pcb 50 ohms

There might be many pins, but often there are only two or so pins that carry microwave energy. For those few microwave signals, run a 50 ohm line as close as you can, and then mitre down the line width as you approach the pin.

The Pin looks like a series inductor, the open end of the trace where it solders to the pin looks like a shunt capacitor. The mitred section looks a little like a series inductor. So, it kid of looks like a 3 pole lowpass filter. If you are not too high in frequency, it somewhat matches to 50 ohms. Of course, if you are too high in frequency, that "lowpass" effect will cause big ripples!
 

width track 50 ohm

just taper your 50 ohm line and connect it to IC pin and don't worry more at this frequency.
Regards
 

I think you can route the width same as the pin 0.3-0.4 ,because it is very short . Then connet the pin with 1.4mm width track .
 

The frequency used is 1.3 GHz ,,,

heres an attached image...

the wide trace is 1.4mm microstrip
the thin trace is 0.4 wide , 0.4 tall .....

IS THE SOUTION GOOD ? or there's better solutions to use ?
 

Why don't you use 200um height of pcb ?? In this case track width will be around 300um.
You can cascade 200um and 1.6mm substrate and if you use second layer as a ground, you'll have thinner track widths.
 

If you are limited with the 0.8mm FR-4 (so you can not use thinner PCB), perhaps the better solution would be as shown in the attached picture. Of course I've assumed that you have the space around the IC...

regards,
rfmw
 

    actra

    actra

    Points: 2
    Helpful Answer Positive Rating
Impendance of trace depends on track width and layers stackup. Choose approprate layers stackup to reach desired trace with and nominal impedance. With thinner laminates you can use thinner trace withs for desired nominal impedance.
 

Hi. You may try to use grounded coplanar waveguide (GCPW) trace. The centre trace width could be set to match the pin width. Adjust the ground separation gaps on both sides of the signal trace to achieve 50 ohm
 

i think it is not necessary to care about width on 1.3GHz,
but i will do like this:
1.4mm-0.8mm-0.4..........
can it work?!!
 

I think everybody missed an important question. Is the 0.3mm pin input (approx.) matched ?
If it is approx. matched, you need not worry about anything at 1.3 GHz.
If it is somewhere of the total reflection range (e.g. FET gate input) then every effort should be made to match the width of the microstrip line to the pin, as Bigboss has written above.
g579
 

rfmw ..did u use pcad pcb to creat the above picture ? if so ..ijust wanted to know how can i change the RED routing line "track" TIP ? from rounded tip to tapped or flat tip in pcad pcb ?

Added after 13 minutes:

by the way the IC above is a prescalar..ithink its approx. matched to 50ohm..
 

Hi actra,

yes, I used P-CAD (as you did I assume :) ). I draw/route my high frequency PCBs in P-CAD almost always with "Place polygon" function. I wasn't satisfied with rounded ends of wire (Route manual function) just as you noticed now. If only there is a way to disable rounding the ends of a wire...
 

do you know how the lenght of line effect on matching?
which interconnect's lenght is most suitable?
 

if you use a four layer board, 50 ohm microstrip's width will be about

0.4mm.


best regards



actra said:
im using FR-4 ....50 ohm microstrip = 1.407 mm track width
i use an RF IC that has 8 pins ... every pin of 0.3 - 0.4 mm wide only ? how can i connect the microstrip to it with out much mismatching ?
Click to expand...
 

:( how's about the length ? don't u mind tell me it influence
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top