new to pcb, please any input would help.

[rubdawg]

I am trying to layout a pcb board for a test board and I have been trying to caluclate the width of a trace to make sure it is 50 ohms. I am an RF engineer and when I did my calculations I end up getting 2.54mm (milimeters) or (0.111 inches). Seems a little big but below is my parameters and attached is the picture of the paramters:

H=0.062 inches
T= 0.0017 inches
Zo=50 ohms
Er=4.6
and afer using a calculator it gave me W=0.1111 inches (2.54 inches)

This is a two layer board, copper on top and bottom. I used this site to caluclate the width: **broken link removed**

 

[Loq]

Hi,
With a 1.6mm thick board, the width of a 50R track is effectively too wide. Then you can work with 4 layer board and a thinner Top to bottom layer. Or if it is posiible you work with higher impedance tracks (it is the case if you work with high speed logic circuits by example). Please let me know if you have further questions. Good luck.

 

[House_Cat]

The results you got from the on line calculator are very close to the results I get with a field solver.

Your options to reduce the trace width are to reduce the thickness of the board, or run a return ground path in parallel with the top trace. The spacing of the ground path would be adjusted to give you the desired impedance with the desired trace width. This, of course, means two traces where you would have normally placed one.

Another option is similar, but the structure is different - you run your signal as a coplanar waveguide. To do this you run your signal down the center of a ground plane on the same layer (in your case the top) by making a slot of the proper width in the copper pour. The disadvantage to this method is the loss of space on the top of the board for other components because of the ground pour.

Reduced board thickness, or the use of internal planes with thinner dielectric between the signal and the return path is the most efficient if you have many components. Differential routing, using two traces (one is the ground return), is the simplest way to do what you want with only two layers and the same board thickness. The coplanar waveguide is the cleanest from a signal integrity standpoint, but uses more space on the top of the board. You will have to chose which compromise gives you the best solution for your particular board.

 

[edaedaeda]

If you can Do a co-planar wave guide with gnd plane reference you should be able to do something like the following:

board thickness: 0.062
ER: 4.6
trace width: 0.030
Trace to co-planar 0.0065
Your trace thickness is not correct if you are going to have plated holes. If you have plated holes on this design your copper thickness will end up being 0.0022
Also you want to make sure your Er is correct. Check this with your fabrication house.

Good luck
Eda