I need to draw a trace of characteristic impedance of 50 Ohm using Allegro 16.2.
I also want to verify that it is actuallly 50 Ohm of characteristic impedance.
Could anybody please tell, how I can draw it and verify it.
Hello on the higher tier Allegro tools there is a RF module that would allow you to draw that trace as a shape but on the lower tier products there is another way to do it.
Since a trace of a specific impedance is really characterized as a "Transmission Line" the first thing you will need is a Transmission Line calculator to assist in figuring out the width of the trace.
Here is a link to a good free tool to use.
Things you need to know in advance would be what is the layer stackup of your board, 2lyr, 4lyr etc. Your trace will be above a ground plane when complete. The important things are the w/h width to height ratio and also the er constant of the material and the thickness of the conductor.
So lets assume you want a 50 ohm impedance trace and you are using 1oz copper and have a standard 0.062" double sided finished boardThe numbers work out like this.
Actual board thickness 59.6 mil "measured copper top to bottom"er of FR4 = 4.5 typical "Check data sheet first, make note of intended frequency of use"trace thickness 1.4milrequired impedance 50 Zfrequency 100Mhzcalculated width of trace = 110 Mils
Ok so we worked out the calculations for a MLIN and can see that our trace will need to be 110 mils wide.
In allegro you can draw that trace just like a normal trace or you can use a rectangluar shape instead. I prefer to use a shape for transmission lines.
Keep in mind the trace is a simple straight trace, if you have bends or curves the impedance will change but not by too much. Also do not have a ground plane or other copper close to your trace because it will change the impedance of the trace if it is close.
To verify your trace is indeed 50 ohms in the real world you are going to need access to a VNA "Vector Network Analyzer" the VNA will be the true test :)
If the trace is truely 50 ohms you can expect a returnloss of > -30dB across your band of interest.If you could provide some more specifics on your board/application I could possibly further assist.BTW in the real world a handy way of making sure your traces are really the impedance you want is to do a test board first with lines of different widths that can be measured with a VNA. Every board house has different process to make a board so the material you receive from one board house might not be the same as from another and these little difference can change the actual real world impedance of the traces.Hope this helpsThanks Scott.
Thanks a lot for your reply.
Actually my application frequency range is 100M to 4GHz. The board is two layer ( top & bottom layer).
Also what is generally the minumum possible spacing of other copper from the traceto ensure it doesn't affectmuch .
16.2 also has RF Module . Won't it work ?
Well I see you are wanting a controled impedance from 100Mhz to 4Ghz so a better idea than a standard transmission line is to use what is called a "coplanar waveguide" this will keep the impedance more uniform over your required bandwidth.
It is best to work out these kind of things with a RF simulator, Allegro is pretty good for doing the etch but a rf sim is king here. There used to be a free RF sim from Ansoft called "serenade sv" this program can help you figure out the math in a easy way.. Try google for it.
fyi a coplanar waveguide on a pcb is a trace above a ground plane with another ground plane spaced away from the trace a certain distance. Think of it as a trace that has a copper pour around it on one side of the board.
For a 2 lyr 1oz copper fr4 board with a er constant of 4.5 and a thickness of 59.6 mils you would be looking at using a trace width of 40 mil above a solid ground plane, assume the trace is on the top side of the board. An additional ground plane either side of the trace should be used, the trace must be 19 mils away from the edge of the top side ground plane. I used a trace length of 3 inch in that example. When dealing with microwave frequencys things can get critical real fast. Simulations can go out the window in a flash. Pay careful attention to the material you use. Dont assume anything. Stuff like connectors "SMA" and poor data sheets on the imput impedance of a IC Pin can blow up the work you put into getting your pcb transmission lines correct. What I mean is your board might be perfect from the perspective of returnloss S11 on that transmission line but the components at the end of the transmission line will and can degrade the whole system performance. So your original intent of a good match can turn into junk pretty quick. You cant really think of the PCB as an island in this regard because it is not. You kind of have to think of the system as a whole. Can be difficult to get right :)
Other note, Plating of the transmission line will change the impedance only slightly. Keep solder mask off the line too. You can also stitch the top and bottom ground planes together with small vias along the length of the transmission line. Doing this reduces the inductance of the ground planes between top and bottom side of the board.
Hope that helps