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 board
The 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 1.4mil
required impedance 50 Z
calculated 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 helps