Is there an ideal PCB trace width for data lines?
The resistance of the traces is seldom important for signals. Wider traces have lower characteristic impedance (transmission line impedance) than narrower traces. Sometimes this matters.

For example USB and ethernet. In those cases, the trace width must be chosen so that the impedance is correct. RF signals, such as GPS or bluetooth or wifi antenna signals, have very exacting trace impedance requirements (usually 50 Ohms). Video signals usually are required to be routed at 75 Ohm impedance if they go off-board.

The second major factor which affects impedance is the distance from trace to the nearest plane. One useful rule of thumb is that a trace will have approximately 50 Ohms impedance when the trace width is double the height from trace to plane. This is for traces on top or bottom, not inner-layer traces. So a 10 mil trace separated from GND by a 5 mil dielectric will be around 50 Ohms characteristic impedance.

For more accurate numbers, you can use a trace impedance calculator online.

There is some relationship with trace width and board cost in mass production. If you need to mass produce PCB's at low cost, the minimum trace width should not be pushed too hard. Best is 5mils, but 4mils is OK, too.

Also, the copper thickness affects the minimum trace width. If you ever use something thicker than 1 oz (35 um) copper, you will want to increase your trace width and spacing. I can't give you the limits off the top of my head, but you can research it if you ever need to do that.