I would like to take advice from experts. I want to know that when we design the PCB how much size of trace should keep.

I hope someone has experience with eagle. When do you design PCB on eagle, How much size of trace do you keep ?

 

I make my boards on a CNC mill. It can manage 0.3mm tracks and spacing (0.2mm at a push) so that is the minimum that I use. I will use wider tracks for higher current traces (a different 'class' in Eagle speak) and maybe for ground traces if I don't have a ground plane.

If you are making your own boards the method you use will have a minimum it is capable of doing reliably.
If you get a board made commercially then the board house will specify their limits.

 

Designing an ultra fine line PCB for production is very different from designing for hobby interests. The key objective is manufacturability. You want to make sure that the PCB can be made with consistently reliable traces. In that regards, I will opt for wider traces and wider spacing rather than go for the finest.

Even though the PCB shop may have excellent fine line capabilities, I would opt for 12t to 16t (0.3-0.4mm) if space allows.
Power rails could be as large as 20t to 50t (0.5-1.3mm) and wider if the current demands it.

With DIP 0.1" through-hole pin spacing it is common practice to route one or more traces in between pads. In general, I would avoid routing any trace in between pads if it can be avoided. I would not route a trace under an 0805 SMD component.

In summary, 16t (16mil) trace width is a good place to start.

 

It might go without saying but I'll say it just to make sure it is covered: Trace width is also a function of the amount of current the trance needs to carry. Higher current means a wider trace, and possibly a parallel trace on the other side of the board coupled with vias.

 

If you get a board made commercially then the board house will specify their limits.

When I design PCB in software, I set the trace size and hole size. Does this mean that if I send my design to manufacturing house, they can change parameter like trace size or hole size. Does it happens I don't know about it.

 

If you get a board made commercially then the board house will specify their limits.

Look at the manufacturers web site. They will give you specifications on how small a trace they can produce and how small a hole they can drill. Keep in mind, though, that you don't always want the smallest hole or the narrowest trace. Some manufacturers will charge for the smallest holes and finest traces.

Designing an ultra fine line PCB for production is very different from designing for hobby interests.

MrChips makes a good point. Production PC boards will need to be designed properly so that the bare board manufacturer can actually build them at a reasonable cost. As traces and part lead pitches get smaller, a board may cost more. Additionally, constraints may be placed on a board so that pick and place machines can properly place the parts and so that during reflow the parts are soldered correctly. I've used assembly houses that asked to modify my design to avoid problems during assembly, including part tombstoning as well as solder shorts circuits.

If you are designing for hand assembly, you will need to determine what you can assemble and how much you want to spend on hand assembly tools. The PC board design should allow you plenty of room for soldering irons or hot air reflow tools.

Probably what you should be most concerned about is DickCappels point. You'll need to review what each net does. If it carries a large amount of current then it will need wider traces and larger plated through holes. Most digital traces and low current (less than 10 mA) analog traces can use a 0.008 inch or 0.010 inch trace. Power supply rails and ground returns should be wider. Outputs to motors, solenoids or other power devices should be wider as well. Remember too that a wider trace has a lower impedance, very important in some analog circuits.

Before you start your PC board layout, you should list all signals that will carry large currents, determine the expected current for each signal and specify a trace width that can carry that current.

 

It Eagle it's easy to define several traces configurations. Simply edit the Net Class rules to match the desired 'net' with the desired trace parameters for the board.

https://www.autodesk.com/products/eagle/blog/what-you-didnt-know-about-eagle-net-classes/

 

When I design PCB in software, I set the trace size and hole size. Does this mean that if I send my design to manufacturing house, they can change parameter like trace size or hole size. Does it happens I don't know about it.

Usually they shouldn't, unless you push their technical limits. Most FABs accept minimal trace widh and clearance 6mils (about 0.154mm) and minimum drill 0.3mm as standard and also cheapest requirement. If you want thinner tracks and smaller drill size then you are charged by their higher requirements prices.