pcb prototyping fabrication with very low clearance and width

i am used to manufacturers like iteadstudio and oshpark that offer a couple of PCB prototypes for under 100$. This time i am making a PCB with more difficult capabilities, ~2 mil for track width/clearance because of BGAs. I am searching for a manufacturer that specializes in prototypes without a high base cost for mass production but also has some better capabilities than iteadstudio and oshpark, hopefully not going over a couple of hundreds dollars. thank you!

Your spacing should firstly be in hard metric as should your design as modern components are hard metric...
The 0.05 track and gap is far too small for reliable manufacture, why is it so small, I think you may have to review your design criteria....
I have done 0.5 and 0.4mm BGA designs where standard 0.1/0.1mm track and gap was used.
The world has been hard metric for years don't work in an outdated measurement system, its daft.

2mil width/clearance is quite difficult for normal PCB makers, maybe some Japanese manufacturer can make it, but I don't think you will accept their price. As said above, you might have to review your design.

Anyone will struggle with these sizes... its down to getting the etchant between the tracks and catering for etchback... the initial copper weight would be very small, even cutting edge manufacturers such as Wurth and others would struggle, more with the gap between traces.....
Look at the design, give us more info and maybe we can suggest a different solution......

It's possible, Würth Elektronik has a high end PCB prototyping service that can probably do it, alternatively ACB can also be an option. Be prepared to spend a lot of cash on your boards though.

"Your spacing should firstly be in hard metric as should your design as modern components are hard metric..."
thats good to know; i prefer metric but a lot of datasheets are still in mils, but ill gladly switch to mm.

i reviewed my design.
my BGA has a 0.3mm ball diameter and 0.5 pitch. I used NSMD pads of 0.25mm. I would like to be able to route a trace between 2 rows of pads, but this is not possible at 0.1/0.1mm, but its fine at 0.075mm/0.075mm or barely at 0.1/0.075mm. I am still deciding between those options: 0.075/0.075mm trace between pads, diagonal escape vias for middle row pad (not all pads have a signal), or micro-vias on pads. Please tell me if you think one of these options is better. My BGA has only 3 rows and space in the center.

After having reviewd my design rules, what would be examples of manufacturer that match those specs that you would recommend?

Thank you!

75 µm technology might be reasonable for 0.5 mm BGA. Vias in pads is an effective way to increase the circuit density, often more effective than blind or burried vias. Check the available options with your PCB manufacturer.

0.075 is available from the likes of Wurth previously mentioned, higher end manufacturers are more likely to be able to do it than cheaper houses. If a PCB fabricator can do controlled impedance designs he should be able to work to your geometries.....

I work for a pcb fabricator. based on what i know about minmun trace width and space for reliable fabricaton, it is safe to say 0.4mm trace clearance /width is very easy to be fabricated. in most of fabricators, 0.2mm trace clearance/width fabricaton standard does not require extra costs.
the 2 mil/0.5mm for track width/clearance design will be reletively expensive and only available in some high tech PCB fabricator. regarding to fabrication costs, i suggest to avoid dense trace design the PCB. If it is possible in your requirement, rearrange your trace layout, add extra layers or increase the board size will make the fabrication easier.