On FR-4 material you can get down to about 0.10 mm (4 mil, 0.004") trace widths.  

OH, and the tolerance is about +/-1 mil (0.025 mm) so make sure you take that into account on the transmission line.  

A microstrip of 0.3mm (.012 mil) is no problem on FR-4 for in a general use RF design (I assume you are on FR-4). Actual width may depend even upon how old the gerber photoplotter your board vendor uses, and how consist his process is from run to run.

Other factors for FR-4 (which I assue you are using) are dielectric variations lot-to-lot, the actual frequency of the signal (dielectric varies slightly with frequency), actual weight of the copper (copper thickness) and the prepreg glass content of a multilayer board.

Assuming your 0.3mm is on a multilayer (would have to be if it's 50 Ohm) the required width may vary with how much the copper is pressed in the prepreg in the lamination phase, which then again is dependent upon the glass/resin ratio for the particular prepreg(s) used to obtain the desired thickness. Then again, dielectric constant can vary slightly from one FR-4 manufacturer to another

Then again, many of the forumulas used to calculate the width of a microstrip are only approximations, and they vary when compared against each other.

What I'm trying to get at is there are a lot of approximations in getting to a solution for impedance matched traces on a PC board. You get close and that's fine for 90% of all designs. Unless you are working on a Teflon substrate, and measuring afterwards with a network analyzer to adjust your design, what you end up with is only a approximation.

It is OK to manufacutre such a width.

The only think you have to consider before you will order your PCB is what type of software did you use for optimization. If it wasn't any real 3D or at least 2.5D simulator so You have to expect that measured results compared with simulations will be more or less (depending on working freq.) shifted.

This all sounds like good information here so I would like to ask a question without starting a different post.
What do you think the advantages and disavantages of FR-4 vs polyimide for microstrip work in the sub 2 GHz range?  Also, is there something other than a genenric FR-4 to get lower variation in RF properties between batches or even vendors on FR-4?

Well, the only advantages of FR-4 is that it is cheap and it is good enpugh for RF circuits.
Disadvantages are changing RF properties depending on vendor. Problem is that every vendor prepare the whole material itself. Compared with for example ROGERS materials, which are very stable despite the vendor, all materials needed for preparing of PCB needs to be bought from ROGERS.

You should also keep in mind that FR-4 is more lossy then other materials. But it is nothing wrong sometimes. Thanks to it You can achieve better backward isolations, better return loss in wider freq. range, spurious signals on higher freq. are more attenuated etc. etc.

Other alternative which is a bit better then FR-4 and not so expensive as ROGERS and other teflon materials is BT-epoxy. But, sincerly, I have no idea who is using it nowdays. MAybe someone from this forum have same info?