Can I submit bitmaps to be used for PCB silkscreen?
Since there are probably not hard and fast rules to this, I will give you my marginally informed opinion.

To the best of my knowledge, no, you cannot submit bitmaps to a PCB fabricator. PCB fabrication houses work from gerber files. Any silkscreen artwork must be converted into the gerber format in order to be reproduced on a PCB.

The gerber format basically allows you to draw arcs or lines and to flash apertures. An aperture is an arbitrary shape which may be "flashed" onto the relevant layer. Rectangle and circle apertures are default, pre-defined apertures. Basically the aperture can be thought of as an opening in a screen where ink will be applied. Arc and line width may be varied arbitrarily, however, there is probably a minimum acceptable line width that is vendor-dependent. I think 0.005" (0.13mm) may be a ballpark number for silkscreen layers.

Apertures are solid images, not outlines. The purpose of the aperture is to allow odd shaped pad sizes for components. There will obviously be some resolution limit on features in an aperture. Features that are 0.005" (0.13mm) or smaller may not reproduce very well. It would probably be best to think of the aperture in terms of drawing the outline with a 0.005" (0.13mm) wide pencil on a square grid with 0.010" (0.25mm) grid spacing.

If you can produce your artwork within these constraints, it may be reproduced acceptably on the PCB.

As far as I know there is no limit to how many custom apertures may be created. An entire image could conceivably be created using thousands of unique apertures.

The copper layers support noticeably higher resolution. In some cases, you may be able to put your artwork in the top or bottom copper layer. This is still clearly visible, but in a more subtle way compared to silkscreen artwork. There is a lot of vendor variation in minimum line width in copper layers, and it also depends on how thick the copper is (18 micron vs 35 micron, etc). Check with the vendor on minimum copper track width for your board. Often, for boards with 35 micron copper, the minimum track width on copper layers is 0.004" (0.1mm). But finer widths are available with better suppliers. These finer widths may make the PCB more expensive.

As far as actual conversion of artwork to gerber, I really don't know if there are sophisticated tools available to do it either intelligently or with fine-tuned control. For absolute best results, it might be wise to start with line drawings where the minimum line width and minimum space between lines is 0.005" (0.13mm), and import these as vector graphics. Large areas which need to be filled can be filled with repeated lines, or with simple shapes such as rectangles and circles.

Also, avoid splines. Gerber files do not natively support splines. They must be approximated as multiple arcs or straight line segments.

You can find extensive detailed technical information about gerber files here:
https://www.ucamco.com/en/gerber

Gerber files are text files which can be read using text editors. Perhaps it would not be too difficult to write a script to inject custom artwork into a gerber file.