This will be a long post. Its late for me, so I will try to add some examples and links to specific youtube videos or tutorials in a later post.
There are several types of images and types of carvings that can be created from them, depending on the software you are using. Generally you cannot rely entirely on software to do everything for you - for every image type you will need to provide some context as to what you want. For example, most image formats do not include any size information - do you want that image carved 10 inches or 3 feet across. In most software, that is one of the first steps, choosing the size of your workspace. The software will generally allow you to resize the image to fit the output size you want.
After reading below - I urge you to follow the advice above and use a demo of several software programs and try each type of image - most of the programs have tutorials for some of the types of image below. Usually there is some sort of 3D display that you can rotate on screen to get a sense of what the carving will look like, and often a “simulation” where you will see the bit moving around and removing material like the CNC will, starting with a simple block (you will define the “stock” size the machine will start with) and ending with the finished part. You will also choose a point on the stock (often a corner, or the center) that is the origin that represents X0, Y0 and Z0.
1. CAD file. This is where you specifically design something you want cut in full 3d. For example, the body of an electric guitar. There is a “profile” or outline of the part, and there are “pockets” or areas carved to different depths, and there may be holes, which might be through holes or just to a certain depth. The CAD file contains the full definition of the part - but you will still need to add context to instruct the computer when doing the CAM part - creating toolpaths or the instructions for the CNC. For example - what size bit will you use to cut the outline, how deep will you cut on each pass around the outline, will you leave tabs connecting the cutout part to the rest, etc. Often you will choose to use multiple bits, perhaps a large diameter one for larger areas (roughing) and a smaller one for more details (such as smaller holes or radiuses). Fusion 360 is an example of a program you can use to do both the 3D design of a part and the CAM portion in one program (free for hobbyist or under $100K/year commercial use).
2. Vector image - for example an image created in Adobe iIllustrator or Corel Draw, an "SVG" image downloaded from online or even a DXF file exported from AutoCad or other programs. Think of words or logos. These can be imported into software such as V-Carve pro ($799), Aspire ($2000) or ArtCAM ($360/year), or f-engrave (free) and you will be able to create toolpaths. Here the context you are adding is if you want the image raised (background cut away), or recessed ( the image cut to a certain depth) and by how much or if it is a line image, carving along the lines (V-carving). You can create this type of image directly in this software as well. The “vectors” are mathematically defined - there is no “dots” or pixels in the image - smooth lines and curves as far as you zoom in. You also need to choose the size of bit you are using (large bit for big areas, smaller for more detail. For V-carving you will need to decide on the angle of the V - bits are available from 30º - 120º. Different angles will have a major impact on the appearance of the carving.
3. Monochrome or a few solid color bitmap. This could be a black and white image - on the screen may look just like the vector images - text or logo etc. But if you zoom in, you will see that the image is make of dots or pixels. These can be imported into these same software titles and “traced”. This means the software will “outline” or create vectors from the bitmap, and then you proceed as in #2. Usually the program will do each solid block as a separate closed vector (outline) in one quick step.
All of the items above are carved as vectors - series of curves and straight lines. G-code only handles straight lines and arcs - the software doing the CAM will approximate any other type of curve using straight lines and arcs. You can usually assign a tolerance value - how far the approximated path of the tool can deviate from the mathematically perfect path. The smaller the tolerance, the more little straight lines and arcs are used. You will see the CNC move directly around your machine like the curves on the screen look.
The next image types are carved differently - they are raster image formats and get carved like an inkjet printer prints - you will see the router go in parallel lines, back and forth, with the Z axis going up and down. This can be very time consuming, depending on values you will set for the size of the bit (usually a ball end bit - so the diameter ) and the “stepover” or distance each row is from the previous - usually defined as a percentage of the diameter of the bit you use. The smaller the bit and stepover, the more rows of passes and the longer it takes. The more detail the better it looks The G-Code itself is still just lines (usually no arcs) - they are just lots of short moves across and up and down.
4. Bitmap images designed specifically for CNC carving (reliefs). These are special grayscale images that are set up so that the color of each pixel encodes the relative height of that point. For example a light colored pixel will high, and dark low. Again, you need to provide context in the software - what distance do you want between high and low - 1/8 of an inch or 1 inch? Think of a topographic map, where the color reflects the altitude. There are sellers of these images or they can be created by 3D scanners. Often these reliefs can also be created directly in programs such as Vcarve, ArtCAM or Aspire by operations such as extruding a vector or sweeping a vector along another one, or revolving one. Even though these are mathematically created shapes - they get carved in the row by row format. Autodesk has free software for smartphones that can create a relief from a series of pictures you take of a physical object from multiple angles. Lets say if you have a carving you need to reproduce.
5. A standard bitmap image (photograph, etc.). The software will attempt to analyze the image and create a relief - some programs do this better than others trying to infer relative hight by analyzing shadows - some just treat light areas as high and dark as low. Some images work very well, others do not. The tiger image you linked to would probably not work very well without some work (isolating the tiger from the grass background, etc.)
Others may be able to add additional formats, but I believe the above are the major types. As you can see - for every type of image you start with (or create) there will always be something you need to define or do to create the toolpaths.
Finally, the toolpaths (expressed as a g-code file) gets loaded into your machine control program (such as Mach, WinCNC or LinuxCNC) these are the programs that execute the g-code and actually operate the CNC. This program will need to be configured specifically for your CNC. You need to set up things like how many discreet "steps" it takes for each axis to move 1 inch (or mm), and how fast your machine can move (inches per minute). If you buy a machine, the manufacturer should preconfigure this for you. If you build one, you need to do this yourself. This is generally a one time operation.
Finally, you will need to locate the stock on the table of the CNC and set up the machine to the same origin that you defined way above when you started (remember that X0, Y0 and Z0?). Then and only then will you be able to carve.
All this sounds intimidating. It is merely a set of skills and terminology that need to be learned. Download demos, follow tutorials and it will make more sense. Ask questions. You'll get there.
Richard