You can use Autodesk fusion to determine feeds, speeds and cut depths per pass for the bit you are using, even if you don't want to use their CAM. You should always reduce the given feeds, and pass depths by 50% if you are not an advanced user. For newer users, I don't recommend going slower or faster than 50% of the given feeds as these will give a good chipload at BoXZY's achievable spindle speeds (start the mill around half of full speed and adjust based on results). This is really important for keeping the part and bit cool. The only thing you'll want to personally determine is step-over (vs depth per pass in some cases). Keep in mind the first cut is usually cutting on both sides of the bit, this is the hardest part on the bit. When doing a step-over the machine is only cutting on half the bit and can more easily shed chips (go to advanced information below to know more about how to take advantage of this). Here's a few details:
Brass and aluminum - Material clearing with a 1/4" bit: I wouldn't personally exceed 1/16" depth per pass, 1/32" per pass is safest for quick clearing, go even lower for higher tolerances ( less than 25% of the tool diameter is a good rule for max depth on very hard materials). You can infinitely reduce the depth per pass based on your comfort level without any real issues. Max step-over should be 20% of the bit diameter, I recommend 15%. You can always go more aggressive but it adds noise and stress. I use midway between 3 1/2 and 4 1/2 on the Makita speed control, depending on the hardness. WD-40 should be occasionally applied over the part when milling metal (cover the part, not the bit).
Wood and plastic - Material clearing with a 1/4" bit: I wouldn't exceed 1/8" depth per pass for an internal cut, 1/16" gives really clean results (50% of bit diameter is a good rule for max depth per pass on softer materials). A step-over around 25% of bit diameter works well. For plastic, create a conservative toolpath that will not overheat the bit and melt the plastic. This can take testing and tuning.
The thinner the bit the lower the depth you'll want to cut per pass. I do this by percentage. If the bit is 1/8", I would not exceed 25% of the bit diameter or 1/32" max cut depth in hard materials and 50% of the bit diameter or 1/8" in soft materials . I even then still reduce it a little just to be safe.
- Some more advanced information -
You can use a lower initial cut depth when you are cutting on both sides of the bit and have a higher number for the step-over. Here's an example; I cut a raspberry pi case and I used my max depth to clear the initial cut with two passes, I then used a much more conservative step-over and cut away portions twice as deep as my initial max depth per pass to clear away material and enlarge the cutout (because I was then only cutting on one side of the bit).
You can also reduce the depth per pass and increase the step-over. Example: Do a 1/16" depth cut instead of a 1/8" depth cut and increase your step-over to 40% from the original 20%. This is just preference in my opinion. The cut takes roughly the same amount of time, though it's safer to get more aggressive with the step-over than with the depth per cut.