Short answer:
Sounds like you are cutting too slow. With the specs you listed I would start at .1mm per tooth per rev which would be 2000mm/min. But my guess is your sweet spot will actually be much faster then that (2x-3x).
Don't fall into the trap that cutting slower is better. The problem is that the tool needs the cut material to cool it. If the pieces are too small then it's like spinning your tires. It makes some noise and burns up the tires (bits).
Long answer:
RPM:
RPM will be dependent on the tool you are using. Different manufacturers use different tool geometries which will mean they all have different good RPMs.
What you can do is try to get the SFPM recommendation for the material you are trying to cut then use the following. (3.82xSFPM)/tool diameter. So lets say your SFPM is 1200 (random number. I don't know that material) that would be (3.82*1200)/0.2364 (sorry don't have the metric formula handy)=19390RPM.
A simple way of thinking of this is that you are trying to get a good impact velocity for the flute of the tool. Too fast and you will have extra noise and kill your tool faster. Too slow and you will limit your feed and possibly have other issues, torque comes to mind.
Plunge:
A good plunge rate is always a game of trade offs. Go deeper and you finish sooner but you have to worry about tool deflection and increase your chances of breaking your tool.
A good place to start is usually 1 diameter of the cutter. So if you have a 6mm cutter that would be 6mm per pass plunge. You can increase your plunge but you put more stress on the tool and can increase tool deflection (the tool actually bends as it cuts). If you are having trouble with a material then you can decrease the plunge and it will take stress off the tool. This is almost always a better option then lowering the feed rate.
Feed:
Rule of thumb is based on a percentage of the cutter diameter. However, the best feed will vary with the tool geometry and material being cut.
If you want to know for sure where you should be, get some scrap material and run a test. Write some code that will start you at one corner then start with your starting feed and cut a "V" then repeat the code increasing the feed at every end point (see code below).
Here's a code example to show you want I mean. If you try to use this you need to zero your machine in the bottom corner piece of your material with your Z being zeroed at the face of the material being cut. This code also lacks a header, one would need to be added. Again, this is an example I just wrote up to demonstrate the process. If you use it in any way you need to check that it will work on your CNC and check the code for errors.
I TAKE NO RESPONSIBLY IF YOU USE THIS CODE AND SCREW SOMETHING UP.
Code:
G90G0 (Absolute programming, rapid)
X0Y0 (Zero position)
Z-6F10 (Plunge 6mm into material)
G91 (Incremental programming)
X25Y6F2000 (Move 25mm in X and 6mm up in Y at 2000mm/min)
X-25Y6F2000 (Move back to starting X and 6mm up in Y at 2000mm/min)
X25Y6F2100 (Move 25mm in X and 6mm up in Y at 2100mm/min)
X-25Y6F2100 (Move back to starting X and 6mm up in Y at 2100mm/min)
X25Y6F2200 (Move 25mm in X and 6mm up in Y at 2200mm/min)
X-25Y6F2200 (Move back to starting X and 6mm up in Y at 2200mm/min)
X25Y6F2300 (Move 25mm in X and 6mm up in Y at 2300mm/min)
X-25Y6F2300 (Move back to starting X and 6mm up in Y at 2300mm/min)
X25Y6F2400 (Move 25mm in X and 6mm up in Y at 2400mm/min)
X-25Y6F2400 (Move back to starting X and 6mm up in Y at 2400mm/min)
X25Y6F2500 (Move 25mm in X and 6mm up in Y at 2500mm/min)
X-25Y6F2500 (Move back to starting X and 6mm up in Y at 2500mm/min)
X25Y6F2600 (Move 25mm in X and 6mm up in Y at 2600mm/min)
X-25Y6F2600 (Move back to starting X and 6mm up in Y at 2600mm/min)
G90 (Absolute programming)
Z10 (Lift tool 10mm above material)
This will allow you to test what feedrate works best for you. Each "V" will be a different feed rate and you can then evaluate them right next to each other. You will also hear a changes in the sound of the cut as you go. If it starts to sound really bad stop the cut as you are probably exceeding the tools ability.
Machine:
Keep in mind that all of the above can be effected by your CNC. Runout, flex, backlash, spindle/router specs, and tooling. All of those can limit how you need to cut.