Sudo:
Yes, chatter actually always happens. There's a tiny bit of chatter in every cut, simply from the force of the cutting edge making that initial contact with the material, which deflects the bit, z-axis carriage and gantry system. It's more pronounced in machines like ours that flex, but even the big monster machines show chatter marks.
For really bad chatter, there are typically two places to solve this.
The first, major one, is really more "judder", where the movement of the whole system seems to move in spasms. Horrible to watch! That one can usually be solved by cutting less deeply per pass. In some designs that are more "machining' than carving, you can sometimes control that effect by choosing which axes the bit is moving in (more on that below). In carving type designs, there's less opportunity for that control, other than maybe setting the angle of the cutting passes.
The second one, the one you're most likely experiencing, is good-old chatter. This is actually a resonant phenomenon of the whole motion and cutting system vibrating with the material. Depending on your spindle RPM, changing that up or down by just a few percent can move it out of resonance. If there are multiple passes being made, that initial chatter can actually force the system into even more chatter when the bit hits those even-harder-to-cut chatter bumps.
If I'm seeing bad chatter, and I know it's coming around for another pass, I'll sometimes kick up the RPM by a couple thousand RPM, to give it more power to cut through, and then I'll put my hand on the spindle motor to steady those vibrations. Typically doing that once will smooth the surface enough that a smaller change (~200 RPM) will do away with that chatter on the next pass, and it will slowly reduce to nothing. But, that might very well be due to the way those cuts were being run, not necessarily any great technique. I did notice that if I just gritted my teeth and let it go, in 3-4 more passes in the pocket, the chatter marks were gone.
And really, that's an important criteria to consider. If the amount of chatter is so much that it looks like it's damaging the machine with that flex, of if the cutting effects the final cut surface, then yes, it should be dealt with and removed. But, if the chatter just sounds horrible, and those chatter marks are going to be cut off in the next pass or two, then in most cases, I've just ignored it. I mean, do I really care if there are chatter marks on material that is going to be completely removed in just a minute or two? Nope, those can stay!
But, if those marks ARE affecting the surface finish, then my advice is to add an allowance of about 0.015-0.025 in wood, and 0.005-0.015 in metals, onto those roughing toolpaths. Then, come back through with a separate, high-RPM, VERY thin stepover finishing pass to remove that final amount. Because the stepover is so much smaller, you often want to use a longer depth of cut too, so there are fewer overall passes, and those will be using the same cutting edge. And, if you run that same finishing path twice, that will often leave very nice surfaces.
All that said, our Sharks have a special issue: their cartilage. Because each axis adds at least a little plastic into the chain of floppiness, HOW you cut can sometime be important. But first, let's establish our axes. I'm going to say X runs along the width of the gantry, across the T-slots. Y runs along the length of the T-slots. And of course, Z is vertical. When working at a single Z-axis height, the X and Y will have different characteristics depending on the movement. In the X axis, as it moves back and forth, the forces on the bit will cause the z-axis carriage, and thus the bit, to "rotate" around an axis in line with the Y axis, and will deflect in the XZ-axis plane. This is usually a reasonable amount of flex, and should be considered your "strong" axis. Because the Z-axis carriage sags downward, when the Y-axis is moving toward the router, the bit will tend to dive down into the material. In the opposite direction, when the Y-axis moves in the direction away from the router, it's pulls the bit, and that tends to make the z-axis carriage flex UP and out of the material. In the Z-axis, plunging and drilling when done "too" fast, will flex that carriage up, and you'll get an elongated hole where the initial cut is not on location in the Y axis, and depending on the material and RPM, it can even throw the bit a little in the X-axis direction.
On difficult cuts, like a full slot that goes deep into the material, pushing the bit along the Y, using a square-tipped end mill should be avoided, but pulling the bit is often fully successful, since the tendency isn't to dive deeper and deeper into the material. This can also be greatly helped by using "radiused" endmills, with those sharp tips precision-ground to some radius. (If you're haven't tried radiused endmills, y'all be cray cray!)
But, I digress. You're using a v-bit, so you won't likely see much diving, since the slope of the cut will tend to push the bit upwards. (Yay!).
I try to not push their site too much, but CNC Cookbook has a great series on machining; it's mostly for metals, but the same rules apply. Here's there article on chatter and how to avoid it:
http://www.cnccookbook.com/CCCNCMillFee ... hatter.htm
Hope that helps, 'cause chatter SUX!
Regards,
Thom