One of the lesser known features of Mastercam is Arc Filter Tolerancing. When this is disabled, Mastercam outputs lines instead of arcs for all of it’s movements. This leads to both stuttering of the machine and Faceting of the parts.

Example

When Enabled, Mastercam uses the tolerance to smooth out the toolpath within the tolerance.
Machines are able to decode and interpolate arcs far faster and with greater feed than lines which will usually be about .010 long.

If you are roughing, you can increase the speed of the toolpath drastically by enabling this properly. 
My suggested settings are below

Cut tolerance and line arc tolerance both are a part of the total tolerance. My suggestion is to set the default to 50% on both. My understanding of the difference between cut tolerance and line arc tolerance is this.
Cut tolerance is the distance between the model and toolpath. 
Line arc tolerance is the max distance between the arcs being generated and the lines that Mastercam would have used if the feature was turned off.
This means that while you might finish with a part that is up to the total tolerance different from the model, what usually happens is the part is only different where the arcs are concerned, and then, usually only by half the distance of the total tolerance.
Mastercam does not go into detail about what either of the options actually does, but the total tolerance is your deviation from the model. This means if you are leaving .025 on a surface so you can come back to finish, you could set your tolerance all the way to .025 without gouging the finished part. This is overkill though because unless you are trying to machine at 100Ipm or more, a total tolerance of .005 is sufficient. There is a con to using arc filter tolerancing though. It takes much longer for Mastercam to filter all of the points into arcs, and it usually does not change anything about the toolpath other than the code that is outputted. For this reason, I prefer to leave it disabled until I am ready to actually post the program to eliminate extra processing time for the computer.

There are a couple of sub options that I will explain.
Most machines are not able to process arcs in xz and yz so I would leave those disabled unless you are running raster passes over an arced vertical surface, like a sphere or a speed bump.
One way filtering should always be selected or you may get micro gouges or mixed facets.
I would not suggest using the smoothing setting as it causes micro gouges in most surfaces.
Output 3d arc entry is another option that is very important to have selected if your machine can helix down. (most newer machines can, but ones from the 90’s or before are not.

The important takeaways are:
Only enable it before posting.
Total tolerance should not be more than .025 or less than .0025 for roughing, more than .005 or less than .0005 for finishing. Going outside these numbers may cause Mastercam to take either too long to process, or it just won’t output arcs.
Always use one way filtering.