Feed and Speeds in VCarve

Just got off the phone on an interesting tech support call that I thought might be interesting to y'all...

Customer was loading files into fabmo-- on some files the tool would go to the start point of the cut dive down--then immediately lift up and go back home and end the job...skipping the whole file.

Some jobs worked and other didn't...so I looked at a set of his files. In the working file the feedrate designation at the start of the file read "MS, 0.1, 0.0" which would mean a feedrate of 0.1inches per second in the X and Y axes and a feedrate of 0.0 inches per second in the Z axis. Seemed like an obvious problem...however, the file worked and seemed to just use the non-zero value for the Z axis in the absence of any other speed info.

The files that didn't work had "MS, 0.0, 0.0"...but the customer swears he has speeds in VCarve...
So what are the speeds?
4 inches per minute
which works out to 0.066 inches per second.

Looking at the code for the inch post processor for VCarve I see that it multiplies inch/minute speeds by 0.0166 and rounds down to the nearest 0.1...so anything less than 6 inches per minute will be rounded down to zero.

However, the handibot is totally capable of moving at 0.05 inches per second...or even 0.0000005 inches per second if you want.
He just had to go into the code and manually change the MS command to MS, 0.06, 0.06

Weird bug that was producing very strange behavior when he described it over email...thought you might find it interesting!