4th Axis G code issue

When I enter
G1 A-85 X-47 F200
into the MDI, it does not use the F200 feed rate. Instead seems to use the default feed rate, but if I enter
G1 A-85 F200 it does accept the lower feed rate. Can anyone clarify why you cannot specify a feed rate when there is more that one parameter?

I would hazard a guess that Pathpilot is timing the moves together so that both motions end at the same time. Is that what you see, or does X or A finish while the other is moving?

The diameter of the workpiece is 57.33mm. The first move (A-85) is from A0, so it is 85 degrees or about 40mm. At 200 mm/min, it should take about 12 seconds. The X move is only 3 mm, which as you point out, should start and end at the same time as the longer move. What I see, however, is the whole move in about 4 seconds.

A is a rotary move, so F is interpreted in degrees/minute for that axis. PathPilot has no idea what the stock diameter is so can’t make the calculation you describe.

To do that, you need to select inverse time feed mode - see G Codes (linuxcnc.org)

G1 A-85 x-47 F5

Will perform the move in 1/5 minutes or 12s.

Once G93 is in effect, every move must be accompanied with a F word.