Is there a way to slow down the feed rate when making direction changes? I am cutting parts that have a lot of long straight lines and several small slots. If I set the feed rate high enough that it doesn't take all day to cut a part the inner radius at the end of the slots is pretty sloppy. I've slowed the feedrate and the quality of the inside corners improves dramatically. Outside corners don't seem to change with feedrate.

Will slowing the motor acceleration do this, or is there a better way?

Thanks!

Ryan

Put your fast feedrate for the straights and set a slower feedrate for the arcs, all done in your code with the F word. Or I may be misunderstanding what you are wanting.
Hood

That's what I'm wanting...sort of. The narrow slots are pretty long. I would like to slow the feed rate down when making the direction changes at the end of the slots then ramp it back up again for the long cuts.

Slots are .250 wide and 18 inches long.

I've noticed in the FRO DRO that Mach slows down when making abrupt direction changes (or it appears to). What I was hoping for was a way to manipulate this so I could cut the long side of the slot at a higher feed rate than the short sides.

I'm cutting foam and running at 35 ipm. The end of the slot looks pretty sloppy when traveling that fast. If I slow the feed rate down to 10-15 ipm the corners of the slot turn out much sharper. It would be far too time consuming to cut the entire part at a slower feed rate.

Any other suggestions or ideas?

Ryan

What I am meaning is alter your code, if its not too much code then it should only take a few mins to edit it to put a F15 in for the G2/G3 moves
As an example

G0 X0 Y0 Z0
G1 Z-3 F100
G1 X100
G2 X100 Y-3 R-1.5
G1 X0

That would cut at a feedrate of 100 for all of it


G0 X0 Y0 Z0
G1 Z-3 F30
G1 X100 F100
G2 X100 Y-3 R-1.5 F15
G1 X0 F100

That would feed at 30 for the Z  cut the straight at 100, the arc at 15 and then the next straight at 100.


Hood

Doesnt' this happen automatically when using cutter comp?
Joe

Joe,
No, cutter comp has nothing to do with feed rates. It is used for:
A: allowing you to program to the centerline of the spindle and then put in the radius of the tool used to properly position the tool, or

B: adjust for tool wear or for an undersize tool when programmed to the edge of a known diameter tool

Some CAM programs will adjust the feedrates for you, slowing it down for an inside corner, and speeding it up for an outside corner, the idea that the feedrates to the edge of the tool (where it's doing the cutting) will be different from the centerline of the toolpath as programmed

HTH

Mark

Thanks for the primer on the obvious features of cutter comp. When cutter comp is enabled, the controller calculates the feedrate on the contour, not the toolpath, so in the above scenario, it would slow the feedrate at the ends of the slot.
Joe
1st class machinist
Moldmaker
CNC programmer

Looks like editing the code is the way to go. Shouldn't be more than about 12 or 15 lines to change. I'll give it a shot and see what happens.

Are you running in Constant Velocity mode or Exact Stop? CV must round off corners since we can make instant changes to direction. Exact Stop will slow to a stop, then make a square corner and accelerate back up to speed in the new direction.

Mach starts up in the mode selected on the Config->General Config menu in the block called Motion Mode. You can change the mode in programs with G61 or G64.

Are you running in Constant Velocity mode or Exact Stop? CV must round off corners since we can make instant changes to direction. Exact Stop will slow to a stop, then make a square corner and accelerate back up to speed in the new direction.

Mach starts up in the mode selected on the Config->General Config menu in the block called Motion Mode. You can change the mode in programs with G61 or G64.

You may have just made my day Ron!!! What are the effects of running exact stop vice constant velocity if any? How does it effect arcs at the end of straight cuts. Does it stop there also before cutting the arc?

I would think exact stop would have more of a tendency to leave tool marks every place it stopped. True?

I should clarify that the slots I'm cutting are square ended (no arcs). There are however arcs being cut elsewhere in the workpiece. That's my reason for the above question.

Ryan