Ramping Into A Profile

[partsman]

I have been evaluating several CAM programs looking for a program that will let me ramp into/out of a profile tool path. Why don't most CAM packages allow you to do this? How is everyone else getting around this? I always see "don't plunge cut or you will shorten tool life" but I have yet to find a good way to router out parts from a sheet without plunging. Any suggestions or comments?

Thanks in advance

[LeeWay]

Sheet Cam ramps just fine for me.

[Ken_Shea]

Partsman,
A couple of options,
1) Draw your own ramp into the existing profile..
2) Pre-drill a hole location outside or inside the profile that allows you to plunge into the pre-drilled hole and then proceed with the horizontal cut in x or y.

I have wondered why the no ramp myself in my own cam software.

Ken

[Jason Marsha]

Try VCarve Pro from Vectric.

Jason

[genem]

A good machining practice would be to Pre-drill a hole If you have a 3/4 end mill use a 7/8 spade drill or indexable, Most of your higher end Cad/Cam programs such as Catia and Unigraphics will have Ramp in/Ramp Out Geometry, You can control the Direction, Length and Feed.

[partsman]

Thank you everyone for all of your suggestons. I had just tried all of your suggestions to see which would be best when I got a call from VisualMill. The new version 6.0 will ramp into profiles!!!! AND it will be available as RhinoCam V2 due out soon! I already use Rhino to do all of my CAD work so I think I found exactly what I needed.

Thanks again for all of your suggestions.

Aaron

[bp092]

vcarve allows ramping, I don't recommend plunging down a z at all, especially not with spiral cutters, I always ramp when I can.. it extends the life of the tool and spindle significantly and really doesn't add a lot of time onto toolpaths

[dapoling]

Another option to this that I use at the machine is to write a little program at the machine using the current tool that you will be machining with and has less tool pressure then just ramping from point a to b.
It is a simple helical mill that is used with a M97 subprogram call up.

example:
%
G0G20G40G80G90
M6T1
G0G90G54X0Y0S3000M3
G43H1Z2./M8
Z.1
G1Z0F20.
M97P1000 (THIS CAN BE CALLED UP MANY TIMES FOR THE SAME PATH AND WITH OUT CHANGING PROGRAMS)
(CONTINUE AT PROGRAM DEPTH)
G0Z2.M9
G91G28Y0Z0
M30

O1000
G91X.0625
G3I-.0625Z-.01L10(ADJUST AS NEED THIS WOULD BE .100 DEEP)
I-.0625
G1X-.0625
G90
M99
%

[ExMachina]

Another sweet way to do this is feather in on a tangent circle.