How close do you rapid?

[johnrobholmes]

I was once told by a machinist (while changing the machine parameters and overriding some safety functions to make a part) that 0.005" of clearance might as well be a mile. He always ran rapids to 0.005" clearance and didn't seem to have problems. I did the same on the Mazak and never had issues. But it was also a brand new machine.

How close do you cut it?

 

[bigjon61]

Usually .06" on our lathes. The crayon eating mill guys probably 10"

 

[gustafson]

chip under a part and break a drill?
no thanks

 

[Shawnrs]

I usually rapid to .05".

 

[Mtndew]

On lathes I rapid to within .1" on X and .05 on Z.
On mills, I rapid Z down to within .250" with a jump height of 2" to clear clamps and whatnot.
You can crash a lathe all day long, but crashing a mill will cost you big $$$

 

[DDoug]

For all of you "rapid within .001" are you in that much of a hurry ?
Have you Time studied the job to take out all of the other time wasters ?

 

[GregSY]

I use 10" and I'm usually chewing on a crayon when I do. Preferably magenta.

 

[gustafson]

mmmmm magenta

[burp]

 

[TeachMePlease]

Standard for me is .100", leaves room for operators to make crazy offsets without damaging anything.

 

[DouglasJRizzo]

I was once told by a machinist (while changing the machine parameters and overriding some safety functions to make a part) that 0.005" of clearance might as well be a mile. He always ran rapids to 0.005" clearance and didn't seem to have problems. I did the same on the Mazak and never had issues. But it was also a brand new machine.

How close do you cut it?

Terrifying. Literally.
I've been running NC since the 70s, and that is just the scariest thing to do.
I rapid to within .1" except on castings/forgings and certain tools where it's .25"
All you need is an offset out of whack and *KABOOM* - if you're rapid-ing to within .005.
No thanks.
With .1 or greater, you at least have a chance to react, as I always prove out in single block with the rapid down.

 

[5 axis Fidia guy]

For me, 5x machine. First start point, block center 2" above piece, then all rapids and skims are .025" radially, .070" axially, collision checking .001" shank clearance, .020" holder clearance, .70" machine clearance.

 

[BT Fabrication]

I use 10" and I'm usually chewing on a crayon when I do. Preferably magenta.

I like to taste the rainbow. mmmm

but ususally about .5 to 1 inch depending what i feel like for the day. its not 1000's of parts either. more like 50 at most. part change takes longer.

 

[Larry Dickman]

the default clearance on my cam is .250
I've always just left it there, and it seems reasonable.

 

[angelw]

Both on a Machining Centre and Lathe in Z, to 10mm in Rapid, followed by a very rapid Feed move to 1mm. When running the first part of a new program there is just that bit more control with G01 and a fast feed rate for the final move close to the work-piece. Then in production, the time difference for that last 9mm move between Rapid and the Fast Feed rate is infinitesimal.

Plus the rapid to Z10.0 (mm) doesn't scare the shit out of an operator like a rapid to Z1.0 off a new program.

Regards,

Bill

 

[chad883]

I like to rapid to .1 unless it is a saw cut surface, then .250. I have worked with a few people that like to rapid to Z-1.

 

[Volitan]

Usually .06" on our lathes. The crayon eating mill guys probably 10"

"Crayon eating" lol I'm stealing that one

 

[doug925]

On lathes: X & z are usually 0.1"
Mills = Rapid 0.5-1.0" if jumping vises, Rapid = 2.0" when jumping strap clamps
Clearance for drills = .05 - 0.1"
endmill helix start = 0.02"

 

[Job Shopper TN]

Mills… Solidcam puts out three planes. Start height is 3”, clearance height between chains is .50”, and safety distance to go to and switch from rapid to feed is .050”.

I usually change the clearance to .100” on jobs that are either higher volume or have a lot of holes, chains etc..

Lathes, usually .100” in X (.050 per side) and .050 in Z. On volume jobs I’ll set it down to .020”. Tool retract moves I usually start high and tweak it down at the machine if I have the chance, usually allowing at least 1/2” of clearance for toolchanges.

 

[mhajicek]

.5 to 1.0 mm. But my tools and parts are very small. I found if I cut it closer, I can clip corners coming up out of a pocket as the rapid motion gets smoothed.

 

[Booze Daily]

"Crayon eating" lol I'm stealing that one

I call ‘em “window lickers”.