Using control comp in lead in-outs

[hardmill]

Radius comp is pretty old school, not that many people use it
now that we have cadcam (noy you jay). Back in the day
it was easier to program(manually) the numbers on the
print than to figure out tool centerline. Then offsett 1/2
the tool dia. with your tool comp.

I know this stuff and it makes me feel old.
PEACE

[CAMmando]

One exception to this is Wire EDM where the control is comping wire offset based on power settings. In this application it is still common to program part priofile.

[abcdef]

use this formula
y = (dia of hole - dia of tool) / 2 * .4142

put y in length of line and arc radius ( NOT IN percentage column)...

135 Degrees in Sweep...

that's it and tool comes down right in center...
good luck..

[MnotLyon]

Originally Posted by badRandle When I try to contour a .5 hole with a .25 endmill using control comp. climb milling, the lead in - out goes outside the .5 hole boundary. How do I get the dia. comp to follow the lead in-out?? Confused *&^($@ ThanX Randle

On some controls you can turn cutter comp on, make your first straight line move, then move z into the hole. That won't work on older controls though.

In this case, I would use an entry exit arc of about .22 and 90 deg. Then, I would use an entry line of .22 that is perpendicular to the arc. That will cause you to drop into the hole pretty close to the center, and should give you enough room to turn on your comp for most controls.

[Mike Mattera]

Didn't read the whole thread but..... Sounds like Line, Arc will fix any comp errors your getting.

If your doing a hole, Put a point at the center and Pick the Point, Then pick the Arc (for the Contour). On the Lead In/Out page make sure you select Start from the Point & Finish at the Point. And of course Line & Arc lead on values.

Mike Mattera

[rapid]

i once had problems with this using a drill/chmf/threadmill tool.
our guys were used to using 0 for cdc offset or wear but i had to use full cdc.
i never had the thought at the time and it was a expensive tool so much that we switched to standard drill & tap.
all i needed to do was add a macro to check the limits of the offset and if out of range alarm.
hindsight i guess.

[chuy]

us circle mill toolpath always starts center of hole...if not here's a little formula to make it start center of hole everytime...Hole dia.- tools dia. / that by 2 x that by .4142 insert this # into the entry and arc with an angle of 135 deg works for whatever size hole....

[cadcam]

WOW Chuy tat is old MC9.0 not even V9.1 .

Hey for fun a gigles try this tell it to create virtical lines. now create say 35 just by sketing the what happens?

[cnc-king]

Originally Posted by badRandle When I try to contour a .5 hole with a .25 endmill using control comp. climb milling, the lead in - out goes outside the .5 hole boundary. How do I get the dia. comp to follow the lead in-out?? Confused *&^($@ ThanX Randle

why not use the circle mill routine?

Toolpaths - Next Menu - Circle Toolpaths - Circle Mill and just pick the circle you want to cut, the cutter will start at the center and arc out to the diameter you want to cut or you can set it up to cut a helix going down in the hole

[JROM]

Put a point in the center of the circle
Turn on "use entry point" and "use exit point"
Select the point before the circle.
Enter the blend rad.
Enter the overlap.
Use computer comp not control comp.
Using control comp is giving away control of your tool paths. BAD
Only use cutter comp (control comp) for tight tolerance work.
Works every time.
Also pre drill the point if you can then the plunge is much nicer.
Goodluck

[Uncle Buck]

when using the lead in and lead out command check on gouge check lead in/out...