Lead In/Out problems

[TK-32™]

Hi guy's I'm having problems using Lead In/Out. I'm trying to cut a .312 dia bore with a 5/32 E.M. It's roughed with a .302 drill. my proble is:

When I add Lead In/Out of 0.077875 (so that it plunges right at center of bore) it adds the line. I can see in Backplot. Now when I add an arc of the same rad the whole Lead in/out like is gone.

I hope I was able to explain my problem, Thanks in advance.

[Guest]

Try circle mill instead using the start at center and perpendicular options checked

[90rsgnuguy42]

.0323 line, .0323 arc lead in and out, 135° lead in and out

[TK-32™]

I just tried Circle mill and it's great. I come from MasterCam 7 and this is new to me. Thanks JParis.

Colin, in 7 i used to set the same lenght for the line and rad. I'll try your way and will let you know.

[TK-32™]

[crazy^millman]

Put 0 in for the Radius angle, use an overlap of .05, and it will do better.

 

HTH

[TK-32™]

I used Overlap and kinda did what i was trying to get in the first place.

 

Thanks for your patience

[crazy^millman]

Did you know you can ramp that hole with contour Ramp and you can also do that with Helix Circle Mill toolpath as well?

 

HTH

[shazam/TPP]

gcode set your compensation type to control not computer and your lead in/ lead out will be correct. you may need to change radius to a smaller amout as well.

[Robert Ouellette]

or you could put a point in the center of the hole and pick point then circle and in leadin/lead out page use start from point and 0 line and rad and never gouge a hole again and no math to do. i love it that way for the same stuff.

[billystein]

+1 bob

 

that's how i do it always. I just use a radius of .01 or .02 and 0 for line length and use start point.

[Programinator]

circle mill works good and you dont have to even drill the hole. It will ramp in and rough the hole and then finish it starting on center.

 

Works great for me

[Justin Beebe at Folsom Tool]

I do like Bob and billystein. By selecting a point in the center then chaining the arc with use entry point selected, mastercam will automatically calculate the line length if have a value of 0 for line in your lead in/out parameters.

[Thee Dragracer1951]

Yea, I been starting to use the point in the center to define the entry point as well. Sometimes (I was doing a .357 dia yesterday with a .187 EM. enter on point, helical in at 5% and 20% dia. it wouldn't do it untill I chnaced the XY clearance to less than the default .1

I thought that was strange...

[neurosis]

quote:

---

Did you know you can ramp that hole with contour Ramp and you can also do that with Helix Circle Mill toolpath as well?

---

Very cool. I like this for ramping holes.

[WeGrok69]

If you subtrct the endmill dia from the finish hole size then divide by two(the finish tool path radius)multiply that by the tangent of 22.5 deg(.4142)and use that answer for both the line and the arc and use tangent and 135 deg sweep.

That will put you in the center. .312-.1562=.1558

.1558/2=.0779 .0779X.4142=.0323 as 90rsgnuguy said

[90rsgnuguy42]

I found that formula on this forum and interpolate all the holes I make like that. I love it. Adding points and circle milling and all that other monkey motion is just too much work.

[gcode]

quote:

---

Adding points and circle milling

---

circle milling can use either a point or a circle.

If you use a point, you have to tell it how big the circle is.

If you use a circle, that's what you get