cutter comp. with resharpened endmills???

[Oppiz]

After reading posts and from personal experience, I like most of you feel its better to let MC handle cutter comp., not the control. This may be a redundant question but I'm going to ask it anyway. What is the best way to handle cutter comp. when you have a superviser that is determined to used odd ball resharpened endmills?

[Guest CNC Apps Guy 1]

If using Version 9 - Wear Comp is best(kind of the best of both worlds

 

If using Version 8 and below, use Comp in Computer AND Comp In Control. This is the equivalent of wear compensation.

 

Program to a normal sized tool, then adjust up or down in your offset page in the control. Using wear compensation gives you the ability to switch out cutters without having to re-post another program. Just change the diameter/radius value in the control and you're good to go.

 

JM2C

[Keith Graydon]

I gotta agree with James on this. Remember this, tho:

The part is CUT on the machine , not on the computer.

 

KLG

[md]

Remember to leadin to turn comp on

and leadout to turn comp off.

Leadin should be at least the amount

you think your tool is small.

1" mill is .950 leadin .05 min.

[md]

One more thing your comp will be

-.025 for Rad. comp or -.05 for Dia. comp

[Oppiz]

I'm going to give wear offset a try. I'm not sure if one of our old mills allows for negative cutter comp. at the control.

[JAMMAN]

Oppiz- control comp is evil. Not really, but I find the results much more predictable and if your network to your machine is decent you can have the cutter size changed, re posted and out there before your operator can find the wrench to loosen the tool and change it. Way faster than going into most tool registrys and changing diameter. Take note this is the first time in forum history I have dis-agreed with James!

[md]

JAMMAN:

 

As you cut your endmill wears changing Dia. right?

The same 1/2 endmill in a diffrent hard holder

cuts a diffrent size thats called cutter runout.

So you spend alot of time reposting and with

your operaters because parts are not to size.

If you think about what your doing cutter comp will work just fine.There was a time without Mastercam and we used the part Dim. right along with G91 Incremental programing.

[JAMMAN]

quote:

---

faster than going into most tool registrys and changing diameter

---

(quoting myself)

 

I have done it both ways. If you have a 486 and carry the program to the machine on a 3.5 floppy, then I can see it. Otherwise..............

[RAJ]

cutter comp works great on control as long as u dont have a FADAL!!!

[Kenneth Potter]

quote:

---

cutter comp works great on control as long as u dont have a FADAL!!!

---

You said it Dude!

[Oppiz]

I've been using cutter comp at the control for 10 yrs. for two reasons: resharpened endmills( I'm not always there to repost) and I work in a close tolerances. MC can't take into account things like tool deflection. My number one problem with comp at the control is when I use converted autocad files our designers sometimes round off the corner radii. If I don't detect this before its gets on the floor, the machine will get a tool nose radius error.