Need Help!- Chamfering holes

[English]

Hi, We have a Mazak A16 with X,Z and C axis (full). The machine is equiped with a T+ control.

So drilling and tapping bolt circle holes is no problem BUT has anyone managed to chamfer the holes prior to tapping? I know that I could do this with my CAM software but I wanted to see if it could be done either with Mazatrol or by using a macro. Anyone done this?

[Philabuster]

Chamfering as in plunge in and out? That can be done in a drill cycle or boring cycle--just have to feed to a much shallower depth than with drilling. This will be on its own process. Just copy the drill cycle and make the depth shallower using a different tool.

If you mean interpolating the chamfer around the holes, that takes a lot more programming, but it can be done.

[Kaszub]

ISO G-code for Mazatrol + Plus if you have that option.
It is in your manual if you have one.

G72.1 X...Y...Z...R...P...Q...

X,Y,Z,P,R same as any other drilling cycle

P=overlap amount
Q=radius of hole to chamfer minus radius of cutting edge of your tool

[philipev]

I am not familiar with Mazak but what I do is program the center drill deep enough to leave a chamfer. It's not a 45 chamfer but it does break the corner and gives a good start for the tap. For example on a 3/8 hole use a 7/16 or 1/2 center drill and program it to .400" deep. It generates @ .400" diameter chamfer a little bigger than the 3/8 threads.

[JCVineyard]

if you are using Mazatrol. When you write the unit for tapping. it should ask you how much of a chamfer you want around the hole. then it is just discribing the tool properly for the machine. for larger holes. there is a unit for "chamfer in" . then you just tell it the canter position of the hole, and the Radious of the hole.

[English]

Unfortunately I do mean interpolating around!

[rusty1979]

i run a 410a and variaxis i just use circular mill unit to do my chamfers instead of chamfer in cos it can interfere with the hole size for some reason !
i just descride a standard 10mm carbire 90deg spot in machine as 10m but put a diameter of 2mm in the tool table and program 2mm deep to what ever rad u want around hole then adjust z depth to suit size of chamfer/break edge !