cavity mill approaches?

[moog2]

I'm creating a 5 axis cavity mill, on an angle (NX4), i want to change the engage and retract moves, because they end up outside the m/c envelope(due to the angle).
I can change the engage to come from a point, and that works ( couldnt get vector to do anything),
But the retract move , to point won't work.
Any ideas why ??

 

[joycejo]

It may depend where the Work Coordinates are located. I would try placing the WCS at the plane your milling on. The Vectors are relative to the XC, YC, ZC.


John Joyce
Tata Technologies iKS
1675 Larimer St.
Denver, CO

http://www.myigetit.com

 

[moog2]

thanks John, i tried what you suggested but that didn't fix it either, any other ideas,??

 

[wmalan]

Without seeing the operation it's hard to explain. Play with different angles. You might have a Check surface your retract is bumping into? Set your Check and Part Stock Clearance values (not the actual stock values) to 0.000. Set your Engage and Retract options to Skip.

Also, pay attention to the default settings. Generally if your retract would hit a part or check surface it will either retract along the tool axis or just stop (on final pass) at that surface with no warning (at least for me).
Tough to tell without pics...

--
Bill

 

[moog2]

i can't find a skip option..., i've done a sample part,as the one at work would be too large,this shows how the engage and retracts go right across to reach the clearance plane, i just want them to go straight up in the ZM direction

 

[joycejo]

I took a look at the example file. The Engage and Retract look OK to me it is the motion to the clearance plane after the retract that seems to need help. On the Engage and retract set the Transfer Method to clearance plane so the tool moves to the clearance plane between cuts.

John Joyce
Tata Technologies iKS
1675 Larimer St.
Denver, CO

http://www.myigetit.com

 

[wmalan]

Yes. John got it. Use Clearance plane for transfer. By default it used Inherited. I used Automatic for the clearance method and it works fine. One word of caution: Within regions I use previous plane for the clearance value most times. This keeps the tool down. Great for older machines with slow rapids. The thing to watch here is that on most cnc's the tool will "dogleg" move from point to point during the rapid which may hit your part (very common in pockets with islands). A clearance plane above the part is safest.

--
Bill