Sequential Milling 2

[kyleb77]

When ever I transform a sequential operation the tool path direction reverses itself. Instead of picking the path in reverse before transforming, is there an easier and faster way that I can reverse the direction?? Normally on most other operations ( ex. Planar ) all you would have to do is choose Convention or Climb and it would reverse but in Sequential Milling there is no option.

 

[wmalan]

Sequential mill has a bit more going on than planer mill I'd suspect.

Are you doing airframe type work?
I havn't found an easier way than using lefthand tools for the opposite hand parts (for airframe work) if possible. Don't know if that helps but for much of my work we'd just mirror at the control and change to lefthand cutters. It also ensures that changes to one side of the plane are incorporated to the opposite side.

Btw, if you use anything other than Automatic engages/retracts in Planner mill, those will flip as well. A 20 deg engage/retract will flip to a -20 and go through the wall.


--
Bill

 

[kyleb77]

Thanks for the post. I also have used left hand tools as well but the company wants to stray away from left hand tools. So basically we have to repick everything in reverse and then mirror the operation. Once mirrored the toolpath is normal again. I hope newer releases of NX will try to fix this.

 

[Candas]

I recommend not to transform sequential milling operations but always create them again. By the way for most of the cases I recommend variable contour instead of sequential milling.

 

[derekkarp]

I don't know if this will help, but sometimes instead of transforming a tool path with the mirror option, we will rotate it 180 degrees and it keeps the direction going the right way. But like stated earlier, sequential mill is picky and sometimes a simple change will make the operation fail.
-Derek

 

[Dawson70]

I also recommend variable contour and boundaries for planar cuts. They mirror just fine with only a few changes needed. You'll have to change the engage direction if using other than relative to cut, and extend the last bounding curve instead of the first to allow for cutter comp. You'll also have to switch climb to conventional. All this takes a matter of seconds on most parts.

The other plus is that you can copy/paste the path and change it to surface area, area mill, etc without having to reset your from point or assign tools, part stock, and geometry group.

I always make opposite programs now since there will always be a lazy operator who'll run a right handed tool and conventional cut. This leads to undercut walls, and many other undesireable effects.