Undercut Machining in 3 axis Milling.

[Ritesh]

Hello Team!

I am trying to cut an undercut area in 3 axis Milling. Not getting any good results. Can anybody guide me with this.

I have attached the part file.

Cutter: T slot: Shank:16mm, Dia:65mm, Upper Radius: 5mm, Lower Radius: 5mm, FL: 10mm.

[jkane1]

It seems you had not attached the part file. Please try again to upload it again.

I am assuming that you want to undercut those bent parts with the right-angle. If they are straight across you could cut them with Planar Profile.

Two things are needed. Specify the Part Boundary as the edge of the vertical wall and specify the Plane as the undercut horizontal face. Next, set the Drive Point in the Planar Profile operation to SYS_OD_Top.

[Ritesh]

Hi,

Thanks for the reply.

I have uploaded the part file.

This undercut is not a straight .

It is a 3D profile.

Please go through the part file.

Regards,

Ritesh

[Mak_Jo]

Please look at the 'PROFILE_3D' operation in the attached part file.

Note that I have just shown the way to crete the toolpath and not set/looked at any other parameter to be used on machine. Hope this helps you.

[ahmetunkur44]

Hi @Ritesh,

I have prepared Planar_Mill operations with T-Cutter. You can check it out operation details on the part which I attached and I explained at the below. (with a T-Cutter tool, Planar_Profile operation is a good alternative with Drive Point options (whether you select Top or Bottom of T-Cutter) )

So, these Planar_Mill operations: one related to Z-axis, another one related to vector direction. I think; the operation according to vector direction is more suitable in this bend area.

Before I start the operation, I used Offset Curve in Face command to offset the edge of the bend 5mm down on the face. In the operation; with Stock option (Specify Part Boundry -> Custom Boundry Data: Stock) you can take the toolpath toward the part. Write here negative stock to cut more from part (that means you will take the toolpath into part!) or write positive stock to leave stock like 0.5 mm for finish operation.Cut Pattern is Profile.Select Conventional Cut to start cutting from the open side of the bend.

And one more thing that in this bend area, it's better to use a bigger T-Cutter tool(like D70 mm). Bcz, in the last toolpath there is only 0.5 mm between wall and Neck Diameter of the T-Cutter. (just to keep in mind)

Have a nice day.

Ahmet ÜNKÜR - NX12.0.1

[Michael_Adam]

@Ritesh 

I attached a vidieo where I use the Fixed contour operation for undercutting.

This works  also for a 3-AXIS machine.

As you can see the tool axis stays the same as the Z vector.

I hope this is the solution you were looking for.

[ahmetunkur44]

Hi @Michael_Adam ,

It looks great. Thank you for your effort. Have a nice day!  

Ahmet ÜNKÜR