Basic NX Face Milling Question

[BarriCA]

Hello Folks,

Im struggling with what Im sure is a very simple problem for you guys. 

I am trying to machine a rim face of a large cylinderical component, as shown below. 

Basically whatever I do I cant get the tool to machine the path in a single pass. 

The tool is 125mm dia, and the width of the rim is only 20mm or so, so easy enough to machine. I'm just pulling my hair out trying to get a single toolpath to travel around the rim using around 60% of the cutter dia.

Im still relativley new to NX and am learning lots, but any help on this issue would be most appreicated. 

Many thanks

[psch_wny]

Facemilling almost always creates a min. of 2 passes. I have gotton 1 a few times, but it is rare

You can mess with the tool overhang parameter. to keep it tighter on the part.

But for a round profile like this I would always use planner mill, probably pick the outside profile and use negative stock to get the tool over the part. Arc on and off engage/disengage

[Keith_Humphries]

Hi,

You can use a planar mill operation.

Specify the part boundary and select curve/edges

Select the inner edge of you cyclinder and make sure you select on instead of tanto from the tool position drop down box.

Then select the face as the floor and arc on and off as already suggested and this should work in one pass.

[psch_wny]

You can make the part boundry "on" when picking the curve, but then you are stuck with the tool right "on" the curve.

If you keep set to "Tanto" and then do negative stock (Say -.25) in cutting parameters the edge of the tool will go over the line by just .25 instead of driving only on the centerline.

Tanto has a little more flexibility in where you want the tool to be.

When you want a specific tool path nothing beats planner mill.

[GerritKoelewijn]

You can try to use Floor Wall for this.

Face milling is less smart in this case.

Attached a Part where it runs only in one pass.

The following parameters influence the behavior:

• Cut Pattern : Follow Part
• Cutting Parameters=>Connections=>Across Voids=>Motion Type : Follow
• Cutting Parameters=>Containment=>Cut Regions=>Tool Overhang

I attached the Sample for NX11

[GerritKoelewijn]

I Verified that this behavior goes back to NX9.

In NX8.5 this behavior is not there yet and you end up with 2 passes.

Looking at the Picture of the Thread Starter, it looks like he is using NX8.5.

So be patient untill NX9

[GerritKoelewijn]

In NX8.5 it is also possible to get the same behavior.

The only difference is that the Cut Pattern must be "Follow Periphery".

Before NX8.5 you are stuck with Face Mill or the other options mentioned above.

Attached the NX8.5 part here.

[59holloman]

Hello BarriCA

Just change the Cut Pattern under Path Settings, set at Follow Periphery to Profile.

Make sure additional passes integer =0

[drafter006]

Other parameters

Tool Diameter = 120 mm

Maximum Distance = 120 mm

Tool Overhang = 50 mm

thats all. Just let you draw your path.Simple process.