Two weeks ago, I had the privilege of attending a Cam Forum for Siemens PLM Software partners. A colleague and I drove down to Troy, Michigan, where we were introduced to new NX CAM functionality in NX11.0.1. We also saw some of the future enhancements coming in NX11.0.2 and beyond. Although there were many enhancements that I could discuss, there was one in particular that I found extremely useful. So rather than give a brief overview of all the enhancements, I will focus on one of my favorite enhancements. Once you’ve loaded NX11.0.1, open the help docs and view the what’s new section, if you’d like an overview of all the enhancements.
Interpolate Tool Axis Enhancements
Prior to NX11.0.1, if machining the part below, with the tool shown, you’d have a tool holder collision issue along the wall.
When situations like this occur, NX now provides a new Control Direction option, when using the Interpolate Vector tool axis option. To access this new option, expand the Tool Axis section, in the operation template. With the Axis option set to Interpolate Vector, click the Edit icon.
Notice the new Control Direction option under the Interpolation Method.
The U and V option retains the behavior from previous releases. The U option controls the tool axis in the U direction only. The V option controls the tool axis in the V direction only. These two options give the new behavior.
In this example, I’ll select the U from the Control Direction list.
Notice the two iso curves. Each iso curve contains a system defined vector at each end. Only one vector is now necessary to define the tool axis along each iso curve.
There is another new option, that allows us to select a system defined vector and tell the system not to consider it, when interpolating the tool axis. You do this by selecting the vector, and selecting the new Ignore Point check box. In this example, I first select vector 4, from the list.
Note: You may also select the vector by single-clicking in the graphics display. Double-clicking reverses the vector direction.
I then select the Ignore Point check box.
I repeat this step for vector 2.
Next, I select vector 3 and use the dynamic axis handle to rotate the tool about the YC axis, until the holder no longer collides with the part.
The third enhancement becomes apparent will doing this rotation. In previous releases, the tool was rotated about the tool tip resulting in the tool cutting below the part surface. The tool now rotates about the contact point and no longer violates the part. See the image below.
When I verify the tool path, I notice that the tool holder no longer collides with the part wall, but the tool axis begins tilting sooner than necessary. This is because NX tilts the tool axis continuously as it interpolates the tool axis between the two U curves.
I can add another iso curve to control how long the tool remains vertical before tilting. To do this I return to the Tool Axis section and click Edit again. In the Interpolate Vector dialog, I select the Add New Set icon.
Next, I select a point on the edge of the part, in the approximate position shown below.
This defines an additional iso curve with a vector that can be used to control the tilt of the tool. By leaving the ZC vector vertical, the tool axis will remain vertical as it approaches the wall until it reaches this curve.
This time, when I verify the tool path, the tool axis remains vertical until it reaches the added iso curve. It then begins to tilt as it approaches the next iso curve.
As you can see from this example, you can now specify either a U or V control direction and ignore system defined vectors, allowing you to interpolate the tool axis for variable axis operations along U or V iso curves, with as little as a single interpolation vector for each curve. This capability greatly simplifies the task of specifying a constant tool axis orientation along the entire U or V curve.