Skip Navigation LinksNX-CAM-Milling-Tips-Part-1


NX CAM Milling Tips Part1:  Tool Path Optimization 

Click here to see a video for this article.

In this NX A to Z article I am going to cover a few features in NX CAM that you may not be aware of that may help you program faster and better. 

Optimize Feed Rate

When you use this feature, NX analyzes the tool motion for your operation relative to the the 3D In-Process Workpiece (IPW) and adjusts the feed rate to maintain uniform tool load. This will extend the life of your tool and remove material more efficiently.

There are a number of options for using this feature.

  • You can configure NX to optimize feed rates for all operations every time they are generated using the Customer Defaults. The path to the default is Manufacturing » Operation » Optimize Feed Rate tab.
  • You can tell NX that you want it to optimize the feed rate for a specific operation every time the operation is generated using the Feeds and Speeds Rates dialog from within the operation. This is shown below.

  • You can also select operations or groups of operations from the Operation Navigator and optimize their feed rates as shown below.

The Feed Rate Optimize dialog box is shown below. Basically, it allows you to set the limits for the feed rate adjustment as well as the Stepover and Depth of Cut that are to be used to calculate the nominal material removal rate (these are initially taken from the values in the operation and can be adjusted here). The Length Interval is the minimum length of tool path between feed rate changes.

You can add the Optimize Feed column to the Operation Navigator so you can see which operations have optimized feed rates. To add columns to the Operation Navigator, just right-click any of the column headers, select the Columns item and then select which columns you want to add.

The image below shows a snippet from the NX documentation with an optimized feed rate on the right a non-optimized feed rate on the right. Needless to say, there is more information in the help files about this feature including an explanation of how the optimized feed rates are determined.

Report Shortest Tool

The Report Shortest Tool feature will determine the minimum length that the tool specified for your operation must project from the holder that you have specified for your operation. A holder must be defined for the tool that you are using in order for this feature to work. By making sure that your tool doesn’t project from the holder any farther than necessary, you ensure that your tool is as rigid as possible which extends the life of the tool and also provides for improved accuracy and surface finish on your part. In order to use the feature, just right-click and operation in the Operation Navigator and select Tool Path » Report Shortest Tool as shown below.

You can also add a Shortest Tool column to the Operation Navigator and after you have determined the shortest tool for a given operation as shown above, the value will be displayed in the Shortest Tool column so you can refer back to it at any time.

Optimized Cut Levels

The next two features that I am going to detail allow you to finish both inclined and horizontal surfaces using Z level profile and a scallop based stepover. If you use a Z level profile operation, you can select a Scallop height for the Common Depth per Cut as shown below; however, the depth of cut is still constant. NX determines the depth of cut along a plane at a 45 degree angle to the tool axis as shown in the image below from the documentation.

Obviously, this will only give the specified scallop height on walls that are at a 45 degree angle to the tool axis. Anything at an angle less than 45 degrees will have a smaller scallop – which is probably fine, but anything at an angle greater than 45 degrees will have a larger scallop – which is a problem. When Optimized cut levels are used, NX will adjust each cut level to maintain the maximum scallop height that is specified. The image below on the left uses a 0.010” scallop with constant cut levels and the image on the right uses a 0.010” scallop with optimized cut levels and as you can see, with optimized cut levels, the cut level changes as the incline on the part faces changes so that the scallop height is maintained.

The use optimized cut levels, just select Optimized for the Cut Levels option in the Cut Levels dialog as shown below.

Cut Between Levels

With optimized cut levels, we can maintain a constant scallop height on the inclined faces of the part even as the angle of the incline changes, but what about the horizontal faces of the part. If you want to machine both the inclined faces and the horizontal faces with a single operation, you have to use Cut Between Levels. Cut Between Levels provides the option of specifying an independent stepover for the horizontal faces, so if you’re using an end mill with radiuses, you can just say you want the horizontal stepover to be 70% of the tool flat for example and this will eliminate the scallop on the horizontal faces. The image on the left is the same one shown previously with the Optimized cut levels and the image on the right uses Cut Between Levels with the horizontal stepover set to 70% of the tool flat and as you can see, the horizontal faces are now finished along with the inclined faces.

Cut Between Levels is on the Connections tab in the Cutting Parameters dialog as shown below. The Feed on Short Moves option will prevent the tool from retracting and re-engaging on short traverse moves. The Max Traverse Distance allows you to specify the maximum traverse move that will be changed to a feed move.

That’s it for the first round of NX CAM Milling tips. Have fun.

Dave Holland