Modifying CAM Operation Templates
How to Modify CAM Operation Templates
If you ever find yourself constantly changing the same setting within your CAM operation, then modifying the CAM operation template is a quick and easy solution to save clicks and keystrokes. The changes outlined below are my personal preference and may not apply to your programming process.
(Would you rather watch the video tutorial? Skip ahead now.)
You will need the ability to change the write permissions on files within C:/Program Files. I recommend making a copy of the folder in case you would like to revert to the default setting.
- Within File Explorer, navigate to the template_part folder within your NX installation.
C:\Program File\Siemens\NX1953\MACH\resource\template_part
English or Metric
In template_part, there are two folders that contain operation templates: English and Metric folder. The folders contain the operation templates for the corresponding units of measurements. If you typically program in English, you will only need to change the files located in that folder. You will need to change both files if you program in both English and Metric. In this example we will be editing the English operation templates.
- Navigate to the English folder -> Open hole_making.prt.
The files names will look familiar. The names correspond with the name of the operation type within Create Operation.
Setting an Operation Type and Subtype
Like the Operation Type, the Operation Subtype name correspond to the operation saved in the template file.
Feeds & Speeds in Your CAM Operation Template
Note: The following changes may not apply to you. These are examples of what I typically find myself changing.
- Open the existing TAPPING operation.
- By default, the feed rate is set to ipm. Taps are typically programmed in ipr. Rather than continuously changing this setting every time you create a tapping operation, we will change it here in the operation template.
- Feeds & Speeds -> Feed Rates -> Cut -> ipr
- OK to save changes made within the operation. There is no need to generate.
- By default, the feed rate is set to ipm. Taps are typically programmed in ipr. Rather than continuously changing this setting every time you create a tapping operation, we will change it here in the operation template.
Customizing Cutter Compensation Settings
- Open the existing HOLE_MILLING operation.
- By default, Cutter Compensation is set to None. This is true for all operations that have the Cutter Compensation available. When migrating to a new version of NX, I will change Cutcom Location to All Passes to ensure every operation cutter compensation can be applied.
- Tool Axis & CutCom -> Cutter Compensation -> Cutcom Location -> All Passes
- OK -> Save file.
- By default, Cutter Compensation is set to None. This is true for all operations that have the Cutter Compensation available. When migrating to a new version of NX, I will change Cutcom Location to All Passes to ensure every operation cutter compensation can be applied.
- The layout of the operation dialog can also be changed within the operation templates. By default, Cutter Compensation in NX 1953 is missing from the dialog. Let’s add it back in.
- Window File Explorer -> Open mill_planar.prt
- Open the existing PPLANAR_MILL operation. Open Customize Dialog.
- Options -> Other -> Customize Dialog
- Set Dialog Item Type to Customizable Items -> Locate Cutcom Parameters in the list.
- You can also search for Cutcom Parameters
- Highlight Cutcom Parameters -> Add to Dialog -> OK.
- Options -> Other -> Customize Dialog
- The Cutter Compensation was placed at the top of Operation. Let’s move this into its own explorer group,
- Open Customize Dialog again.
- Options -> Other -> Customize Dialog
- Switch the Dialog Item Type to Explorer Node
- Label -> Enter Tool Axis & CutCom as the name -> Add to Dialog
- Highlight Cutcom Parameters. Then, click the down arrow to move it into the Tool Axis & CutCom Explorer Node.
- Open Customize Dialog again.
- Highlight Explorer Node: Tool Axis & CutCom and click the down arrow until you are in the position shown.
- When moving Explorer Node: Tool Axis & CutCom, it will cycle through existing Explorer Nodes and continue moving until you are in the correct position.
- When moving Explorer Node: Tool Axis & CutCom, it will cycle through existing Explorer Nodes and continue moving until you are in the correct position.
And there you have it!
Sign Up for Our Newsletter!
Hi, I’m Collin, and I’m a CAM Engineer at Swoosh Technologies. For over 15 years, I’ve programmed various 3-, 4-, and 5-axis machine tools, as well as multi-channel mill turn machines. My experience in the manufacturing industry has given me insight and knowledge in mold making, high volume production, and process improvements.
Post by Collin Kopecky
Hi, I’m Collin, and I’m a CAM Engineer at Swoosh Technologies. For over 15 years, I’ve programmed various 3-, 4-, and 5-axis machine tools, as well as multi-channel mill turn machines. My experience in the manufacturing industry has given me insight and knowledge in mold making, high volume production, and process improvements.
Nice document Collin,
Another aid I would like to see written up is “Tool Path Report”.
– Firstly, some operations show the cut levels in seperate “level” folders. An example is Adaptive Milling. Others like Variable Contour do not. Is there a way to get them to appear? This would be helpful when merging paths.