CADabout.ru starts a new series of arcticles dedicated to the 3 axis milling functionality in Siemens NX CAM module.
In this lesson you will learn about:
- How to launch CAM module in NX;
- The algorithm of CNC-program development;
- The inheritance of parameters in Operation Navigator;
- How to start a new project and adjust it;
- Create your first CAM project and verify it;
1. How to launch NX CAM.
At first you should download an example STEP-file (you’re also can get more information about STEP file format here), which contains training objects. I chose this type of file, because it is easy to import and lightweight, besides it provides good compatibility with all NX releases. It is compressed in .zip archive. Download the file (67 Kb)-download the model.
I used Siemens NX 184.108.40.206 and Siemens NX 10 while preparing this article.
Unpack example from the archive. Import the STEP file into NX: click File —> Open, in the type field select .stp files and choose pressForm_cavity.stp.
Then click File —> Applications —> Manufacturing.
The Manufacturing Environment menu will appear, click Ok to use default settings, but before make sure cam_general Session Configuration and mill_planar or mill_contour CAM Setup are selected.
Manufacturing projects in NX have the same filename extension, as the part files – .prt. User interface in NX is designed based on the Roles. User defines the role that fits his needs at most. It is also possible to create a custom role or select a role from the list of all available roles.
I recommend you to use the Advanced role.
Let’s look more closely into NX CAM user interface. On the whole, it could be splitted in a few local groups. The main window header shows a name of the current module and a name of opened part.
Main menu, which was significantly changed in NX 9 looks as following:
It is splitted up into a few tabs, each of them contains specific features. Frequently use features are located at the Home tab, this will be true in most NX modules.
The picture shows the most used operations, which are: Create Tool, Create Geometry, Create Operation, Create Program and Create Method. The default CAM-workflow looks as it shown on the next picture:
These steps are only a recommended parts of the manufacturing workflow. Siemens NX fully supports the master model concept, so a CAM project should be separated from the design part being wrapped in the parent assembly. Normally, CNC-programmers are tend to operate with WAVE-link of the master model geometry. It makes CAM-geometry isolated from design part, but leaves the descendant inheritance form master to linked copy. We will see this mechanism in the next lesson.
All CAM objects can be grouped in the following sections:
Programs are the objects used to define an operations sequence.
Geometry objects are those, which define the part and stock geometry, clearance options, MCS (machine coordinate system) and others.
Methods are defining the machining strategy, include cutting parameters and tolerances.
Operation Navigator is also contains tools and operatons. You are able to switch between views by select the needed group:
Pay attention to the inheritance between CAM objects. For the instance, operations inherit the tolerances and cutting strategies from parent methods (if defined). Operations are linked to tools, while tools linked to operations. Part geometry and stock geometry are succeed to MCS, while operations could be succeed to both workpiece and MCS.
Come back to our project. Click on the Create Tool button at the Home tab. Under the type list select mill_planar. Define End Mill as a tool subtype (see the picture). Type a name of the tool, as it shown below. Click Ok.
As it follows from the tool name, we will create a milling tool with the diameter of 8 mm and the lower radius of 0.5 mm. In the next window insert the diameter, the lower radius, the tool length and the flute length. The tool geometry preview will be shown in the NX graphic window.
Also, under the Numbers group define the Tool Number, the Adjust Register and the Cutcom Register. Click Ok.
Go to Geometry View and double click on the MCS object.
Under the Clearance Option select Plane and define it, selecting the most upper part surface. This plane will be used to create non-cuting moves of the tool path.
Double click on the Workpiece object in the Navigator.
Workpiece uses to determine Part Geometry, Blank Geometry and Check Geometry. All operations should be linked to the workpiece, inasmuch as they are inherit those geometries. Click on the Specify Part button and select the solid body in the Graphic Window. Then click on the Specify Blank button and insert the following parameters:
The final step – create the operation.
Click on the Create Operation button on the ribbon menu:
Under the Type list select mill_contour, Operation Subtype is Cavity Mill.
Append this operation to the PROGRAM, assign MILL_D8_R.5 milling tool, link it to the Workpiece and select MILL_ROUGH method. Click Ok. In the very bottom of the next window, under the Actions list click on the Generate button.
The tool path for the operation will be generated:
Now click on the Verify button.
In the new window switch to the 3D Dynamic tab, reduce the Animation Speed to 5-7, and click Play.
You will be able to see the tool path verification for the current operation in the NX Graphic Window.
The end of Part 1.
If you have found this article helpful, in case you consider it useful for your work – make a 1$ donation. It will help us to make more quality articles.