Fourth Axis Indexing can be accomplished two different ways inside of BobCAM. Choosing the method depends mainly on what type of geometry is used to create the toolpaths. The first method is most commonly used if the toolpath is being generated from sketches, and the second method is commonly used when working with a solid or surface model. However, either of these methods can be used for any type of geometry.
Method 1:
Inside of every milling feature, you have to ability to specify a 4th axis rotation angle to be output in the posted NC program. This can be found on the Posting page of all milling wizards.
When selecting the Output Rotary Angle check box, the Rotation Angle box becomes available. You can now type the Rotation Angle. As a result, the 4th-axis rotation code is output at the beginning of the operation so the 4th axis indexes to that angle before performing the operation.
For example, this method might prove to be the most efficient if you are drilling holes around the circumference of a cylinder. The following example shows the method for drilling 3 equally spaced holes around a cylinder drilled 1 inch deep. You can use a sketch for these types of scenarios because creating a complete solid model of the part may prove to be less efficient. Again, this method can be used when repeating the same operation multiple times at different index locations.
To accomplish this we can start out with a sketch of a circle located on the front plane. In this example the 0.375 inch diameter hole is located at the center of the cylinder, 1 inch from the face of the part.
Next, a line needs to be drawn to specify where the center of rotation occurs. For this example, we are going to drill these holes around a 3 inch diameter cylinder, so a line is drawn 1.5 inches down in the Z-axis.
Now, the entity describing the rotation axis must be assigned to the Machine Setup. To do this, right-click Machine Setup and click Re/Select. Select the Rotation Index Axis Origin check box, and assign the newly created line to the Rotary Index Axis Origin selection box.
Next, to add a drilling operation to the CAM tree, right-click Machine Setup, click Drill, Hole, Next, and Finish to exit the Wizard. By default a Hole feature is created in the CAM tree containing a Center Drill operation, a Drill operation, and an optional Chamfer operation.
Next, you assign the geometry to the Hole feature by right-clicking Geometry in the CAM tree below Feature Drill Hole, and clicking Re/Select. The Selection Manager appears, and by clicking the circle inside of the sketch, the geometry is assigned to the Hole feature. Click OK.
Now edit the feature by right-clicking Feature Drill Hole and clicking Edit. The depth of the hole needs to be entered, and parameters such as pecking can be chosen. Please see the Hole feature for more details on these settings.
In order to have the system perform an index, navigate to the Posting page inside of the Hole feature. On this page, select the Output Rotary Angle check box and type 0 in the Rotation Angle box. This outputs the appropriate rotation code for 0 degrees inside of the posted NC program.
Create 2 more Hole features by repeating the previous steps. This time type a rotation angle of 120 degrees in the second feature, and an angle of 240 degrees in the third feature. A program is now ready to post that will center drill, drill and chamfer 3 holes at 0, 120 and 240 degrees around the piece of material.
METHOD 2:
This method can be used when working with a solid or surface model, a 3D wireframe of the part, or if the rotation angles are not known. By using the Index System item, you can associate a plane or planar face to the Index System item, and the system automatically calculates and assigns the rotation angle from the selected rotation axis to the milling features created below the Index System item.
For the following example part, 3 faces of the model require different operations to be performed. To begin the toolpath generation process, a Coordinate System (to specify the zero location), and an axis (to define the center of rotation) need to be created. Please refer to the SolidWorks Help System for creating Coordinate Systems and Axes if more help is needed.
Once these items have been created, they need to be assigned to the Machine Setup. To do this, right-click Machine Setup and click Re/Select.
The Selection Manager appears and the Coordinate System can be assigned. First, click the Selected Items box, so it turns blue, then select the Coordinate System in the graphics area.
Next, select the Rotary Index Axis Origin check box, and then click the Rotary Index Axis Origin selection box (it turns blue when selected). You can associate an axis, temporary axis, or a sketch line to specify the rotation axis. The axis must also be parallel to the axis of rotation specified in the Stock dialog box. If the axis is not parallel an error message is displayed. If this is encountered, ensure that the entity being used for the axis of rotation is parallel to either the X-axis or the Y-axis, depending on the specific machine configuration. After both items have been assigned, click OK to finalize the selection.
Now that the zero location and the rotation axis are defined, an Index Item needs added to the CAM tree. Right-click Machine Setup and click Add Index.
Next, right-click Index System and click Re/Select.
The Selection Manager appears, and by selecting a planar face of the model, BobCAM automatically calculates the rotation angle for this face.
NOTE: The angles are calculated based off the assumption that the positive Z direction of the assigned Coordinate System is the 0 angle.
Select the face shown next and click OK.
Now that the Index System has been configured, right-click Index System and click Mill 2 Axis, Pocketing. This adds a Pocketing feature to the CAM tree below the Index System.
NOTE: It is important to right-click Index System when adding the milling feature to assure that the angle calculations are included in the machining feature. Adding a milling feature by right-clicking Machine Setup or Milling Tools does not include the rotation angles in the feature.
Next, assign the face of the pocket floor to the Pocketing feature, and modify the parameters as needed. After setting up the Pocketing feature, calculate the toolpath, and the result should look like the following image. Here an Offset Out pattern has been used at one depth of cut. Notice when editing the feature, that the Output Rotary Angle check box is automatically selected and the corresponding angle has been entered.
Now that the machining at this index location is complete, another Index System needs to be added to the CAM tree to tell the system a new rotation needs to occur. If more machining were required at this specific index location, just continue adding milling features to the appropriate Index System. Right-click Machine Setup again and click Add Index to create another Index System in the CAM Tree.
Assign the next planar face, where machining needs to occur, to the newly created index system. Shown next is the face select for the hole drilling that needs to occur.
Again, right-click the new Index System and click Drill, Hole to add a Hole feature to the corresponding Index System.
Assign the two cylindrical faces on the inside of the holes, in the model, to the Hole feature, and the diameter and depth are automatically set inside of the Hole feature. Again, the Posting page can be reviewed, and the Output Rotary Angle is selected and the new rotation angle is assigned. Finish the machining feature by computing the toolpath.
The same steps can be repeated, for the 3rd index that needs to occur, to cut the last pocket in this model. After setup and computing, the finished part should appear as follows.
This concludes the 4th Axis Indexing Tutorial.