Once you have created your part in the modeling portion of Fusion 360 or imported a model from a different CAD program. You are ready to start generating your toolpaths for your part. This page will give you an example of how to do that for the Pocket NC using the 12 sided die shown below.
We aren't going to go into too much detail about how to model the part in Fusion 360's CAD model(Autodesk has great resources for that here) but it should be noted that the orientation of your model in space in the CAD module has no effect on how it will be oriented with respect to your machine. All of that is taken care of in the CAM module.
One thing to note about the placement of your model in space in Fusion 360 modeling is that the X, Y, and Z axes referred to in the model(which determine which sides are top, left, front, etc) will not determine the placement of your model on the machine for writing toolpaths. This is especially true for our 5 axis machine because as you rotate the part, it's orientation relative to the machine coordinate systems will change.
Center of rotation
Before moving on to generating toolpaths, we need to stay in the Model module of Fusion 360 to generate some reference geometry in order to machine on the different faces of the die. Every time you machine using all 5 axes of the Pocket NC for 3 + 2 machining, you will need to create a point in space that represents the center of rotation of the machine, or the point where the A axis and the B axis cross.
Keeping in mind that the A axis is parallel to the X axis, and the B axis is parallel to the Y axis. The A axis and B axis cross at a point called the center of rotation. On the Pocket NC, this point lies 0.885 inches or 22.479 mm above the B axis table. This is the point we need to create on our machine relative to our part.
For this example, I will be fixturing the stock material which is approximately 2.5 inches tall by 2 inches in diameter directly to the B axis plate. If the part is positioned at the top of the stock and is 1.429 inches tall, this means the center of rotation will be 0.196 inches from the bottom of the part.
Tool orientation Axes
Once we get to the CAM portion of Fusion 360, we will need to define the tool orientation relative to the part. The options for choosing your tool orientation are Setup WCS orientation, Model orientation, Select Z axis/plane & X axis, Select Z axis/plane and Y axis, Select X & Y axes, or Select coordinate system. We will be demonstrating how to use the Select Z axis & X axis option.
What this means is that for each face you will be machining from, you will need an axis or edge that to represent the Z axis (parallel to the spindle) and the X axis. For side one, the face happens to line up with the model's origin coordinate system so no additional axes need to be created.
Because sides 2-6 are at an angle, to use a 2D facing tool path we will need to create axes that are perpendicular to those sides. In order to do this we will use the Construct Axis Perpendicular to Face at Point option as shown below.
For side 2, first select the face of side 2, and then select any point on that face. This will generate an axis perpendicular to the face as shown below. After that we will do the same for sides 3-6.
Defining Material Setup
Next we need to define the material setup for our part. As seen below, we will be using a cylinder that is 2 in in diameter by about 2.5 inches long. An extra 0.25 in is added to the top of the material stock. It is good practice to account for some extra stock than you will actually be using to avoid plunging into material, just make sure that the dimensions from the table are correct.
Adaptive Clearing Toolpath
The first toolpath we will be generating is a 3D adaptive clearing toolpath from the top of the part to rough out our part.
The first tab of the Adaptive Clearing toolpath sets the tool type and feed & speed. For this part we will use an 1/8th in flat end mill and as the Pocket NC does not have coolant, disable that option. Then set the feeds and speeds for wood. For beginning guidance on feeds and speeds, please see the Feeds and Speeds How To page.
Moving on to the geometry tab, the first step will be to set the Tool Orientation. We will use the method of selecting the Z axis & X axis. Then choose the center of rotation that was created earlier as the origin. In the model selection area, select your entire model.
In the Heights tab, set the bottom face of the part as the Bottom Height (dark blue), the stock top as the Top Height (light blue), 0.2 in from the stock top as the Retract Height (green), and 0.5 in from the retract height as the Clearance Height (red).
The final tab we will modify is the Passes tab as shown below. Be sure that in the Smoothing section it is set to 0.005in or greater, otherwise it can cause the machine to slow down from overload of data.[caption id="" align="alignnone" width="326.0"] Once you have clicked "OK", the toolpath will generate and we can move on to machining the angled faces. [/caption]
2D Facing Toolpath
We will use the 2D facing toolpath to machine at an angle for the 5 top side of the die.[caption id="" align="alignnone" width="491.0"] The tool tab of the facing toolpath will be the same as for the Adaptive Clearing toolpath. In the geometry section, we will first set the tool orientation. Once again, we will use the Z axis & X axis method. For the Z axis, select the axis that you created earlier that is perpendicular to the face you want to machine (in this case the 6 face). For the X Axis, select the top edge of the section you are machining as this lines up with our X axis. For some geometry, this may not be possible and you will have to create a reference axis as we did with the Z axis. For the stock contour, select the contour of the face you wish to machine. [/caption]
The height for the facing are as shown below. The remaining settings will be the same as for the Adaptive Clearing toolpath. Click OK when you are done to see the new facing toolpath.
To finish machining the top of the die, repeat the 2D Face toolpath for the remaining 4 sides.