The VisualCAD/CAM Part
The part selected for this case study are custom wheel hubs that allow you to mount GSXR 600 brake rotors onto a BMW bike’s front wheel. This then will allow you to upgrade to a Suzuki front end that provides much better performance than the stock front end supplied by BMW. The component is cut from 6061 aluminum and is 5.16” inches in diameter and 1.63” inches wide.
The part contains an interesting set of features including profiles, pockets, flanges, and holes as well as machining from two sides. The center thru-hole requires some tight machining tolerances. KC can CAM program all of these features to the required specifications using his VisualCAD/CAM software. We invite you to continue reading to learn more about this component and how it was programmed and posted to KC’s CNCMaster 3 Axis mill!
The bottom side of the component contains a flange with 4 mounting holes, a larger pocket, and a thru-hole. The 3D solid model is shown here oriented bottom side up.
The VisualCAD/CAM Setups
Setup 1 (Top Side)
Setup 1 (Bottom Side)
Machining the Top Side
2-Sided Machining Videos
If you are unsure if your parts require 2-sided machining, we invite you to watch a few of our videos on this subject. They are listed below. Enjoy!
CAMJam Short #253: Do I Need 2-Sided Flip Machining?
CAMJam Short #249: 2-Sided Flip Machining in PRO vs STD
CAMJam Short #250: Basic 2 Axis Bridge-n-Flip Method
CAMJam Short #251: Basic 3 Axis Box-n-Flip Method
CAMJam Short #252: Advanced 3 Axis Flip-n-Jig Method
Drilling Operations
As shown in the Machining Job above the first 3 folders are Drilling operations. The first two are roughing operations. The first of these is a Center Drill of 0.125” dia. The depth of the cut is 0.01”. The second is a Deep Drill operation using a #7 (0.201” diameter) drill cutting 0.35” deep with 0.1” peck increments.
The third is the finishing operation using a 0.3125” drill cutting 0.30 deep with 0.05” peck increments. Note that you do not need to use three drilling operations. We use them here to illustrate the use of pre-drilling operations. In the illustrations below we see the finishing 0.3125” dia. toolpath on the left and the cut material simulation illustrated on the right.
In the illustrations above we see the finishing 0.3125” dia. toolpath on the part geometry model on the left. On the right side illustration, we see the cut material simulation model produced by VisualCAD/CAM.
2½ Axis Facing
The location of cut geometry is set to At Bottom, the total cut depth, rough depth, finish depth, rough depth per cut, and finish depth per cut are all set to 0 (zero). This means that there will be just one cut level with the bottom of the cut residing on the top of the part lip. The 2½ Axis Facing toolpath is illustrated on the left (below) and the cut material simulation model is illustrated on the right.
3 Axis Horizontal Roughing
The next operation in the Machining Job is 3 Axis Horizontal Roughing. It is used as a roughing operation to remove excess stock material. In this method, VisualCAD/CAM automatically calculates what material needs to be removed based on a 0.500” diameter end mill, the part, and the stock geometry. The cut parameters used include 0.01” tolerance, 0.025” stock allowance, an offset cut pattern, mixed cut direction, a 25% stepover.
Each cut level depth is set to remove 50% of the tool diameter (which is 0.25” inches), depth-first ordering, and a bottom limit of 1.024”. The cut engagement is set to helical motions. Arc Fitting is also enabled (blue-colored motions). The resulting toolpath is illustrated on the part geometry model on the left (below). The cut material simulation is illustrated on the right.
2½ Axis Pocketing
The first upper 2½ Axis Pocketing operation is shown above with the toolpath illustrated on the left and the cut material simulation illustrated on the right.
2½ Axis Profiling
Note:
You may be asking yourself:
“How can I make my toolpaths simulate in different colors?”
Here are the steps to make this happen:
- After defining the toolpath operation, right-click on the folder from the Machining Job and select Properties. Use the dialog to set the simulation color. Do this for each toolpath operation in the Machining Job tree.
2. Then select the Simulate tab and look at the toolbar at the bottom. Where it says “Default” drop the menu down and select “MOp”. This stands for Machining Operation.
3 .Now simulate your machining Job to see the colors applied.
The cut parameters for the second Profiling operation include a total cut depth of 0.4” with 0.1” stepdown increments resulting in 4 cut levels. Refer to the illustrations above.
2½ Axis Pocketing & Profiling
The last methods in the Machining Job will cut the pattern of thru-pockets located within the upper lip and around the flange. The first is a 2½ Axis Pocketing operation for roughing and the second is a 2½ Axis Profiling operation for finishing. Note that these pockets can be cut with just the Pocketing operation. However, we wanted to illustrate the combination of Pocketing and Profiling for roughing and finishing a pocket.
The 2½ Axis Pocketing operation rough cuts all 20 pockets. Cut parameters include 0.001” tolerance, 0.01” stock allowance (to be removed during the Profiling operation), offset cut pattern, climb cut direction, 25% stepover, and a cut depth of 0.4” divided into 4 cut levels. Pocketing entry is set to ramp and exit is set to linear. You can see the toolpath and the cut material simulation in the illustrations below.
As we mentioned above, the 2½ Axis Profiling operation finish cuts all 20 pockets. Cut parameters include 0.001” tolerance, 0” stock allowance, mixed cut direction, and a cutting depth of 0.4” divided into 4 cut levels. Arc fitting is enabled with a fitting tolerance of 0.002” (dark blue motions). The operation includes a ramp entry and a straight retract exit motion. You can see the toolpath and the cut material simulation in the illustrations below.
The 2½ Axis Profiling operation finish cuts all 20 thru-pockets. The toolpath is shown on the left and the cut material simulation is on the right
This completes the top side for this part. The Setup1 as shown in the Machining Job tree above can be posted out in one g-code file (if you have an automatic tool changer) or posted out as separate g-code files, one operation at a time if you need to change tools manually for each operation.
The Top Side Completed In-Process Stock Model
Machining the Bottom Side
The Bottom Side Setup
3 Axis Horizontal Roughing
2½ Axis profiling
Deep Drilling
2½ Axis Hole Profiling (the Flange Holes)
The last three methods in the Machining Job are 2½ Axis Hole Profiling operations. In Hole profiling, the tool profile cuts each hole in a helical motion until it reaches the full depth of the cut. You can control the helical pitch which is the vertical distance between each full 360-degree helical motion. When the bottom of the hole is reached, a full circular motion is performed (dark blue), cleaning up the entire hole diameter. The toolpath and simulation are illustrated below.
2½ Axis Hole Profiling (rough and finish the center hole)
The accuracy of the thru-hole at the center of the part is critical in this case. We are using a combination of two 2½ Axis Hole Profiling operations to achieve this. The previous 3 Axis Horizontal Roughing operation left 0.015” of stock material around this 1.00” diameter hole. The first Hole Profiling operation cuts to a diameter of 0.950”.
The second Hole profiling operation will cut the hole to its full diameter. Two operations are used to minimize tool deflection during the final pass. Alternatively, you could use one profiling operation with two XY stepovers. However, using a second operation allows us to use a tool for the final cut! The hole depth is 0.75” and the helical pitch is set to a vertical depth of 0.06”. At the bottom of the hole, a full circular arc motion is added for increased accuracy. The tolerance is set to 0.0005” for the final operation.
Note that this hole can also be machined using a Boring operation. However, since not everyone will have a boring bar tool, you can meet and exceed the same level of accuracy using 2½ Axis Hole profiling with a few tolerance adjustments. Refer to the note box below.
When close fits, in this case between a rod and a hole, are required, there are several parameter adjustments you can make in VisualCAD/CAM to achieve the exact level of accuracy required. You can refer to the following two resources:
- How to Increase Tool Path Accuracy (Blog Post)
- A case study for a real-world example
- Note: These adjustments are the same for all MecSoft CAM plug-ins.
The PRO Configuration
In PRO, Setup 2 is oriented and not part geometry. In our case, the X axis of Setup 2 is rotated 180 degrees so that the +Z axis of Setup 2 is facing the bottom side. This is all that needs to be done. The remaining toolpaths are programmed similarly to setup 1. In PRO, you can also simulate both setups at the same time, revealing the in-process stock model after each setup. The resulting simulations of both setups in the PRO configuration are shown below.
We hope you enjoyed reading about this fantastic project! We want to extend a very special thanks to KC Gager, Owner/Operator, and his team at BRG Racing for allowing us to write about their cool work with VisualCAD/CAM!