Spot drills are more commonly used than center drills when starting holes on milling machines. Like center drills, spot drills are short, rigid tools that tend not to deflect and thus are an excellent choice for a hole-starting tool. However, spot drills are preferred over center drills because if a spot drill with a 90° included angle is chosen, the spot drill will not only start the hole, but will also leave the required chamfer when programmed to the correct depth.
Because most spot drills do not come to a true point but have a small flat or chisel edge, as shown in Figure 1, the flat size must be taken into account when programming the tools depth, which is typically calculated based on a point. Figure 1 provides the length deviation of the tool based on its diameter. If spot drills came to a true point, calculating their drill depth would be easy, due to the fact that the depth would equal the radius of the desired chamfer or the hole radius plus the chamfer radius, since a 45° angle is employed in the depth calculation as shown in Figure 2.
For example, if you are using a 3/8-in spot drill to leave a 0.025 chamfer on a 0.25-in hole, the calculated depth would be 0.150 = 0.250/2 + 0.025. However, due to the flat on the drill, this will leave a chamfer of 0.025 + 0.026/2 = 0.025 + 0.013 = 0.038 in. In order to leave the desired 0.025-in chamfer, the correct programming depth would be 0.150 – 0.026 = 0.124 in.
When a drilling cycle is being used in Mastercam, the Depth Calculator from the Linking Parameters section (see Figure 3) can be used to compensate for the flat size. Simply select the calculator icon, as shown in Figure 4.
In section 1 of Figure 4, you can accept the default setting to use the selected tool diameter and included tip angle or you can uncheck the “Use current tool values” option and enter a custom diameter when you do not wish to create a new tool to match the actual tool used.
In section 2, the desired finish chamfer diameter is entered, as is the diameter of the spot drill at the flat in section 3. In the case of the 3/8-in spot drill, enter 0.026 x 2 = 0.052.
In section 4, you can use this newly calculated value, –0.124, to overwrite the current depth by selecting the “Overwrite depth” radio button, or you can select the “Add to depth” radio button to add this calculated value to the current hole depth.
If the hole and the part’s Z zero are on the top surface of the part, you will want to select the “Overwrite depth” option as shown in Figure 5, regardless of whether the depth calculation is an absolute or incremental value.
If the part’s Z zero is on the top surface of the part and the hole is below the top surface as shown in Figure 6, then you will want to select the “Add to depth” option for an absolute depth value and the “Overwrite depth” option for an incremental depth value.
If the part’s Z zero is at any location other than the top surface of the part, you will want to use the “Overwrite depth” option for an incremental depth value.
Users who take the time to learn the proper use of this calculator will become more proficient at creating the correct chamfer size and their programs will require less tweaking at the machine.
About the Author
Fred Fulkerson is a graduate of the Faculty of Education, University of Western Ontario, and of the general machining program at Conestoga College in Ontario. He is a Canadian Red Seal certified general machinist and CNC programmer and a certified Mastercam and SOLIDWORKS instructor.