Mastercam Tutorial—How to Spot Drill for Multiple Hole Diameters in One Toolpath

Mastercam users can save machining time by spot facing for multiple size holes and on different surfaces in the same cycle.

Hole making is one of the most common machining tasks and when programmed poorly, a significant amount of a shop’s profit can be lost. Figure 1 represents a simple aluminum block with various hole sizes on various levels. Typically, all of these holes would be started with a spot drill and because there are a large range of hole diameters, it is likely that more than one spot drill would be used.

Figure 1. Aluminum manifold used to hold five 3/2 pneumatic valves.

For the part shown in Figure 1, after the steps have been machined a 1/2-inch-diameter spot drill will be used to start the four clearance holes for the 1/4 socket head cap screw and to start the 15 1/8 National Pipe Thread (NPT) holes.

Many inexperienced programmers using Mastercam would spot drill for these two sizes of holes in two separate operations. It’s not wrong, but it wastes time and over many parts, this wasted time adds up to lost profit. Time is wasted because the linking parameters will cause the spot drill to retract above the part, cancel the drilling cycle between operations and then establish a new drilling cycle.

To correctly spot drill the 1/8 NPT and the 1/4 Socket Head Cap Screw (SHCS) holes in the same cycle and keep the cycle time to a minimum, Mastercam users can follow the steps outlined below.

• Create wireframe geometry for the part similar to that shown in Figure 2. Using different colors for each hole type can make the selection process quicker and easier.

Figure 2. Wireframe geometry with the various hole types drawn in different colors.

• Switch to the top view.  (This will ensure the tool plane is set to the top.)

In the Sorting window, select Use entity at highest Z depth from the Depth filtering menu.

 (This will tell the system that you wish to use the circle in the top).

Accept this selection. 

In the Drill Point Selection window select Mask on Arc.

 (This will allow only the selection of arcs with the same diameter—an arc does not need to be a complete circle. Mask on Arc does not select that circle as a drilling location. It merely sets the size of arcs that may be selected.)

Figure 3. Window-selected arcs. (Images courtesy of the author.)

Even though the circles in the front face are selected, they will not be seen as drilling points because they do not lie in the tool plane.

You should also notice how both the top and bottom of the holes are selected. The system will automatically sort out duplicate hole locations, so these holes won’t be drilled twice.

• Press Enter on your keyboard to end this selection of holes.
• Select Entities.
  
  
• Select the top of the four counter-bored holes as shown in Figure 4—again use the Mask on Arc option—and then select the four circles. (Using the Mask on Arc option will also ensure that only the centers of the arcs are selected as drilling locations. If you do not use the Mask on Arc option, be very careful that one of the four quadrants of a circle are not accidentally selected as the center.)

Figure 4. Counter-bored circles selected as the drilling locations.

• Press Enter on your keyboard to end this selection of holes.
• Accept these selections.
  
  

To see this being done watch the video “Z Depth of Holes Selection.” 

• Select a 1/2 Spot Drill as the tool. 
  
  
  
  
• Set up the tool parameters as shown in Figure 5.

Figure 5. Spot Drill parameters.

• Set up the Cut Parameters 
  
   as shown in Figure 6.

Figure 6. Drilling cycle with dwell time calculation.

• Set up the Linking Parameters 
  
   as shown in Figure 7.

Figure 7. Linking parameters for the spot drill.

The depth must be set to incremental. Because the two hole sizes are on different surfaces, you must tell it the incremental depth to which to drill.

• Turn the coolant on 
  
   and accept these selections. 
  
  
• Verify 
  
   all of your toolpaths and the results should look similar to Figure 8.

Figure 8. Verify simulator results with the solid stock set to “see through.”

The procedure as described works well when all holes can be spot drilled to the same depth, relative to the starting surface; however, when each hole type requires a different depth, then the following steps will also need to be followed after the previous steps are complete.

• In the Toolpath Manager window, expand the spot drilling operation.
  
  
• Click on Geometry to open up the Drill Point Manager window as shown in Figure 9.

Figure 9. Drill Point Manager window.

• Select point 16. (This should be the first of the counter-bored holes. If you have selected the holes more than once, your first counter-bored hole may not be point number 16.)
• Right-click in the white space near point 16, and select Change at point.
  
  
• In the Drill change at point window, enable the Depth option, set the new depth to –0.25 and apply these changes to subsequent points as shown in Figure 10. (This will set the new drilling depth for the four counter-bored holes.)

Figure 10. Drill change at point window showing the new drilling depth applied to the current and all subsequent holes.

• Accept these selections.
  
  
• Close the Drill Point Manager window. 
  
  
• Regenerate the toolpath. 
  
  
• Post the code for this toolpath and you should see that these last four hole locations have the new Z drilling depth as shown in Figure 11.

Figure 11. Spot drilling canned cycle showing the counter-bored holes will be spot drilled at a depth of –0.25 from the surface and the 1/8 NPT holes will be drilled –0.24 from the surface.

To decrease the cycle time further, you could change the retract level to a Z level of –0.4 absolute.

 However, you need to be aware of the order in which your holes are drilled, or the machine will move the tool at the rapid feed rate (I.E. as fast as it can travel) through the part as shown in Figure 12.

Figure 12. Retract height issues causing the spot drill to rapid through the part.

To avoid the tool crashing into the work piece, you will need to set the retract values, which are applied after a hole is drilled, to an absolute value of 0.1. After the tool moves across the part to the opposite side it may then be set back to an absolute value of –0.4, for the area in which the tool will only move through the machined shelf area. 

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.