The articles in this section of the Knowledge Base involve working from the Tool File interface. For general information regarding Tool Files or how to access them, see Understanding the Tool File Interface.

This article provides information regarding adding a new vertical drill within a tool file.

From the Tool File interface, with the Vertical Drills radio button selected, select Add Tool.

A new tool named "Tool 0 – New Vertical Drill" appears in the Tool List. Select the new tool.

Fill in the missing information to the right of the Tool List.

1. Tool Name (Optional) – User determined name for the vertical drill being added. The Tool Name is the name that appears in the Tool List Panel on the left of the Tool File UI.
   
2. Common Tool Name – This number should be in the form the machine needs to see in the G-Code. The Common Tool Name and Actual Tool Name should match each other.
   
3. Actual Tool Name – This number should be in the form the machine needs to see in the G-Code. The Common Tool Name and Actual Tool Name should match each other.
   
4. Common Tool Diameter – This value is used by the program to determine which tool to use.  
   
5. Actual Tool Diameter – This value refers to the new diameter of sharpened bits and is the value used in G-Code.
   
6. Feed Speed – This value is the speed the tool uses once it has penetrated the material.
   
7. Entry Speed – This value determines the tool's penetration speed from the face of the material to the end depth of the machining operation.
   
8. Rotation Speed – This value refers to the speed of rotation.
   
9. Pecking Number – The number of times the bit plunges into a single hole (for thick, delicate, or rigid materials). In other words, the depth of the hole is divided by the Pecking Number.
   
10. Type Info  – This setting only applies if the type of bit being used by the machine is specified.
    
1. 0  – No Type
   
2. 1  – Brad Point
   
3. 2  – V Point
   
4. 3  – Large Diameter
   
5. 4  – Horizontal Bore Only
   
6. 5  – Horizontal Bore & Dowel          
   
11. X Position – This value refers to the position of the bit on the X-axis. It can be left blank unless you plan on gang drilling with this tool.
    
12. Y Position – This value refers to the position of the bit on the Y-axis. It can be left blank unless you plan on gang drilling with this tool.
    
13. Z Position – This value refers to the position of the bit on the Z-axis. It can be left blank unless you plan on gang drilling with this tool.
    
14. Minimum X and Y , and Maximum X and Y reflect how far the bit can physically reach on the table.
    
15. Offset X – The offset value of the bit on the X-axis. It can be left blank unless you plan on gang drilling with this tool.
    
16. Offset Y – The offset value of the bit on the Y-axis. It can be left blank unless you plan on gang drilling with this tool.
    
17. Tool Safe Height 1 – This sets the retract height of the tool head. Safe Height 1 is the value that the head retracts to when making rapid movements between operations requiring different tools or moving to begin a machining operation. Tool Safe Height 1 may be set to any value as desired, but a typical value is .75" above the material's surface. This setting applies to both spreadsheets and IPP files.
    
18. Tool Safe Height 2 – This sets the retract height for the tool head. Safe Height 2 is the value that the head retracts to when making rapid movements between operations requiring the same tool. Tool Safe Height 2 may be set to any value as desired, but a typical value is .25" above the material's surface. This setting applies to both spreadsheets and IPP tool files.
    
19. Head Value – This sets the number identifying a specific head in multiple head machines. An example of these machines would be dual head machine systems (top and bottom heads). It is a reference to which head is required in a machining operation. Some single head machines may also need it. This setting applies to both spreadsheets and IPP tool files.
    
20. Binary Value – This sets a unique binary placeholder equivalent for each vertical drill. For example, see the list below for tool numbers on the left, and their binary placeholder equivalents on the right:
    

1 = 1


2 = 2


3 = 4


5 = 16


6 = 32


7 = 64


8 = 128


9 = 256


10 = 512


11 = 1024


12 = 2048


These binary equivalents make it possible for the program to create a unique number for each unique combination of drills required in a machining operation. The unique number identifies which drills are to be used in a single operation using multiple drills.


Enter the binary placeholder equivalent numbers for each drill number as per the list above, and select the Apply button after each one is entered. This setting applies to both spreadsheets and IPP tool files.


21. Use Router – This determines if a router bit from the router spindle is used to drill the specified diameter holes.
    
22. Aggregate Drill Block – This sets whether or not the drill tool number represents an aggregate drill block. If the checkbox is checked, additional options are displayed for the drills to be included in the aggregate block. Enter values for the properties as required by your machine. This setting applies to IPP tool files only.
    


Fig. 03 – Aggregate Drill Block Properties



1. #X Drills – Number of drills in the X-Axis
   
2. #Y Drills – Number of drills in the Y-Axis
   
3. X Drill Spacing – Space in mm between the X Drills
   
4. Y Drill Spacing – Space in mm between the Y Drills
   
5. Index X – X row number that the Index Drill resides
   
6. Index Y – Y row number that the Index Drill resides
   
7. Allow Over Drilling - Allow the aggregate to drop on existing holes
   
8. Max # Redrills – Maximum number of times a hole can be redrilled
   


Fig. 04 – Aggregate Drill Block Pattern
23. Rotation – Select one of the following:
    
1. Clockwise
   
2. Counter Clockwise
   
24. Axis – This is used for line boring or gang drilling. If the new bit is on the part of the head that runs in the X, select "X Axis" otherwise, select "Y Axis."
    
25. Default Depths – Add at least one Default Depth for the vertical drill. A Default Depth value is necessary for the tool to show up in the Single Parts Editor (2D Machining Tools).
    

Before leaving the Tool File UI, select Apply to save the new Tool and OK to exit.