Adding machining to parts, whether it be vertical or horizontal drilling, routing or sawing, the steps are very similar.
To add machining to a part, you must first select the desired tool, then enter a depth and specify if the operation will be on FACE 5 or FACE 6. For routing and sawing tools, you will need to select the type of tool compensation to use: Left, Center, or Right.
To use the Pick Existing Entities, you must have an object or polyline drawn.
For vertical drilling operations, the diameter of the circle drawn has to match the diameter of the tool used.
For horizontal drilling operations, you will need to either draw a rectangle and convert it to a polyline or draw a polyline – the width of the rectangle must match the diameter of the tool being used, and the length must match the depth you specified.
Also, for horizontal drilling operations, a value in the Other Z Value will move the center of the drilling operation along with the thickness of the part.
When using the Draw function, you must do the following:
For vertical and horizontal drilling operations, you must pick a point in the drawing based on the center of the hole. As an option, you can select a second point (creating a straight path) and specify the distance between holes.
For routing operations, select the type of machining operation to draw from the list:
None - Allows you to draw a polyline freely. Once the command has been completed, the machining will be applied to the new polyline.
Square Cutout/Pocket - Allows you to create a rectangular cutout. Requires you to pick a point for the starting corner of the rectangle and then to pick the opposite corner creating the width and length of the rectangle simultaneously.
Round Cutout/Pocket - Allows you to create a circular cutout. It requires you to pick a point for the center of the circle and specify the diameter of the hole.
Corner Notch - Allows you to notch the corner of a part (for example, a toe kick notch). It requires you to pick a corner on the part and then specify the width and length of the notch.
Radiused Corner Notch - Allows you to draw a concave radius on a corner. Requires you to pick a corner on the part and then specify the radius.
Chamfer Corner - Allows you to create a diagonal cut across the corner of a part. It requires you to pick a corner on the part and then specify the distance along each edge.
Fillet Corner - Allows you to round over the corner of a part. Requires you to pick a corner on the part and then specify the radius.
For sawing operations, you must create straight, vertical, or horizontal lines by pick a start and endpoint.
In the event that machine tokens do not represent the location of the intended operation location correctly, double check that the orientation of 3D space is correct, to avoid any erroneous token placement, as the default orientation of the XYZ axis in 3D is not reflective of the way most parts in a product will be oriented. Altering the XYZ axis is as simple as rotating the compass on the bottom left corner of the UI, and rotating the compass until it accurately displays the way the part is oriented. Checking Part Properties will display the orientation of the part and assist in determining where to place the token.
Whole part misoriented vs. a single operation on the wrong face: If the entire part appears mirrored or misplaced, the cause is usually the 3D orientation/XYZ compass issue described above. If instead only one machining operation (for example, a single dowel or construction hole token) is on the wrong face while the rest of the part is correct, check that operation's own token parameters first — several associative tokens (including CAMLOCK, CONST, and HOLES) include a "Drill from the Opposite Side" parameter that independently controls whether that specific operation machines Face 5 or Face 6, separate from the part's overall orientation. See Machine Tokens for the parameter details of each token type.
If the issue instead affects every part rather than one operation, the machining is still coming from the parts — check whether a shared subassembly or library template carries the token, and whether the Global file's default tooling has been changed.
The "Flip Face 6 Type" setting will not help here. That setting controls only how parts that already have Face 6 machining are oriented in the CNC output. It does not add Face 6 machining, it does not remove it, and changing it will not suppress an unexpected or empty Face 6 file. Changing it on a machine that requires a flip will cause every genuine Face 6 part to run misoriented. See Overview: Integrated Post Processor Tool Files (IPP) before altering any tool file value.
Shelf holes drilling on the wrong face after a manual depth change: If adjustable shelf holes (SHLF or SHELF tokens) move to the wrong face after manually shortening a token's Face Bore Depth, check the global variable G!Drill_Through_Back_for_Adj_Shelves before troubleshooting the token itself — if it's left enabled, machining can shift to Face 6 (the external/back face) once the depth no longer reaches through the panel. See Machine Tokens for the SHLF/SHELF token parameters.
This video provides helpful tips to do this effectively: