CNC and CAD/CAM | 2D Toolpath Terminology

In this article, we describe 2D toolpath terminology with all details include milling, drilling, tapping and etc..

0
347

2D Toolpath Terminology

Though the terminology and ways of working vary widely, all CAD/CAM software needs the same basic information to function. Figure 4 shows parameters common to 2D tool paths.

Figure 4: 2D Tool Path Terminology

Clearance Height is the first height the tool rapids to on its way to the start of the tool path. It is usually set 1.000in above the top of stock because this makes it easier to see if the tool length offset register was set properly.
Rapid Height is the second height the tool rapids to, and the height the tool retracts to between moves (unless set higher to clear clamps). It is usually set to .250in above the top of the finished part face.
Feed Height is the last height the tool rapids to before starting to feed into the cut. It is usually set to .1000in above top of stock. No rapid motion occurs below this height.
Top of Stock is the top of the finished face of the part. This value is used as the reference plane for depths.
Stepdown is the depth of material removed with each cutting pass. This illustration shows one pass, but for deeper cuts or harder materials, many passes may be required to cut to the final depth.
Depth is the final cutting depth of the machining operation.
Stepover sets how much material the tool removes with each pass in the XY direction.
XY Stock Allowance is the material remaining on the finished wall of the part to be removed by subsequent operations.
Z Stock Allowance is the material remaining on the finished floor of the part to be removed by subsequent operations.
Toolpath Centerline represents the actual coordinates in the CNC program. In this book, rapid moves are shown as dashed lines and feed moves as solid.

Facing

Facing is often the first machining operation. It is used to cut away excess material and finish the highest flat face of the part.Depending on how much stock is removed, several roughing cuts may be required. A smaller finish pass ensures a flat surface and good surface finish.
Use a face mill when possible for all but the smallest part. The large diameter of facing mills and multiple carbide insert cutting edges provide for very high material removal rates.
High speed loop transitions between cut passes produce a fluid tool motion that place less stress and wear on the CNC machine.

Figure 5: 2D Facing Toolpath

Rules for Facing

  • Because face mills do not plunge well, start the tool path far enough away from the part so the tool does not plunge into the stock material.
  • Be aware that saw cut stock can vary considerably in thickness from one part to another: as much as .05in or more. When planning roughing passes, be sure to account for the worst case stock material –maximum height and add additional roughing passes as needed. It is better to have a “air cut” or two with the shortest stock than to have the tool engage too much material for the highest which could cause the tool to break or the part to be pushed out of the vise or fixture.
  • Facing tool paths do not use cutter compensation (CDC).

You may be interested also “CNC Milling | Difference Between 2D – 3D and 4-Axis Machined Parts”

2D Contour

Contour operations are used to rough and finish outside part walls as shown in Figure 6. Use Cutter Diameter Compensation (CDC) on high tolerance features so the tool path can be adjusted at the machine if needed to account for tool wear and deflection.

Figure 6: 2D Contour Tool Path

Rules for Contouring

  • Only use CDC when needed. Ifusing new tools and conservative machining parameters, features will likely be within .005 inches of the programmed path without adjustment.
  • Start the tool path off the part to allow CDC to be fully in effect for the entire operation.The combined line-arc lead-in/out moves shown in Figure 4 work for most contours. The line is for activating/deactivating compensation, and the arcs blend the path into the part wall smoothly.
  • Set a rapid height value to clear all clamps or other obstacles between cuts.
  • Rough the walls and leave a constant thickness of material for the finish operation. This ensures even cutting pressure on the finish pass and thus a more accurate part.
  • Extend the cut depth of full walls slightly below the bottom of the wall, but be careful not to cut into the machine table or vise hard jaws! This way, when the part if flipped over to face the other side, no flashing will be left on the bottom of the walls.
  • Mill tools cut well in the XY direction, but not as well when plunging in Z. When possible, plunge the tool away from the part to avoid Z-moves into the stock material.
  • When taking multiple depths of cut, make the last pass at full depth to remove any marks left by previous depth cuts.
  • For tall walls, consider taking one additional finish pass. This so-called “spring pass” follows the same path twice to ensure the walls are perfectly straight and not slightly tapered due to cutting pressure which causes the tool to bend.

Cutter Diameter Compensation

Cutter Diameter Compensation provides a way for tool paths to be adjusted at the machine to compensate for tool wear and deflection. Figure 5 shows how CDC Right (G41) causes the tool to veer to the right of the programmed path.
The compensation value is found by measuring the part feature and subtracting the actual dimension from the desired dimension. The difference is entered in the control CDC register for the tool. The next time program is run, the tool will be offset by this value.

Figure 7: Cutter Diameter

CDC must be turned on or off with a line move, never an arc. Commanding G40/G41/G42 with an arc move will cause a diameter compensation error that will stop the program.
CDC is activated at the end of the line on which it is called, as shown in Figure 5. Notice how the tool moves at an angle from the start to end of the lead-in line. Activate CDC while the tool is away from the part so this angle move happens away from the finished part surfaces. The line-arc moves shown in Figure 4 provide ample clearance for the tool for this purpose.

Pocketing

Pocket tool paths are used to remove excess material. An example of a spiral pocket with helical entry is shown in Figure 6. CDC is not active during the roughing cuts, but may be used for finish passes on walls.

Figure 8: Pocketing

Rules for Pocketing

  • Rough passes should leave a constant thickness of material on the walls and floor of the pocket to be removed by the finish passes.
  • Consider using a roughing end mill to remove most of the material. These serrated mills can remove material at a far faster rate than finish end mills. They do leave a poor finish on the floors and walls that must be finished with a separate finish tool and operation.
  • Helical moves are a good method for entering a pocket. If space does not allow a helical entry, use a center-cutting end mill or plunge the tool through an existing hole, or a pilot hole created for this purpose. The pilot hole must be at least 50% of the tool diameter.
  • Spiral pocketing paths that start near the center of the pocket and move outward in a counter-clockwise direction are best because they cause the tool to continually climb cut.
  • Use CDC only on finish passes.

Slot Milling

Slots may be machined using the CAD/CAM contour, pocket, or specialized slot milling functions.

Rules for Slot Milling

  • Use a tool smaller than the width of the slot whenever possible.
  • A ramp plunging move as shown in Figure 7 is the most efficient way to mill a slot.
Figure 9: Slot Milling

Chamfer Milling

Chamfer is a type of 2D contour milling. Chamfer mills are of various tip angles are in high speed steel, carbide, or as insert type tools.

Rules for Chamfer Milling

  • Because the tip of a chamfer mill is not a sharp point the width of the chamfer may be wider than expected if you set the tool like an end mill. To prevent cutting too deep, consider raising the TLO about .010 inches after setting it. Then machine the chamfer, check its size, and adjust the TLO down as needed to produce the correct width chamfer.
  • Offset the chamfer mill as shown in the magnified view below to move the tool tip is away from the bottom of the chamfer. This ensures a clean bottom edge and, because tool rotational velocity increases with tool diameter, is a more efficient to use the tool.
  • Chamfer with a spot drill to precision de-burr sharp corners.
Figure 10: Chamfer Milling

Radius (Corner-Round) Milling

Radius milling is a form of contour milling. Corner round tools are available in high speed steel, carbide, or insert type tools.

Figure 11: Radius Milling

Rules for Radius Milling

  • The horizontal and vertical cutting edges of a radius mill are sloped slightly to blend the radius into the walls.
  • Take two finish passes to improve surface finish.
  • Another way to form a corner radius is to use a ball mill and 3D contour tool path. This method saves purchasing a radius mill and is suitably efficient for prototype and small production manufacturing.

Center Drill

Center drills create a conical cut on the face of the part. This helps prevent subsequent drill tools from wobbling and thus ensures they will be positioned precisely.

Figure 12: Center Drilling

Rules for Center Drilling

  • A good rule of thumb is to use a tip depth equal to the radius of the subsequent drill hole.
  • Use a combination center-spotting drill for spot faced holes.

Drilling

Holes that are less than the diameter of the drill can be created with a single plunge move. Deeper holes use a Peck Drill cycle where the tool is retracted after removing a small amount of material (typically .050 inches).

Figure 13: Drilling

Rules for Drilling

  • Center drill all holes to ensure they are located precisely.
  • Peck drill (G83) holes that are deeper than the diameter of the drill. Full retract peck drill cycles take more time than partial retracts, but minimize the chance of tool breakage.
  • CNC Programs control the tip of the tool. Be sure to provide additional depth to compensate for the tool tip and include a breakthrough allowance to prevent a flange or burr on the bottom.

Tapping

Tap cycles are similar to simple drill cycles except the feed and speed are coordinated to properly match the thread lead. CAD/CAM software calculates the feed according to the cutting speed and threads per inch (TPI) of the tap.

Figure 14: Tapping

Rules for Tapping

  • Use the drill chart in Appendix A to find the correct drill diameter for cutting taps. Use the manufacturers recommended drill size for form taps.
  • Consider brushing on tapping fluid instead of using coolant for small tapped holes to help prevent the tap from breaking.
  • Tapped holes smaller than about #8 can be difficult to create on the machine without breaking the tap. Consider tapping these holes by hand rather than on the CNC.
  • If the machine does not support Rigid Tapping, a floating tap holder is required to tap.
  • Be sure to specify a tip depth sufficient to account for the tip and initial taper of the tap.
  • Older machines may require a larger feed height to allow the machine spindle to reach full speed before the thread engages the material.

Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleCNC Milling | Difference Between 2D – 3D and 4-Axis Machined Parts
Next articleCNC | Identify the Elements of CNC Lathe