1. Introduction: Why Use Automatic Chamfering?

In manual programming, calculating the coordinates for a simple 45° chamfer or a 90° radius used to involve complex trigonometry and multiple lines of code. However, modern CNC controls (such as Fanuc, Haas, and Mitsubishi) offer a built-in shortcut that allows you to program these features directly into your linear motion blocks using ,C and ,R.

Using automatic chamfering and rounding provides three major benefits on the shop floor:

  • Reduced Code: Perform complex corner moves in a single line of G-code.

  • Accuracy: Eliminates manual calculation and rounding errors.

  • Speed: Drastically reduces the time required to write and debug programs.

2. Syntax & Working Principle

The tool moves toward the intersection point defined by the X and Z coordinates (the “virtual” corner where the two lines would normally meet). The control looks ahead, calculates the start and end points of the feature based on your value, and “cuts the corner” before proceeding to the next coordinate.

Side-by-Side Programming Logic

OPTION A

Chamfering (,C)

Inserts a flat, angled surface cut between two intersecting linear steps to break sharp edges cleanly.

Command Syntax:

G01 X_ Z_ ,C_
  • X, Z: The target coordinates of the intersection point (virtual corner).
  • ,C Value: The linear distance from the corner to the start of the chamfer.
OPTION B

Corner Rounding (,R)

Creates a smooth, blended circular arc radius tangent to both intersecting lines of programmed tool motion.

Command Syntax:

G01 X_ Z_ ,R_
  • X, Z: The target coordinate position where the intersecting straight lines meet.
  • ,R Value: The specific radius dimension value of the blend arc to insert.

Note:   On many Fanuc controls, the comma ( , ) is mandatory before the C or R variable.

3. Practical Turning Program Example

Imagine a part where you need to turn an outer diameter from 20mm to 50mm. You want to insert a 2mm chamfer at the first corner and a 5mm radius at the second corner.

N10 G00 X0. Z2.0 ;
N20 G01 Z0. F0.2 ;
N30 G01 X20.0 ,C2.0 ; (Move to X20 and insert 2mm chamfer)
N40 G01 Z-25.0 ,R5.0 ; (Move to Z-25 and insert 5mm radius)
N50 G01 X50.0 ;
N60 G00 X100.0 Z100.0 ;
Explanation:

  • N30: The tool prepares to turn the face up to X20, but stops 2mm early to execute a 45° chamfer toward the next Z move.

  • N40: The tool moves along the Z-axis but, instead of a sharp corner at the end, it creates a smooth 5mm radius before moving to the next X diameter.

Important Notes for the Shop Floor

  • Next Block Requirement: The control must know the next move (the next block) to calculate the chamfer or radius. You cannot end a program immediately after a ,C or ,R block.

  • Tool Compensation: For maximum accuracy, ensure G41/G42 (Cutter Compensation) is active. This ensures the tool nose radius is accounted for, preventing “under-cutting” on your chamfers.

  • Value Constraints: The value of the chamfer (C) or radius (R) must be smaller than the length of the shortest line segment in the move. If it’s too large, the machine will throw an “Improper Geometry” alarm.

Key Fanuc Parameters for Chamfering & Corner Rounding

1. Parameter 3405 (Bit 4: CCR)

This is the most critical parameter for the syntax you requested.

  • Setting: If Bit 4 (CCR) is set to 1, the control recognizes the comma (,) before the C or R.

  • Setting: If set to 0, the control may expect just C  or R  (which can sometimes conflict with axis names or taper commands in G01).

  • Recommendation: For modern programming standards on cnclearning.com, ensure this is set to 1 to use the ,C  and ,R format.

Parameter 3405 (Bit 6: RDP)

This bit determines how the radius is calculated.

  • Setting: It specifies whether the corner rounding value is treated as a radius or a diameter increment.

  • Standard: It is almost universally set to radius (0) for corner rounding.

3. Parameter 5111 (Chamfer Amount)

This parameter defines the default chamfering amount used in cycles like G76 (threading) or when a specific value isn’t fully defined in certain canned cycles.

How to Access and Change Parameters

Warning: Changing system parameters can alter machine behavior. Always back up your parameters before making changes.

  1. MDI Mode: Place the machine in MDI mode.

  2. Parameter Write Enable: Press the [SETTING] softkey and change “PARAMETER WRITE” from 0 to 1. The machine will usually trigger an alarm (this is normal).

  3. System Screen: Press the [SYSTEM] hard key on the keypad (visible in your uploaded image).

  4. Search: Type the parameter number (e.g., 3405) and press the [NO. SRH] softkey.

  5. Edit: Use the arrow keys to highlight the specific bit (Bit 4 is the 5th digit from the right, as they count 7-6-5-4-3-2-1-0).

  6. Input: Type the new value and press [INPUT].

  7. Reset: Turn “PARAMETER WRITE” back to 0 and press RESET to clear the alarm.

When working with ,C and ,R commands, your Fanuc control might trigger specific alarms if the geometry or parameters are incorrect. Here is a guide to the most common issues you’ll encounter on the shop floor.

Alarms and Troubleshooting

This is the most frequent alarm when using automatic cornering.

  • The Cause: The value of the chamfer (C) or radius (R) is too large for the programmed move. If your line segment is 5mm long and you command a ,C6.0, the control cannot “fit” the chamfer.

  • The Fix: Reduce the C or R value, or increase the length of the coordinate move in the following block.

  • The Cause: This occurs when a corner rounding or chamfering command overlaps with the next corner command. Basically, you are trying to start a new chamfer before the previous radius has finished.

  • The Fix: Ensure there is enough linear distance between corners to accommodate both features.

  • The Cause: Often caused by Parameter 3405 Bit 4 (CCR) being set to 0. The machine reads the ,C but doesn’t know the comma is part of a special command, so it treats it as a syntax error or simply ignores it.

  • The Fix: Change Parameter 3405 Bit 4 to 1 to enable the comma-based syntax.

Parameter Name Function Recommended Setting
3405 #4 CCR Enables Use of Comma (,) for C and R 1 (Enabled)
3405 #6 RDP Specifies Radius or Diameter for Rounding 0 (Radius)
5111 Standard C Default chamfer for specific canned cycles Set per shop standard

  • Check the Next Block: Does a motion command (G01/G02/G03) immediately follow the ,C or ,R block? Non-motion blocks like M08 or G04 can sometimes break the “look-ahead” buffer.

  • Check Tool Compensation: Are you using G41/G42? If so, ensure your tool nose radius (R) in the offset page is accurate. If the tool radius is larger than the programmed corner radius, the machine will alarm out.

  • Check Plane Selection: Ensure you are in the correct plane (G17 for Milling, G18 for Turning). Corner rounding functions are plane-dependent.

Leave a Reply

Your email address will not be published. Required fields are marked *