- Home
- Courses
- Courses for Manufacturing
- CNC Lathe & Turning Centers
- Course Types
- Internet Course
- DVD / CD-ROM Course
- Video / Print Course
- CNC Machining Centers
- Course Types
- Internet Course
- DVD / CD-ROM Course
- Video / Print Course
- CNC Swiss
- Course Types
- Internet Course
- Precision Measurement for Machinists
- Course Types
- Internet Based Course
- CD-ROM Based Course
- Automatic Bar Machines
- Fastener Production Equipment
- Stamping Presses
- Geometric Tolerancing
- SPC
- CNC Lathe & Turning Centers
- Courses for Education
- CNC Lathe & Turning Centers
- Course Types
- Internet Course
- DVD / CD-ROM Course
- CNC Machining Centers
- Course Types
- Internet Course
- DVD / CD-ROM Course
- CNC Swiss
- Course Types
- Internet Course
- Precision Measurement for Machinists
- Course Types
- Internet Course
- DVD / CD-ROM Course
- SPC
- CNC Lathe & Turning Centers
- Courses for Individuals
- Online Courses
- Cursos De Español
- Dominio de Tornos CNC
- Automático Barra Máquinas
- De un Solo Husillo
- Brown & Sharpe
- Tornos Bechler / Strohm
- Multi-Husillo
- Acme Gridley
- Davenport
- New Britain
- Custom Development
- Courses for Manufacturing
- Quick View
- Tools & Information
- Support
- Company
Quality Control Troubleshooting Guide
CNC Lathe and Turning Centers
It often takes years for a new machinist to learn all of the likely causes for the various quality problems that will arise. These troubleshooting algorithms can help your personnel by giving them the benefit of years of experience at the click of a mouse. Select the Quality Defect in the list below, then follow the links (if applicable) to learn the most likely causes.
Select Quality Defect:
Select the statement that best represents the situation:
- Several features cut by the SAME TOOL are out of tolerance by the SAME amount in the SAME axis directions.
- Several features are out of tolerance which were cut by DIFFERENT tools.
- Only ONE of the features cut by a tool during a tool path is out of tolerance.
Several features cut by the SAME TOOL are out of tolerance
by the SAME amount in the SAME axis directions.
- For New Setups:
- Check the setup documentation to be sure the correct tool is being used for the cut.
- Check the cutting edge to be sure it is not worn, damaged or broken. If so, replace the insert and adjust any WEAR offset as required.
- Be sure the Tool Offset for the tool is entered in the Offset Table and made active in the Program.
- Determine if Tool Nose Radius Compensation (TNRC) is applied to the tool. If it is, be sure it is activated in the Program with the correct G41 or G42 code. If TNRC is not required, be sure G40 is active to cancel any previous TNRC value which may have been active for a previous tool.
- Check the Tool Tip value is correct for the configuration of the tool holder being used.
- If TNRC is active, check the TNRC offset amount to be sure it is the correct value.
- Be sure the work holding device is operating properly and its locating surfaces are making full contact with the workpiece.
- Make sure the Tool Holder is securely mounted and the tool correctly aligned in the holder.
- For Maintaining an Existing Setup:
- Check the cutting Insert to be sure it is not worn, damaged or broken. If faulty, replace the Insert and adjust any WEAR offset as required. If the Insert is not faulty, consider calculating and entering a Wear Offset.
- Be sure the workpiece is placed against the locating surfaces and it is securely mounted.
- Be sure there is no damage to the work holding device or its locating surfaces, such as chuck jaws.
- Be sure the Tool Holder is securely mounted and correctly aligned.
- Perform a Zero Return or HOME to remove any errors in the Coordinate System.
Several features are out of tolerance which were cut by DIFFERENT tools.
- Perform a Zero Return, or HOME, to remove any positioning errors that may have occurred.
- Check the part to be sure it is seated against the locating surfaces on the work-holding device.
- Check the location of Program Zero to be sure it is correct for the part.
- Check the Program to see if Tool Nose Radius Compensation (TNRC) is either required but not active, or not required but remains active. Enter the code to correct the situation as required.
- Check the Tool Offsets to be sure they were entered correctly and that the correct code occurs in the Program to make them active.
Only ONE of the features cut by a tool during a tool path is out of tolerance.
- Consider entering a second Tool Offset for the tool. Make it active before the problem feature to correct the problem, then reactivate the original Offset after the feature is completed. Notify the Programmer of the problem.
- If program editing is allowed, find the coordinates in the program that created the feature and edit them to correct the problem.
- Check to be sure the cutting edge of the Finish Tool Insert is not dull, chipped, broken, or has material build-up.
- Be sure the Insert is correct for the type of finish cut.
- Check to be sure the cutting edge is positioned on the centerline of the spindle.
- Check the size of the workpiece after the Rough pass to be sure the Finisher is not removing too much material in the finish pass, or that the Finisher is not removing enough material.
- Check the Feed Rate for the Finish pass.
- Check the Spindle Speed during the Finish pass.
- Be sure the coolant reaches the Finish Tool during the cut so that chips are flushed away from the Insert during the cut. Be sure long chips do not tangle around the holder and scratch the surface.
- Make sure the material for the workpiece is correct and that its hardness is within normal limits.
Select the statement that best represents the situation:
- Chatter source can be isolated to a SINGLE tool.
- Chatter source CANNOT be isolated to a single tool.
Chatter source can be isolated to a SINGLE tool.
- Check the cutting edge to be sure it is not dull, worn, or broken.
- Be sure the cutting edge is on the Centerline of the Spindle.
- Check to be sure the tool is firmly mounted in the Tool Holder and does not extend out any further than necessary.
- Make sure the workpiece is fully supported during the cut, especially if the part is long.
- Be sure the Tool Holder is firmly mounted to the Turret.
- Check the Feed Rate of the cut. Increase if possible.
- Check the depth of cut. Increase if possible.
- Check the Spindle Speed during the cut. Decrease if possible.
Chatter source CANNOT be isolated to a single tool.
- Be sure the workpiece is securely mounted in the holding device.
- Check the Feed Rate.
- Check the Spindle Speed.
- If the lathe is Bar fed, be sure the bar is not bent and has the proper support along its length.
- Check the material to be sure it is correct and that the hardness is normal.
- Check the coolant supply to be sure it is the correct concentration and is clean.
- Ask maintenance to check the Spindle Bearing.
- Make sure the machine is securely mounted to the floor.
- Look for an external source of vibration either inside or outside the shop.
- Be sure the Drill is the correct diameter.
- Check the Drill Point to be sure it is sharp and not damaged.
- Check the Drill to be sure it is not bent.
- Check the Drill Collet to be sure it is clean and not not broken or damaged.
- Be sure the length of the Drill Point cutting edges are the same.
- Be sure the Tool Holder is properly aligned with the centerline of the spindle.
- Make sure the Feedrate is not too high causing the Drill to deflect or bend.
- Check the drill point to see if the drill is dull, broken or damaged.
- Check the Drill Collet to be sure it is holding the Drill securely.
- If all holes created by this Drill have the same depth problem, check the Z axis Geometry and Wear Offsets for the Drill to be sure they are correct. Adjust as required.
- If the other holes created by this drill are correct in depth, adjust the Z axis coordinate in the Program of the problem hole.
- Check the drills that precede the final drill to be sure they are the correct size.
- Be sure the final drill is not dull or damaged.
- Be sure the coolant is reaching into the hole or consider using a coolant hole drill.
- Check the drill to be sure it is not bent.
- Check the Drill Collet to be sure it is not damaged, is clean, and firmly holds the drill.
- If chips are not breaking into small sizes that are easily removed from the hole, consider a chip-breaking drill.
- Roundness:
- Check for a bent Drill.
- Be sure the drill does not extend from the Drill Collet any further than necessary to create the correct depth of the hole.
- Check the length of the cutting edges of the Drill to be sure they are the same length.
- Be sure the Feedrate is not too high causing the drill to deflect or bend.
- Concentricity:
- Check the Spot Drill which precedes the Drill to be sure it is not broken, chipped or dull.
- Check the Drill collet to be sure it is not dirty, broken or has burrs.
- Make sure the Drill Collet Nut is securely tightened.
- Check the Drill Holder to be sure it is correctly aligned to the Spindle Centerline and securely mounted.
- Make sure the work holding device or Spindle Bearing does not have any runout.
- If the Boring Bar is adjustable, be sure the lock screw on the adjustment mechanism is tight.
- Check the cutting tool to be sure it is sharp and not damaged.
- Be sure the correct Tool Offset values have been entered and are currently active.
- Check the Boring Bar to be sure it is not bent.
- Be sure the Tool Holder is properly aligned with the centerline of the spindle.
- Make sure the Depth-of-Cut or Feedrate is not too high causing the Boring Bar to deflect.
- Check the condition of the Boring tool to be sure it is not damaged or worn.
- Be sure the correct Boring Bar is mounted and called up by the Program.
- Check that the correct Tool Offsets are entered and active.
- Be sure the Boring Bar is securely mounted to the Tool Holder.
- If the boring bar is following a drill, be sure the drilled hole is correct.
- Be sure the Feedrate is correct so that deflection of the Boring Bar does not occur.
- On bar fed lathes, be sure the workpiece is not pushed back into the collet.
- Check the cutting tool to be sure it is sharp and not damaged.
- Make sure the tool cutting edge is correctly positioned and on the centerline of the workpiece.
- Check to be sure the Tool Holder is securely mounted.
- If possible, reduce the length of the bar that extends from the Tool Holder.
- Use the largest diameter boring bar possible for the workpiece diameter to increase tool stiffness.
- If the workpiece is long, shorten the overhang or change the order of machining to increase workpiece stiffness.
- Make sure the Depth-of-Cut is not too high on the final pass.
- Use the Override control to change the Speed and Feed rates until the finish improves. Note the percentage used and calculate and enter new rates if allowed by shop practice.
- Check the depth of cut and adjust as required.
- Incorrect Diameter or Pitch of Threads:
- Check to be sure the correct style of tap is used and it is the correct diameter and thread pitch.
- Be sure the drilled hole is not oversize or undersize.
- Be sure the correct tapping G code is active.
- Make sure the no X axis tool offsets are applied.
- Make sure the hole to be tapped is straight.
- Faulty Thread Form:
- Make sure the tap is sharp and coolant is reaching the hole to clear chips during the cycle.
- If a floating holder is used, make sure the proper amount of float occurs and that the holder is properly aligned with the workpiece.
- Make sure the hole to be tapped is straight.
- Make sure the drilled hole is not undersized or oversize.
- If chips are packing into the flutes, use a fast spiral tap.
- Reduce the overall tapping speed and the withdrawl speed.
- Poor Thread Finish:
- Check to be sure the correct style of tap is used and it is the correct diameter and thread pitch.
- Be sure the correct coolant is used for the material being machined.
- Reduce the overall tapping speed and the withdrawl speed.
- Damaged Tap:
- Make sure the hole depth is correct.
- Select the style of tap for the blind or through-hole to be tapped.
- Make sure the hole is not undersize.
- Be sure the correct tapping cycle is active.
- Make sure no X axis offsets apply to the tool.
- Make sure the correct coolant type and viscosity is being used.
- Material hardness may not be correct, or there may be hard spots in the material.
- Incorrect Diameter or Pitch of Threads:
- Be sure the correct thread cutting insert is installed and that it is not damaged or worn.
- Make sure the correct thread cutting G code is active.
- Be sure the correct tool offsets are applied.
- Make sure the workpiece has been machined to the correct diameter and no taper exists.
- Be sure the spindle is set to Constant Spindle Speed during thread cutting.
- Decrease the depth of cut and increase the number of passes to reduce "spring-back" in the material.
- Faulty Thread Finish:
- Make sure the cutting insert is not damaged or worn.
- Adjust coolant flow to make sure chips are not being recut during the thread cutting cycle.
- Make sure the insert is correctly mounted in the tool holder.
- Make sure the tool holder is the correct hand for the direction of spindle rotation and is securely mounted.
- Reduce the depth of cut per pass in the thread cycle and increase number of passes.
- Reduce the amount of over hang in the tool holder.
- If shop practice allows, change the machining sequence to increase stiffness in workpiece during thread cutting.
- Make sure the coolant being used is recommended for the material being machined.