Common Problems with Circular Interpolation

Below are common problems an user can experience during circular interpolation.  We recommend using a boring head for holes that require tolerances less than a 0.001 in  / 25.4 μm.

The cutter deflects during the cut.

A long tool can cause the cutter to deflect during the cut.  

Corrective Action:
  • Use the shortest tool possible.

The cutter leaves marks on the part.

Using the same entry and exit point can cause marks on the part.

Corrective Action:
  • offset the entry and exit point.
  • use a shallow exit angle. [1]

Setting 85 (Maximum Corner Rounding) Has an Incorrect Value - Mill

Setting 85 defines the machining accuracy tolerance around corners. The default value is 0.025" (0.635 mm). If the value of Setting 85 is too low, the control may interpret exact stops between lines of code. This can cause jerky motion, finish problems, and repeatability problems.

The control can cut corner [1] within tolerance at a higher feedrate than it can cut corner [2].

Use this setting to smooth out the motion of the machine in corners, or to make the machine more accurate when trying to hold a close tolerance.

A higher value for this setting lets the machine maintain higher feedrates through a corner for decreased cycle times, but it allows more deviation from the programmed path. A lower value reduces deviation, but also reduces the feedrate for increased cycle times.

Note: Setting 191 affects Setting 85. For example, when Setting 191 is ROUGH, the value of Setting 85 is multiplied by 4. When setting 191 is FINISH, the value of Setting 85 is divided by 4. 

Helpful Hint:

You can use G187 to temporarily override Setting 85 in a program. The E address with G187 commands the temporary corner rounding value. For example, G187 E0.005 temporarily sets the corner rounding value to 0.005. Refer to your Operator’s Manual for more information about G187Setting 191 and Setting 85.

Setting 191 (Default Smoothness) Has an Incorrect Value

This setting defines the smoothness setting between Rough, Medium, or Finish. Each of these options represents a set of values for feed acceleration and deceleration.

The Rough option uses the least restrictive values to decelerate faster into corners, change direction more quickly, and accelerate faster out of corners to reduce cycle time, at the expense of part finish and machine accuracy. Use this option to rough out a part, or to decrease cycle times when part finish and accuracy are not critical.

The Medium option uses the machine’s default values.

The Finish option uses the most restrictive values to decelerate more slowly into corners, change directions more slowly, and accelerate more slowly out of corners to improve finish, at the expense of a longer cycle. Use this option for finish cuts on complicated shapes or when part finish and accuracy are critical.

Helpful Hints

  • You can use G187 to temporarily change the default smoothness in a program. The P address with G187 commands the temporary smoothness level: Command P1 for Rough, P2 for Medium, and P3 for Finish.
  •  More information is available on G187 and Setting 191, or refer to your Operator’s Manual.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.