3-D Motion Is Not Smooth

High-Speed Machining (HSM) not Activated

High Speed Machining (HSM) uses a unique "look ahead" function to anticipate machine motion.

In traditional machining, the axis motor must decelerate at the end of each programmed move. Without the ability to look ahead, the machine slows at a consistent rate throughout the program. HSM "looks ahead" through the next 80 lines of code, which lets the control anticipate upcoming movements and vary the deceleration rate. This lets the machine complete the program much more quickly. The control calculates the angle of intersection between the linear and/or the circular motion strokes to maintain the maximum possible velocity through the stroke transition.

The machine can move through wide-angle direction changes more quickly. The greater the change in direction, the slower the machine must go to make the corner, down to a minimum velocity of zero for a direction change of 90 degrees or greater.

HSM Example
  1. Without HSM, the machine decelerates at the same rate at every change in direction, regardless of the width of the angle.
  2. With HSM's unique ability to look ahead in the program, the deceleration is variable. Thus, the part is completed faster.

CAD/CAM Tolerance Settings

The cut tolerance and filtering settings in your CAD/CAM system may produce code that does not leave a smooth surface. The image below shows the same part cut with the only difference being the cut tolerance and filter setting in our CAD/CAD system. Part [1] was cut with a cut tolerance and filter settings that were too large, part [2] was cut with the cut tolerance and filter setting the were much smaller. The tolerance and filter setting to use will vary based on your part requirements and the CAD/CAM system you are using. For more details refer to the Surface Finish Tips section. 

The Program Exceeds 1000 Blocks per Second

The Haas control can process programs at a maximum rate of 1000 blocks per second.

Corrective Action:

If your program commands more than 1000 blocks per second, you may need to use a slower feedrate, or make the XYZ movement of each code block longer.

In your CAM system, increase the Cut Tolerance or Model Tolerance. At a feed of 100 ipm, the shortest distance that each line of code can travel at full speed is 0.0016" (100 / 60000 = 0.0016).

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.

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.

The Program Uses Exact Stops

Exact stops cause the control to completely stop at a programmed position before it processes the next motion block. This is useful in specific circumstances, but it can also cause undesired effects such as shaky motion, faceted cuts, and extended cycle times.

Corrective Actions:

Remove all G09 (EXACT STOP) and G61 (EXACT STOP MODE) commands from your program.

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.