High-Speed Machining

Introduction

High-Speed Machining (HSM) is an optional software feature on Haas mills with software version M10.07F or higher. By the end of this module, you must understand:
  1. Machine requirements
  2. How HSM works
  3. HSM operation
  4. Necessary parameters and settings

Machine Requirements

Between software versions M10.07 and M14.00, this option requires a floating point processor and a software version designated by a "F".

High-Speed Machining (HSM) Overview

What is High Speed Machining?

HSM manages axial deceleration through a unique "look ahead" function that anticipates machine motion. HSM "looks ahead" through the next 80 lines of code.

In traditional machining, it is necessary that the axis motor decelerates at the end of each programmed move. With no ability to look ahead, the machine slows at a consistent rate throughout the program.

With HSM's ability to anticipate upcoming movements, the deceleration rate becomes variable. 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. Wide angle direction changes can thus be negotiated more quickly.

The calculations are done well before the motions. This prevents violation of the acceleration restrictions in the velocity profile during abrupt changes in direction. The greater the change in direction, the lower the velocity must be at the motion transition down to a minimum velocity of zero for a direction change of 90 degrees or greater.

Without HSM, the machine must behave like a race car driver carefully negotiating a brand new course. With HSM, the machine performs like a seasoned race car driver thoroughly familiar with the course.

 

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.

Who benefits from HSM?

Customers that:

  • make complicated parts. They see a reduction of up to 50% in cycle time.
  • make molds.
  • make complicated shapes using ball end mills.
  • run large programs with small linear or circular motion strokes.
  • make complicated 5-axis parts, such as impellers and aerospace parts.

HSM Operation

Remember these two important points:

  • High-speed machining works with smoothly blended shapes where the feedrate can remain high through the blend of one stroke to the next. If there are sharp corners, the control always needs to slow down to accurately make the part.
  • Most programs have sections written with short linear or circular lines of code. The programmed feedrate is decreased in these sections so the machine can make the programmed shape accurately.

1000 Blocks Per Second

The Haas control can process up to 1000 blocks per second (BPS). This means that the control can read and execute up to 1000 lines of code every second, or one line of code each millisecond.

If the program contains more than 1000 blocks, the control must slow down to make the part accurately.

If the program contains more than 1000 blocks, the machine motion can become rough or jerky. This mars the surface finish.

If a customer complains about poor surface finish or rough machine motion, be sure to check the BPS throughput of the program.

1000 BPS Formulas

Both of these formulas use 60,000 because the feedrate is measured in inches per minute. Because the control processes 1000 blocks per second, the formulas use 60,000 blocks per minute (1000 blocks per second x 60 seconds per minute).

  • Maximum feedrate per stroke that will not violate the 1000 BPS processing speed maximum:
    • Maximum inch per minute (IPM) feedrate = stroke length x 60,000
    • Example:
      • Stroke length = 0.0015"
        • 0.0015 x 60,000 = 90 IPM
        • In this example, a stroke length of less than 0.0015" at 90 IPM violates the control's ability to process this stroke.
  • Minimum stroke length required to not violate the 1000 BPS processing speed maximum.
    • Minimum stroke length = feedrate / 60,000
    • Example:
      • Feedrate 150 IPM
        • 150 / 60,000 = 0.0025
        • In this example, a minimum stroke length of less than 0.0025" at 150 IPM violates the control's ability to process this stroke.

80 Blocks of Look Ahead

The Haas control has 80 blocks of "look ahead" when the HSM option is turned on. This means the control constantly reads 80 blocks ahead of the current block.

  • The control uses these 80 blocks of code to calculate how quickly the machine can move through each programmed move.
  • The HSM algorithm always makes sure the machine can decelerate to a stop within the 80 blocks of look ahead.
  • The algorithm can sometimes cause the machine to move slower than the programmed feedrate.
    • Example: while it is most likely the 1000 BPS limit might cause a program with a high feedrate and short linear segments to run more slowly than expected, the 80 block look ahead may also slow it down.

Parameters and Settings

Setting 85, Max Corner Rounding

Setting 85 is a machine motion algorithm. It defines the accuracy of corners within a selected tolerance. But it does not round the corner to the tolerance selected. Use Setting 85 to smooth out the machine motion in corners and make the motion more accurate. At the default value, the amount of corner rounding changes with the feed rate and the input of other parameters. But it is not correct to change more than a few ten thousandth of an inch from the programmed tool path.

  • Setting 85 default value:
    • 0.0050" (0.13 mm) in software versions M11.14 and lower.
    • 0.025" (0.064 mm) in software versions M11.15 and higher.
    .
  • Minimum permitted value: 0.0050" (0.13 mm). Small values in this setting increase the cycle and deceleration times. This can cause the machine to run roughly through the corners.
  • Maximum permitted value: 0.200" (5.08 mm). Large values in this setting decrease cycle time and let the machine flow through the corners with less deceleration.
  • A value of 0 causes the control to act as if the exact stop mode is commanded. We recommend you do not set Setting 85 to 0.
  • Tool recommendations:
    • Ball end mill used to make a complicated shape - 0.100" (2.54 mm)
    • End mill used to make a tight-tolerance press-fit feature - 0.010" (0.25 mm)
  • You can use G187 with an E value to override Setting 85.

Setting 191, Default Smoothness

Setting 191 was added in mill software version M13.14. You can use Setting 191 to change the acceleration and deceleration of the machine around a corner. It applies values to the default set of smoothness parameters used in a delta-V formula. The formula calculates the machine's motion through the corner.

The selections for Setting 191 are ROUGH, MEDIUM, and FINISH. These modes let the operator change the default set of smoothness parameters (Parameters 302, 303, 314, 749, 750, 751, 752, 753, and 754).

  • MEDIUM Mode
    • This is the default mode of operation.
  • ROUGH Mode
    • This setting decreases cycle time and makes faster deceleration into corners, faster direction change, and faster acceleration out of corners.
    • The faster motion can cause finish and accuracy issues.
    • It is best to use this setting where finish is not important.
    • Recommended tool: end mill.
  • FINISH Mode
    • This setting increases cycle time and makes slower deceleration into corners, slower direction changes, and slower acceleration out of corners.
    • The slower motion improves part finish and accuracy.
    • It is best to use this setting where finish is important.
    • Recommended tool: ball end mill.
    • To override Setting 191, use G187 with a P value.

FEED ACCEL Parameters 302, 749, and 752

Setting 191 uses these parameters and G187 Px to change the acceleration and deceleration rate into and out of a corner. This is similar to how a race car driver steps on the brake to enter and on the gas to exit a tight turn.

  • The values in these parameters are set in encoder steps per second, squared.
  • The control uses these values in a delta-V formula to calculate machine motion.
  • Parameter 302, FEED ACCEL MEDIUM was introduced in mill software version M10.07, with HSM.
  • Parameter 749, FEED ACCEL ROUGH was introduced in mill software version M13.14, with Setting 191.
  • Parameter 752, FEED ACCEL FINISH was introduced in mill software version M13.14, with Setting 191.
caution: Be careful when you change these parameters. Make sure you know the effect.

FEED T CONST Parameters 303, 750, and 753

Setting 191 uses these parameters and G187 Px to change the deceleration and acceleration distance (time) into and out of a corner. This is similar to how long it takes a race car driver to decelerate into a tight turn, and how long it takes him to accelerate out of it.

  • The values in these parameters are set in milliseconds.
  • The control uses these values in a delta-V formula to calculate machine motion.
  • Do not set this parameter below 3.
  • Do not set this parameter above 6.
  • Parameter 303 FEED T CONST MEDIUM, was introduced in mill software version M10.07 with HSM.
  • Parameter 750, FEED T CONST ROUGH, was introduced in mill software M13.14 with Setting 191.
  • Parameter 753, FEED T CONST FINISH, was introduced in mill software M13.14 with Setting 191.
caution: Be careful when you change these parameters. Make sure you know the effect.

FEED DELTA V Parameters 314, 751, and 754

Setting 191 uses these parameters and G187 Px to change the maximum change in velocity while moving through a corner, similar to speed at which a race car driver takes his car around a tight turn.

  • The values in these parameters are set in encoder steps.
  • The control uses these values in a delta-V formula to calculate machine motion.
  • Parameter 314, Feed Delta V Medium, was introduced in mill software version M10.07 with HSM.
  • Parameter 751, Feed Delta V Rough, was introduced in mill software M13.14 with Setting 191.
  • Parameter 754, Feed Delta V Finish, was introduced in mill software M13.14 with Setting 191.
caution: Be careful when you change these parameters. Make sure you know the effect.

Parameter 315: 4 High Speed Machining needs to be set to 1 to turn on this option. This parameter requires an authorization code.

Menu Category: 

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.