Mitsubishi M80 Mold Machining Settings: SSS Control, Machining Condition Selection I and the Three Application Packages

Most operators running dies and moulds on a Mitsubishi machine ask the same question: “Does our machine have the mould package, and how do I turn it on?” The name has stuck on the shop floor, but there is no single heading called Mould Package or Mold Package in the official Mitsubishi manual, and no single parameter that switches it on.

On the M80 control this job is done by two separate structures working together. This page explains both in plain operator language, with the parameter numbers and in the order you would actually follow at the machine.

What is the “mould package” actually called on the M80?

The manual covers this subject under two headings:

1. Machining Condition Selection I: parameter groups that store ready-made machining settings as packages.
2. High-speed High-accuracy Control: machining modes called from inside the part program with a G code.

On top of these sit the functions that improve surface quality:

• SSS Control (Super Smooth Surface control)
• Easy SSS
• Fairing
• Smooth Fairing
• Corner deceleration
• Arc and contour accuracy settings

So “turning on the mould package” is not a single keystroke. First you confirm the option is actually installed, then you grant the permission parameter, then you enable SSS, and finally you call the machining mode from the program.

Which controls does this guide apply to?

The parameter numbers and explanations on this page are based on the Mitsubishi M800 / M80 / E80 series Alarm and Parameter Manual. The same logic applies to the M800V and M80V series, but some ranges and options differ with the CNC software version.

Important: Always confirm parameter numbers and value ranges against your own machine’s manual. Mitsubishi manuals are written as if every option were installed; on your machine a given function may not have been purchased, or may have been disabled by the machine tool builder.

How many mould machining packages does the M80 have?

Two different “threes” get mixed up here. They are not the same thing.

1. Machining condition application packages: three of them

The M80 parameter manual provides three separate application parameter groups for Machining Condition Selection I. All three consist of exactly the same parameters; only the numbers shift.

The manual does not force the names roughing, semi-finishing, finishing on these three groups. That naming is done by the machine builder or the user. The most common arrangement in the field is:

• Application 1: Roughing
• Application 2: Semi-finishing
• Application 3: Precision finishing

This is only a suggested arrangement, not a fixed Mitsubishi factory definition. On your machine the builder may just as well have set the groups up as speed / standard / accuracy.

2. High-speed high-accuracy machining modes: three of them

These are not parameter packages. They are machining control modes called from inside the program with a G code.

Control II and Control III cannot be used at the same time. For mould finishing the most widely used mode is G05 P10000, that is Control II.

How is the mould package activated?

Check one: is the function really on the machine?

Do not simply put G05 P10000 at the head of a mould program and run it. Check first whether the option exists, using a low-risk test program.

%
O9001
G21 G17 G40 G49 G80 G90
G05 P10000
G05 P0
M30
%

There is no axis motion in this program. It only tries to open and close the mode. Even so, run a graphic check before executing it.

• If the program finishes without an alarm: Control II is most likely available on the machine.
• If a “No specification”, “No spec” or similar specification alarm appears at the G05 P10000 block: the function may not be installed on your machine.

To be clear about this: an option that has not been purchased or licensed cannot be unlocked by changing a parameter. In that case the only route is the machine tool builder or Mitsubishi CNC service. The “set this parameter to 1 and it opens” advice found on forums does not work for this.

Check two: #8040 High-SpeedAcc

The part system in which high-speed high-accuracy control will be used has to be permitted by this parameter.

According to the manual this value can be set to 1 for a maximum of two part systems. Setting it to 1 for three or more part systems can trigger alarm Y51 0032.

On a standard single-part-system vertical machining centre only the first system is normally checked. This parameter does not make the option purchased; it only defines which part system may use an option that already exists.

Check three: #8090 SSS ON

This is the main user parameter that enables SSS control.

• 0: SSS / Easy SSS disabled
• 1: SSS / Easy SSS enabled

Inside the Machining Condition Selection application groups this parameter has its own in-package equivalents:

In other words, SSS can be switched on and off separately in each package. For a die maker who does not need SSS in roughing but wants it in finishing, a starting arrangement could look like this:

Application 1 / Roughing       : #42016 = 0
Application 2 / Semi-finishing : #42316 = 1
Application 3 / Finishing      : #42616 = 1

This is an example starting arrangement only. The real values for a given machine must be determined from its dynamic behaviour.

Parameters inside the three machining packages

Every Application group contains the same kind of parameters, with the numbers shifted. Use the table below as a road map at the machine.

This structure allows three different machining characteristics to be stored on the same machine and called according to the part type.

What does each parameter do?

#42001 / #42301 / #42601 – G1btL time constant

Affects acceleration and deceleration behaviour during cutting motion.

• Setting range: 0 to 5000 ms on a normal system
• With the time constant expansion function: 0 to 30000 ms

Increase it: the axis accelerates and decelerates more gently. Vibration can drop, but cycle time gets longer.
Decrease it: motion becomes brisker. If the machine is not rigid enough, vibration and surface marks can increase.

#42002 / #42302 / #42602 – SfiltG1 soft filter

The soft acceleration and deceleration filter for G01 cutting motion. Setting range 0 to 200 ms.

Increase it: speed changes become smoother and the surface can come out cleaner.
Increase it too far: the machine slows down more than necessary on small details and sharp corners start to round off.

#42003 / #42303 / #42603 – Sfilt2 second filter

The second soft acceleration and deceleration filter. Setting range 0 to 50 ms.

It helps motion stay smooth on mould surfaces where short CAM blocks follow one another. If you see a wavy pattern on free-form surfaces, this is one of the parameters to look at.

#42004 / #42304 / #42604 – R COMP general accuracy coefficient

Setting range 0 to 99 %. This value is only effective when #8021 COMP_CHANGE = 0.

It governs the balance between accuracy and speed on arcs and contour transitions. The manual states that this parameter is equivalent to #8019 R COMP.

#42005 and #42006 – Corner and curve accuracy

Setting range -1000 to 99 %. These parameters are used when #8021 COMP_CHANGE = 1.

• cor_comp: accuracy behaviour at corners. Base equivalent #8022 CORNER COMP.
• cur_comp: accuracy behaviour on curves and arcs. Base equivalent #8023 CURVE COMP.

A practical rule of thumb: if the size drifts at sharp corners look at cor_comp; if deviation appears on radiused transitions and free-form surfaces look at cur_comp.

#42007 / #42307 / #42607 – Feed forward gain

Setting range 0 to 200 %. This is the control value that affects how closely the axis follows the commanded path. The manual states that this field corresponds to #2010 fwd_g.

This is not an operator setting. A wrong value can cause:

• Axis vibration
• Humming and abnormal servo noise
• Marks at corners
• Surface degradation
• Servo instability

It should not be changed without knowing the value set by the machine tool builder.

#42008 / #42308 / #42608 – Corner deceleration angle

Setting range 0 to 89 degrees. It defines from which angle the CNC treats a direction change as a corner and applies deceleration. Base equivalent #8020 DCC ANGLE.

Decrease it: even gentle angles count as corners, the machine decelerates more often, accuracy improves but cycle time grows.
Increase it: only sharp direction changes cause deceleration, cycle time drops but the risk of corner overrun increases.

#42009 / #42309 / #42609 – Cancel angle

Setting range 0 to 180 degrees. It defines one of the angle evaluation behaviours inside accuracy control. It is the in-package equivalent of #8026 CANCEL ANG.

#42010 and #42011 – Chord error tolerances

Setting range 0.000 to 100.000 mm. These define the maximum chord error accepted on contours that CAM has broken into short linear segments.

• First value: for blocks containing an inflection
• Second value: for blocks without an inflection
• If 0.000 is entered: the block concerned is treated as linear

The manual refers to roughly 10 microns, that is 0.010 mm, as a normal example.

Too small a value: surface accuracy improves, but corners decelerate more and machining time grows.
Too large a value: the machine speeds up, but the fine detail produced by CAM starts to round off.

#42012 / #42312 / #42612 – Fine segment length

Setting range -1 to 127 mm. When a block length in the CAM program exceeds this value, spline processing is temporarily dropped and the control switches to linear interpolation.

• -1: spline processing independent of block length
• Other values: evaluation according to block length

The manual notes that the value can be chosen slightly smaller than the single block length in the program.

#42013 / #42313 / #42613 – Fairing selection

Base equivalent #8033 Fairing ON. The options in the manual are:

• 0: Fairing and Smooth Fairing not used
• 1: Fairing used
• 2: Smooth Fairing used

Fairing aims to smooth the motion between consecutive short CAM blocks. On mould surfaces it can reduce toolpath marks and abrupt speed changes.

Point to watch: in the application group tables this line is shown with a 0/1 range in some printings, while the base #8033 description lists options 0, 1 and 2. For that reason, confirm the availability of option 2 (Smooth Fairing) against your CNC software version and machine specification.

#42014 / #42314 / #42614 – Fairing length

Setting range 0 to 100.000 mm. It defines the block length to which fairing is applied and is only meaningful while fairing is enabled. Base equivalent #8029 FairingL.

#42015 / #42315 / #42615 – Corner judgement length

Setting range 0 to 99999.999 mm. This is the length that determines which small blocks the CNC will disregard when judging corners. Base equivalent #8037 CorJudgeL, used when #8036 CordecJudge = 1.

#42017 / #42317 / #42617 – Standard length

Setting range 0 to 100.000 mm. The standard length value SSS control uses for shape recognition and motion evaluation. Base equivalent #8091 StdLength.

#42018 / #42318 / #42618 – Step width

Setting range -1.000 to 0.100 mm. The width value used when evaluating steps or small geometric changes in machining condition selection. Base equivalent #8093 StepLeng.

#42019 / #42319 / #42619 – Package tolerance

Setting range 0 to 100.000 mm. The tolerance value of the machining condition parameter group. Base equivalent #2659 tolerance.

#42020 / #42320 / #42620 – Maximum machining speed

Setting range 1 to 1,000,000 mm/min. It defines the maximum cutting feedrate permitted in that package. Base equivalent #1206 G1bF.

Entering a value above the machine’s physical capability does not mean the machine can actually cut safely and accurately at that speed. This field is an upper limit, not a target.

#42021 / #42321 / #42621 – Tolerance control filter

The filter setting that comes into play during tolerance control. Because the behaviour of this line can change with the CNC software version, confirm its value against your machine’s parameter manual.

How does the operator apply this at the machine?

1. Back up the current parameters

Before any change:

• Take a CNC parameter backup
• Record the current values in Applications 1, 2 and 3
• Photograph the screens
• Keep the machine builder’s factory setting list

Mitsubishi specifically warns that changing parameters in large quantities can make operation unstable, and asks that unused bits be left at 0.

2. Check the parameter write permission

If parameter editing is blocked on the M80 screen, one of these may be active:

• User level
• Parameter lock
• PLC lock
• Machine builder password
• Edit lock

Do not try to remove that protection at random. An area locked by the machine tool builder is not an operator setting.

3. Study the packages before changing anything

Search for these numbers on the parameter screen and compare the current values of the three groups:

#42001 - #42021
#42301 - #42321
#42601 - #42621

The differences between them tell you how the builder set each group up. For example, if one group has a noticeably larger time constant and a looser tolerance, that group is most likely intended for roughing.

4. Do not invent a package from scratch

The Mitsubishi manual explains what the parameters do and gives their valid ranges, but it does not provide a ready, universal value table for every machine. The correct values depend on:

• Rigidity of the machine structure
• Servo motor and drive configuration
• Ball screw pitch
• Guideway type
• Table and workpiece weight
• Axis accelerations
• Spindle speed
• Tool overhang
• CAM tolerance
• Workpiece material

For that reason, saying “enter these values on every machine for the M80 mould package” is technically wrong.

5. Open the mode inside the machining program

If Control II is available, G05 P10000 is placed before the three-dimensional mould machining section and G05 P0 after it.

%
O1000
G21 G17 G40 G49 G80 G90
T10 M06
G54
S12000 M03
G00 X0 Y0
G43 H10 Z50.
G05 P10000
G00 Z5.
G01 Z-1. F500
(3D MOULD TOOLPATH)
X...
Y...
Z...
G05 P0
G00 Z100.
M05
M30
%

For the other modes:

• Control I: opened with G05.1 Q1, closed with G05.1 Q0
• Control III: opened with G05 P20000, closed with G05 P0

Do not leave the high-accuracy mode wrapped around tool changes, rapid positioning and safe retract blocks. Opening and closing the mode so that it covers only the actual surface machining section is the cleanest practice.

6. Make the first trial a safe one

A new setting should not be tried directly on a real mould. In order:

1. Run a graphic check of the program
2. Perform a safe dry run without tool and workpiece
3. Keep rapid override low
4. Check the first moves in Single Block
5. Run a surface test on a soft trial material
6. Compare time and surface on the same toolpath
7. Listen to servo noise and watch for axis vibration

Can ready-made starting values be given?

The answer that stays faithful to the source: no.

The Mitsubishi parameter manual gives the parameter numbers, their functions, their equivalents and the permitted value ranges. It does not give a definite value for a roughing package, a definite value for semi-finishing, or a definite value for finishing.

Without the machine builder’s own setting table, no definite value should be recommended for these in particular:

• Feed forward gain
• G01 time constant
• Soft filters
• Corner and curve compensations
• Maximum axis speed
• All servo related parameters

Common mistakes

Short summary for the operator

On the Mitsubishi M80 there is no single activation parameter called “mould package”. The mould machining system is made up of these parts:

• Three separate Machining Condition Application groups: #42001-#42021, #42301-#42321, #42601-#42621
• SSS control: #8090, and #42016 / #42316 / #42616 inside the packages
• High-speed High-accuracy Control: Type I G05.1 Q1, Type II G05 P10000, Type III G05 P20000
• Permission to work together: #8040 High-SpeedAcc

If the function is not present on the machine as a purchased option, it cannot be unlocked by changing parameters alone. Servo, filter and accuracy values should not be altered before the existing parameters are backed up and the machine builder’s values are known.

Safety warning and disclaimer

The parameter numbers, value ranges and G codes on this page are based on official Mitsubishi M800 / M80 / E80 series manual information. However, parameter numbers, valid ranges and function behaviour can differ with the CNC software version, the series and the settings made by the machine tool builder. Before applying anything, take your own machine’s parameter and programming manual as the primary reference.

Parameter changes and high-speed machining modes cause physical machine motion. Always take a parameter backup before making changes, test the program first on the graphic screen and in dry run, and make the first cut in single block at a low feedrate. Do not change servo, spindle or safety parameters outside your authorisation.

Mentor CNC cannot be held responsible for tool breakage, part scrap, machine damage or workplace accidents arising from the application of the information on this page. Responsibility rests with the person and the company carrying out the work.