Controls of the Millplus IT

Video showing the functions in millplus
This is a beta test, need lots of editing

The machine controller is MILLPLUS V500/510

The machine is fully ISO/DIN based

There is a simulator to download to this control system

Screen Layout

Red field: Modes of operation

Yellow field: Axis values on the left, residual to Right

Green field: Function buttons with dependency On operating mode

White field: Tool Changer Mechanism

Blue bar: Information button to display alarm and so on

Keyboard

Yellow field : Selecting the operating modes

Blue Bar : Cooling Water

Purple fields : Program Start/Stop

Black Field : Top control fast feed, bottom control Work Feed

Pink Field : Manual Shaft Movement

Light blue Bar : Open Door

Keyboard is used for text input and to introduce values to the control

Machine axes and movement

As usual, X Y and Z are just like on any other machine, however, there are two new axes, B and C.

B is the rotary milling axis of the mill head, values from B-32 to B1. 5 (With M57, -90 deg)

C is rotary milling axis of the table 0-360 degrees

Start the machine

Main switch on

Release the Emergency Stop switch

Press (Hold button), and CLEAR (F10)

Before you can use the machine, the reference point must be run

Select the button below, make sure the door is closed, the machine announces closed door with a small beep

The button text is in swedish but I think you got the message (hey, you understand swedish? cool)

Run the Cycle Start button (the green one)

Manual operation of Machine axes

All axes can be manually run in MDI mode.

The different axis drawings are shown below

1. Z-axle	2	Y-axle
3 X-axle	4 Axle 4
5 Axle 5	6	S Rapid feed

Programming

Select Edit with the menu button

In the folder tree, select Folders.

New program: Enter number. PM to load a new program

Open existing: Select applications and press ENTER on the Keyboard

Program in ISO Code

The first line shall be the program number starting with N

The control keeps track of codes for You

If you want to know the usual M and G codes the system uses, press the (I) button

The whole line you edit is blue marked, but in the blue marked there is a _ that show where you type

Programing exemple

Programming exemple with explanations

N111 (program name

N1 G17 Choice of PLAN)

N2 G54 I90 (Zero point, I is the index)

N3 T12 M6

N4 S1500 M3

N5 M7 (int cooling)

N4 G0 X20 Y40 Z60

N5 G1 Z50

N6 G0 Z100

N8 M30

The machine does not allow two M-codes and G-codes in the same block

axis of rotation of the table is called C and programmed in, for example, C180, C0 is always at exactly the same point

Shaft for turning the cutter head is called B and can be angled 35deg as standard in one direction and 1.5 degrees in the other. Example B-35

But if you use M57 you can turn the mill head to -90deg

There are a large number of special G-codes that can be used for various features of the run, however, there are so many, G stretch up to G700-someting, please read the manual (700 pages) There is also a programming support that help helps you create Runs, check out the Programming manual for that information (I can give you a copy)

Zero-point setting

The zero-point table, G54, has lots of valuse according to the table zero points. These are denoted by I (ex G54 I5)

Set your own zero point :

Start by typing G54 Ix in (the number you want to use) In MDI and press run to select G54

After that, select the Zeropoint button that is available when you press the drive Mode button.

Then you stand in the position that is O and Zero there by putting values in the axis fields

Push

Touch the workpiece with a tool do add the radius before NPF

Zero point register have values for both B and C axis

Running the program

Choose the run mode

Choose your program in the file manager

Programmet is ready to go

Press Cycle start (yellow)

Note that you got two feed rate knobs, the upper for rapid and the lower for working feed

Tool change

Moving the control panel to the left side of the machine behind a transparent door are the tools.

Rotate the right tool with the button in the picture, you get the choice over which direction you want to rotate and which switches the discs you intend to use

The tool that can be replaced is what sits in the middle of the opening on the corresponding tool changer disc.

The tool is gently broken away from the bracket.

The new tool should be inserted with the Capto track towards the LED!

Click Run mode and the Tool button You must specify the approximate radius and make sure the E-number is not 1 or-1, that parameter should be left unfilled or zero.

G-code for tool-measuring with laser

G601: tool length

G602: tool length and dia

Tool length and dia

Before you use the laser to measure a tool you need to pre-config the tool, add tool radius (R10), the approx tool legnht (L100),amounts of flutes or cutting edges (Q4=4) M3 0or M4 (I2=0)

Addresses from the tool register

Following tool values can be used:

L=Length

L4= overshooting lenght (not needed)

L5= length tolerans

R=Tool radius

R4= overshooting radius (not needed)

E=Tillstånd (0: tool not measured, 1: tool measured, -1: defect tool)

E-number can not be 1 eller -1, This numbre shall be Zero if you are useing laser toll measurment.Thid is needed for the tool brake checking, it checks the tool agaisnt the active value and locks the tool with -1 if the tool differ from old value.you got a error code when running a program if the tool is locked with -1.

When the laser set the value you get a 1 as E-parameter.

Do you measure the tool outside of the machine, just set the E to 1

Edit och menu

If you want to use edit and menu function, you got those on the F-part of the kayboard.

Push the F-button again to exit

IPP

Tryck

If you want to make a pocket, square och circular amongs others you want to use the IPP

You'll find the IPP if you push the programming button again.

You need to have the tool set up before using IPP, the functon needs the tool radius to maske the program

A tip for you are that not choose the deep drilling function in the pocket cycle, Use angel to next, ramping (angel to next…)at approx 15 degrees. (A3, Drilling 0=NO…)

Choose Storet o go forward thru the menus.

Do you miss anything, walk thru all the menuse and go back and edit later

G-function repeat

To repeat part and parts of the program, use G14

Parameters for G14 check the pic below.

Radie path I,J and K

When you use circular interpolation you use I, J och K, those are Absolute, They get their value from The workpiece Zero point

Drilling

The drill cycle need G78 do defiine the drill points, drill cycle G81 för cutting values and G79 for the drilling itself

N50 G78 P1 X50 Y20 Z0 Define point 1

N55 G78 P2 X50 Y80 Z0 Define point 2

N60 G0 Z10 T1 M6

N65 G81 X1.5 Y1 Z-30 F100 S500 M3 Define cycel

N70 G79 P1 P2 drill at point 1 and 2

Simulating

To make a simulaton of your program, push the program running button two times, choose simulate and cycle run button to execute. You will see the tool path and the coordinate system. You get an wievof how the milling will proceed and avoid any expensive craches. The simulating do not show any tool, just the coodinate point

You can add a whole workpiece to your simulating

G98, G99 och G199 is used to define the workpiece

Check the manual or the programming help for this

I've never succeed with simulate real 3D, the hardware is to weak

DRY RUN

you can make the machine to do a dry run for testing puroses. Be in Run, choose F-button to reach menu option and choose dry run DRY RUN in the menu.

Filtransfer

(this may not work on you configuration)

If your machine got lan connection do as follow

You need to find the CNC Data station on the internet for download (hard to find software)

Start the program CDS-on your computer

On hte machine push the diskett-button, choose DATA OUT/IN and Select Device, choose DNC (TCP/IP),click OK. go to the computer ad click reconnect