Verification: 937b329de42152d7

Friday, October 1, 2021

Simulating with Millplus IT PC software, nerd level 1000

Simulating with Millplus IT PC-software, WinXP only

=>nerd-level 1000<=


There is a simulation/computer software for the millplus IT v530.

It use to be on the webpage when it was alive.

It's a freeware without saving capability. Ask, I may give it away.

so for the closest mourners, simulate millplus on a PC

A video of some demo I made few years back:

Use a virtual machine with winxp, install the millplus software.

Without a physical Dongle, no saving is permitted.

Theres possibility to sideload a CNC-program, and simulate it.

You can make your own program in ISO and IPP, but not save.

Use the overlay-file to see the machine-button-command.

Menu items are in the upper gray field click to open, but the are not clickeble in its own, use arrow keys on the keybord, enter to chose



You need to run the reference point before anything can be done, by clicking the ”all axis”-button.

Start cycle with CTRL+F8

Now the machine is ready to use.

Place a millplus compatibility CNC-program in the Work-folder,

Open the program in the same manner you do in the real machine

You may edit and program, but, no saving!


Running a simulation.


When you are in the machining view, chose your program to load it. tap the menu row, and move with arrow-key

You can run the CNC-program here, but the syncron graphic is zoomed out too much to make a good  use, more on this later

Go to the Menu-field, use arrows to go to graphics, point down to wire plot, enter

Now you can start the machining by use CTRL+F8 (CTRL+F7 to stop, F10 to clear)


You need too fix the zoom level if you don’t use G98/G99 after starting the machining the first time.

The scale is out of bounds, use the scale buttons to get a nicer zoom lever, note, Z is still out, havent figure it out yet

The 2nd time you run the machining it will be watchble.

You can use G98 and G99 to make a workpiece and run it in "full 3D" if needed.

Friday, May 21, 2021

Internal keyway in CNC lathe, programming help

 My post on internal key way was removed by blogger (google), check mail at the end

Broaching in CNC-lathe

 The simple way to make an internal slot in your CNC-lathe

You need to get or make the tool, it's not included.


An example of tools

Broaching tool

I read a lot of tutorials on how to broach slots, everyone is parametric, with R-values, and so on, and I thought, can you do this easy?.

My solution so far, the main program and a sub-program, some inc programming, and we're there


N10 G54


N30 WORKPIECE(,,,"PIPE",256,0,-35,-30,70,30)

N40 T="PLUNGE_CUTTER_3P" ;zero Z at center of tool

N50 G96 S10 M5 ;not the best "no rotation" command

N60 G94 F300 ;feed mm/min

N70 G0 X30 Z2 ;startpos

N80 KILSUB P10  ;subprogram, P=repetition times (how deep you go)

N90 G0 G53 X500 Z600 D0

N100 M30

and the sub:

N10 G54 ;just in case

N20 G91 X0.3 ;inc cut/sub run, aka cutting depth

N30 G90 ;abs prog

N40 G1 Z-20 ;depth in Z

N51 g0 Z2 ;return of tool

N60 m17 ;exit sub

Things that have a deep impact, the P-value is the cutting depth x how many repetitions needed.

something's not completely finished, never tried this for real, just couch-programming

now for the big techs small people bullying:



     As you may know, our Community Guidelines 
( describe the boundaries for what we 
allow-- and don't allow-- on Blogger. Your post titled "Broaching in 
CNC-lathe" was flagged to us for review. We have determined that it 
violates our guidelines and deleted the post, previously at

     Why was your blog post deleted?
     Your content has violated our Malware and Viruses policy. Please visit 
our Community Guidelines page linked in this email to learn more.

     We encourage you to review the full content of your blog posts to make 
sure they are in line with our standards as additional violations could 
result in termination of your blog.

     For more information, please review the following resources:

     Terms of Service:
     Blogger Community Guidelines:


Tuesday, December 8, 2020

NX, right plane (CSYS) from the start, manufacturing

Get the machine zero secure in NX

a disclaimer may just be in an earlier version of NX, in NX7.5 this is this for real  

NX can be a jerk if you do manufacturing on a workpiece where the CSYS (model zero) are "misplaced"
If you going to avoid that, make the model zero correct for manufacturing from start.
applies for both mill and turn (more on turn below)
check the video

BUT,(maybe an old prob, NX 7.5 do this, can't make it in NX11 now for some reason)
 revolved turning model workpiece work a little different, you should do your model with X as the center axis (usually Z). When you enter manufacturing, like magic, it transforms to Z as it should be....
If you will start with a model with the Z-axis as i "should be" good luck, you got manufacturing with X as center axis, totally wrong and hard to fix at this level. Can do more on that, ask!

Correct me down below if I did a bobo

Wednesday, October 14, 2020

Engraving on mantle surface on a round detail Siemens Sinumerik 840D sl


Engraving on the radius surface on a round detail


Prerequisites in the program is adapted to TRACYL execution:


The simulation program's tool spindle is called 3

The value after TRACYL is the diameter of the part, in this case, diameter 70

The cycle should be run in G19 plane

The zero position of the cycle is changed, e.g. X is the same as Z (depth of milling), then from zero that sits in the center (differ from the pocket cycles there) X1 is cutting depth, Y position on the arc, Z is the same as usual

The simulation shows mirrored text, therefore uses mirror writing

Tool "countersink"

Finished program:

The engraving cycle

Friday, May 8, 2020

thread milling inside or outside without special tools

Want to thread mill?
do not got the mill tool?
got a lathe/turning machine?
with a smaller thread turn tool, a boring tool actually.
This tool needs to be a tool for internal lathe, and then we go

as always, show the pic of the tool, this one is from, othervise sandvik
month the tool in you mill chuck and you're on the go

The tool on the pic is the (only) tool you need

we are going to show how to do it in sinutrain 4.7 (4.07) and cycles.
check the video after the instructions..

Chose an internal tool, called ..:

Threading tool is an option in sinutrain, use that, if you do not know sinutrain, check my other videos.

check the video for the rest, ask by mail for everything else

This work inside and outside, cool or what?


Thursday, February 27, 2020

Heidenhain Millplus IT and Tilting the coordinate system in autodesk Fusion 360 CAM with G7

Tilting the coordinate system in Autodesk Fusion 360 CAM with use of G7
Heidenhain iTNC530 should be on the same principle as Cycle 19

In the CAM-system, when you are about to tilt the work plane for 4-5 axis machining, you need to use the right tool-coordinate system to make this work.
I use this rule to tilt the coordinate system:

(Right-hand rule for axis orientation and direction. (R. Hewitt,

The G7-code in this machine has 3 axis to tilt around  A5, B5 and C5 as X, Y and Z axis, in that order and that make A5 to mill on the Yside, B5 to mill on the Xside and C5 as Zside (damn that's weird..)

(From the millplus IT Ver 5.20 manual)

As mentioned in an earlier post about tilting  the sides have different coordinate systems.
In this case, we will use A5=90, A5=-90 for the Y sides, B5=90 and B5=-90 for the X sides to cover all the sides

All the facts of the CAM in fusion:
Use the pen-shaped button on the upper left.
Find setup1 and setup1 again and the 4 drilling operations but you will not see the tool coordinate system, only the tiny marking for the tool position, Download and use your Fusion 360-program to check this out
We have now a totally 5 coordinate system to juggle with, nice..

The CNC-code:

N1001 (1001)
N10 (T1  D=10 CR=0 TAPER=118deg - drill)
N11 G90
N12 G94
N13 G17
N14 G71
N15 G99 X-10 Y-10 Z-61 I72 J72 K71
N16 G98 X0 Y0 Z-51 I52 J52 K51
N17 G74 Z0 L1
N18 (Drill1)
N19 T1 M6
N20 S5000 M3
N21 G54
N22 G7 A5=0. B5=-90. C5=0. L1=1
N23 M8
N24 G0 X-17.351 Y26.224
N25 G0 Z15
N26 G17
N27 G0
N28 G0 Z5
N29 G81 Z-5 Y5 B1 F1000
N30 G79 X-17.351 Y26.224 Z-1
N31 G0 Z15
N32 G74 Z0 L1
N33 (Drill2)
N34 G7 A5=90. B5=0. C5=0. L1=1
N35 G0 X25.112 Y-14.595
N36 G0 Z15
N37 G0
N38 G0 Z5
N39 G81 Z-5 Y5 B1 F1000
N40 G79 X25.112 Y-14.595 Z-1
N41 G0 Z15
N42 G74 Z0 L1
N43 (Drill3)
N44 G7 A5=0. B5=90. C5=0. L1=1
N45 G0 X17.687 Y24.823
N46 G0 Z67
N47 G0
N48 G0 Z57
N49 G81 Z-5 Y5 B1 F1000
N50 G79 X17.687 Y24.823 Z51
N51 G0 Z67
N52 G74 Z0 L1
N53 (Drill4)
N54 G7 A5=-90. B5=0. C5=0. L1=1
N55 G0 X24.699 Y18.413
N56 G0 Z67
N57 G0
N58 G0 Z57
N59 G81 Z-5 Y5 B1 F1000
N60 G79 X24.699 Y18.413 Z51
N61 G0 Z67
N62 M9
N63 G74 Z0 L1
N64 G7 L1=1
N65 M30
(my G74 needs to be Z-10 to work)

Every G7 has one active value if you'd choose the correct coordinate system when Fusion 360 posts the code.

This video shows how your choice should be done. Take note of how the coordinate arrows are placed on the tool

Back to the CNC-code then. I did a test of the code, it works the way I like it to work. There may be a lot of other ways to do this, I'm not an expert at all, I'm a noob on this, just started.

We will check the video out, I didn't use a proper workpiece ant tool for this, just something as a reference. The height depends of the lack of proper fixture for this type of machining in my DMG DMU80T.
Often, I do not use an edge finder and a bottle of windows cleaner when I'm milling, trust me on that :)

This was not a completely linear description of the solution, but some input on how to do it.
I needed to get this on paper for my own sake, hope anyone else can learn from it.
Comment below if something is wrong, smart, stupid or anything...



Tuesday, May 14, 2019

Drill/mill on the diametric part of the workpiece in Lathe (tracyl) Siemens 840D sl

Drill on the diametric part of the lathe workpiece(G19)
How it’s done,
Y Rotation (Much more on this later)
Z Distance in longitudinal (standard Lathe Z direction)
X depth (Diameter-dimensions).
Starting codes:
Besides the usual...
SETMS (1.. 4); The number of the driven spindle
TRACYL (50); Choice of machining on the diametric surface and diameter of the workpiece

Y will be the length of the diametric surface in mm or inch. (the rotation)
For example, if you have a diameter of 50mm, work out the perimeter and use these dimensions, 50xPi = 157,07963267948966192313216916398
This represents a whole 360 deg turn, use this for suitable split values between holes.
Example of 4 holes around a 50 detail

N41 SETMS (3) (Enable driven tool, the number may vary)
N42 TRACYL (50) (Enable milling diametric surface, dia 50)
N50 G97 S2000 F100 M3
N60 G0 X55 Y0 Z-20 (starting hole at 0 degrees)
N70 G1 X45 (drilling)
N80 G0 X55
N90 G0 Y 39.269908169872415480783042290994 (90-degree hole)
N100 G1 X45 (drilling)
N110 IS G0 X55
N120 G0 Y 78.539816339744830961566084581988 (180-degree hole)
N130 G1 X45 (drilling)
N140 G0 X55
N150 G0 Y 117.80972450961724644234912687298 (270-degree hole)
N160 G1 X45 (drilling)
N170 ................
SETMS (1) (Switch to the main spindle)
TRAFOOF (return to normal turning)