First use of the polar co-ordinate interpolation function (TRANSMIT function)

Polar coordinate interpolations are programmed in a Cartesian plane (as X, Y coordinates). The machine only executes movements by combining a C axis with an X axis.
Swiss type machine high precision turning numerically controlled machine cam machine tools single spindles monospindles multiple spindles multispindles high precision parts lathes NC numerically controlled multi-spindles lathe multispindles machining

Tips and Tricks

First use of the polar co-ordinate
interpolation function (TRANSMIT function)

Compatibility :
all DECO

Technology

• PNC
• TB-DECO
• Software Hotline
• Tips and Tricks

ISO code for the milling operation :
1.	G1 X3=35 Z3=-4 G100 T31 G94
2.	M198 D-1
3.	G1 C1=-18 G100 (PREPARING G42 CONTOURING)
4.	G1 X3=14 C1=-18 F200 G42 G81
5.	G1 X3=14 C1=7
6.	G1 X3=-14 C1=7
7.	G1 X3=-14 C1=-7
8.	G1 X3=14 C1=-7
9.	G1 X3=14 C1=18 (PREPARING G40 EXIT)
10.	G1 X3=35 C1=18 G100 G40
11.	G1 C1=0 G100
12.	M199

Description:
Polar coordinate interpolations are programmed in a Cartesian plane (as X, Y coordinates). The machine only executes movements by combining a C axis with an X axis.

We shall now look at two possible applications of this function:

Number 7 (Dec.98):Milling a square with T31 and end-milling Ø 10

Number 8 (March 99):Milling a square with a circular miller, ø80 mounted on a polygon unit

Use :

The optional parameter D of function M198/M498 is used with value -1.
To activate the polar coordinate mode: M198 D-1.
To deactivate the polar coordinate mode: M199

The operating line containing the M198 D-1 code to execute polar coordinate machining, must comprise axis X as master 1, axis C as master 2 and the third axis (e.g. Z) as the slave.

The first master axis must be an axis with a diameter (X2, X3 or X4).

Milling a square with T31 and end-milling Ø 10

We want to mill the following square shape :

By switching to polar coordinate mode (M198 D-1), axes X and C are now defined as follows :

The part datum is located at the centre of the bar undergoing machining. Absolute coordinates at X and C of points 1 to 4 :

Point	X	C
1	14	7
2	-14	7
3	-14	-7
4	14	-7

In SINGLE mode the result is as follows :

Programmed path.

Path from the centre of the miller
(corrected by G42).

The numbers identify the contour points corresponding to the line numbers of the above ISO code.

THINK PARTS THINK TORNOS

Home Company Applications Products Technology Investor News Contacts Download Site Map

TORNOS SA
Rue Industrielle 111
CH-2740 Moutier
Switzerland

Tel.: +41 (0)32 494-4444
Fax: +41 (0)32 494-4903
www.tornos.com

ENGLISH
FRANÇAIS
DEUTSCH