Denford Software & Machines

How to create G code suitable for a Denford Milling / Routing machine

File extension should be .fnc eg: "My CNC Program.fnc"
Line numbering is allowed but not necessary, eg: N0010 G01 X100 F1000
Metric Code=G21
Inch Code=G20

Typical Head of program:
*********************

{MMINCHCODE}
G90
(Denford Post Output - Created by XXXXXXX
(Date: {DATE}
(Time: {TIME}
(Source File: {SOURCEFILE}
[BILLET X{BILLET0} Y{BILLET1} Z{BILLET2}
[EDGEMOVE X0 Y0
G91 G28 X0 Y0 Z0 M05


where {MMINCHCODE} is G21 or G20
{BILLET0} is the simulation billet size in X
{BILLET1} is the simulation billet size in Y ....
( lines are comments to make the program easier to read

Typical end of program:
********************
G0 Z{SAFE HEIGHT}
G91 G28 X0 Y0 Z0 M05
G90
M30


where {SAFE HEIGHT} is normally about +2mm

Toolchange code:
****************

(TOOLDEF T{TOOL} D{TOOLDIAM}
M5
G90 M6 T{TOOL}
M03 S{SPINDLERPM}


Where {TOOL} would be in the format 0101
and (TOOLDEF is only a comment to ensure the correct tool is fitted (usually manual)


Arc Programming:
****************
Denford use Relative centre point programming

G01 X65.000 Y100.000 F1000 ‘ Start point X65 Y100
G03 X135.000 Y100.000 I35.000 J0.000 ‘ a 180 degree arc with X100 Y100 as the centre; X135 Y100 as the final end position


Or simple Radius programming (this method is not ideal for some arcs)

G01 X65.000 Y100.000 F1000 ‘ Start point X65 Y100
G03 X135.000 Y100.000 R35 ‘ a 180 degree 35mm radius arc

Different arc planes can also be defined eg:
G17 G03 X10 Y10 R5
G18 G02 X10 Z10 R5
G19 G03 Y10 Z10 R5



Axes format:
************

In metric programming mode, axis positions can be programmed to 1uM eg: X999.123
In imperial programming mode, axis positions can be programmed to 1thous eg: X999.1234

Speed / Feedrate:
*****************
Denford Milling machines generally have maximums of:
Spindle 4000 RPM; Feed 3000 mm/min

Denford Routing SRP machines generally have maximums of:
Spindle 23000 RPM; Feed 5000 mm/min



Example Program (see dimensioned drawing of the two boxes)
***************************************************

G21
G90
(Denford Post Output - QuickCAM 2D Design Ver: 1.8.5.343
(Date: 10/01/2008
(Time: 10:43:35
(Source File: Untitled.fnc
[BILLET X110.000 Y105.000 Z10.000
[EDGEMOVE X0 Y0
G91 G28 X0 Y0 Z0 M05
(Machine: ROUTER 2600 PRO
(Material: Foam / Balsa
[TOOLDEF T0101 D0
M5
G90 M6 T0101
M03 S23000
(Follow 1.000mm Deep - T1 6.000mm Diam.
G00 X1.614 Y1.321
G00 Z2.000
G01 Z-1.000 F1250.0
G17
G2 X0.000 Y5.000 I3.386 J3.679 F5000.0
G01 Y40.000
G2 X5.000 Y45.000 I5.000 J0.000
G01 X40.000
G2 X45.000 Y40.000 I0.000 J-5.000
G01 Y5.000
G2 X40.000 Y0.000 I-5.000 J0.000
G01 X5.000 Y0.000
G2 X1.614 Y1.321 I0.000 J5.000
G00 Z2.000
[TOOLDEF T0202 D0
M5
G90 M6 T0202
M03 S23000
(Follow 2.000mm Deep - T2 1.500mm Diam.
G00 X53.227 Y52.643
G00 Z2.000
G01 Z-2.000 F1250.0
G2 X50.000 Y60.000 I6.773 J7.357 F5000.0
G01 Y90.000
G2 X60.000 Y100.000 I10.000 J0.000
G01 X90.000
G2 X100.000 Y90.000 I0.000 J-10.000
G01 Y60.000
G2 X90.000 Y50.000 I-10.000 J0.000
G01 X60.000
G2 X53.227 Y52.643 I0.000 J10.000
G00 Z2.000
G0 Z2.000
G91 G28 X0 Y0 Z0 M05
G90
M30

Does this instruction work for a 1990 Starmill ATC?

How is this instructions for making a post processor? This is directions for creating G-code. A post processor is used in programs like mastercam to create G-code. What I do need is directions for making a post-processor to use in mastercam and Autodesk Inventor to create my g-code. Thank you!

clarkbd wrote:How is this instructions for making a post processor? This is directions for creating G-code. A post processor is used in programs like mastercam to create G-code. What I do need is directions for making a post-processor to use in mastercam and Autodesk Inventor to create my g-code. Thank you!

Nobody said that these are instructions for making a post processor, as how you produce a post processor depends on what CAM software you'll be using.
What it is though, is telling you what format the G-code has to be in, to be compatible with Denford software.

However, I'd try a basic Fanuc post processor. Failing that, a Mach 3 milling post may also work.
And having just searched the Autodesk Post library, there are a couple listed for Denford - http://cam.autodesk.com/posts/