Creating a post processor for a Denford Mill or Router

Anything to do with configuring CAM systems and Post Processors to run on different CNC machines

Moderators: Martin, Steve, Mr Magoo

Post Reply
User avatar
Denford Admin
Site Admin
Posts: 3632
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Creating a post processor for a Denford Mill or Router

Post by Denford Admin » Thu 10 Jan , 2008 12:30 pm

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
Attachments
PostExampleProgram.JPG
The two boxes produced by the example program.
PostExampleProgram.JPG (39.56 KiB) Viewed 17221 times

MechaBeat
Posts: 1
Joined: Fri 19 Dec , 2014 5:26 am
Hardware/Software: Starmill ATC, 1990
Solidworks
HSMExpress

Re: Creating a post processor for a Denford Mill or Router

Post by MechaBeat » Wed 04 May , 2016 16:10 pm

Does this instruction work for a 1990 Starmill ATC?

clarkbd
Posts: 3
Joined: Wed 07 May , 2014 12:34 pm
Hardware/Software: MasterCAM X7
Denford Microrouter Compact
Techno-Isel LC router

Re: Creating a post processor for a Denford Mill or Router

Post by clarkbd » Mon 19 Dec , 2016 15:26 pm

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!

moray
CNC Apprentice
CNC Apprentice
Posts: 97
Joined: Thu 12 Sep , 2013 20:02 pm
Hardware/Software: Triac VMC

Re: Creating a post processor for a Denford Mill or Router

Post by moray » Tue 26 Dec , 2017 0:03 am

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/

Post Reply