Denford Software & Machines

Denford Software & Machines

 
 

Denford Software & Machines

Welcome to the Denford CAD CAM CNC forum


Hint - Try the google search at the bottom of the page
It is currently Thu 30 Mar , 2017 21:23 pm

All times are UTC [ DST ]




Post new topic Reply to topic  [ 3 posts ] 
Author Message
 Post subject: Creating a post processor for a Denford Mill or Router
PostPosted: Thu 10 Jan , 2008 12:30 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse 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.
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:
File comment: The two boxes produced by the example program.
PostExampleProgram.JPG
PostExampleProgram.JPG [ 39.56 KiB | Viewed 5990 times ]
Top
 Profile  
 
 Post subject: Re: Creating a post processor for a Denford Mill or Router
PostPosted: Wed 04 May , 2016 16:10 pm 
Offline

Joined: Fri 19 Dec , 2014 5:26 am
Posts: 1 Hardware/Software: Starmill ATC, 1990
Solidworks
HSMExpress
Does this instruction work for a 1990 Starmill ATC?


Top
 Profile  
 
 Post subject: Re: Creating a post processor for a Denford Mill or Router
PostPosted: Mon 19 Dec , 2016 15:26 pm 
Offline

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


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 3 posts ] 

All times are UTC [ DST ]


Who is online

Users browsing this forum: No registered users and 2 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
cron
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group
Template made by DEVPPL
[ Time : 0.297s | 18 Queries | GZIP : Off ]
 
Loading