Problem Converting Machining Contours to G-Code

[antelnation]

Hi everyone,
So I can finally draw my parts in DFX file format. I can import them into DCAD and I can create the machining contours (I am just making a series of 0.14 inch holes in a rectangular piece of aluminum.... I am building a tooling plate).
I run the machining simulation in DCAD and it looks good. That is to say, the simulation does what I want my mill to do.
Next, I go to "post process" to create my g-code. I am using Mach3 to run my little Taig mill so I chose "LM1-MACH3.ppr" and I left the "file extension" as "pun". Following that, I load that g-code file into Mach3.
This is where the problem is: Mach3 can not read the g-code. Mach3 says:"Unknown word Starting with rline1".
So, how do I generate G-code that Mach3 can understand? Thanks-Josh

[Mike Stevenson]

Can you post your code so I can understand?

[John S.]

Josh,
There is a Syntax error in the post file.
Try this one attached and you will have to have arcs selexted as Absolute in General Config in Mach 3.

Let us know how you go on.

John S.

[antelnation]

Here is the g-code or should I say N-code that DCAD generated.-Josh





%
( Produced :- 14:42:24 Friday, May 16, 2008 )
( CNC File :- V1 )
( Post Processor :- L1M_MACH3 )
( Part Number ID :- )
N6G00G20G17G90G40G49G80
N7G49
N8T1M06 ( End Mill )
N9G00G43Z5.0H1
N10S1000M03
N11X0.0Y0.0
N12X12.0Y5.5
N13X12.0Y5.5Z0.1
N14G01X12.0Y5.5Z-0.5
N15G03X11.9913Y5.5088I11.9913J5.5
N16X11.9825Y5.5I11.9913J5.5
N17X12.0Y5.4825I12.0J5.5
N18X12.0175Y5.5I12.0J5.5
N19X12.0Y5.5175I12.0J5.5
N20X11.9825Y5.5I12.0J5.5
N21X11.9913Y5.4913I11.9913J5.5
N22X12.0Y5.5I11.9913J5.5
N23G01X12.0Y5.5Z0.1
N24G00X12.0Y5.5Z5.0
N25S1000
N26X12.0Y6.25
N27X12.0Y6.25Z0.1
N28G01X12.0Y6.25Z-0.5
N29G03X11.9913Y6.2588I11.9913J6.25
N30X11.9825Y6.25I11.9913J6.25
N31X12.0Y6.2325I12.0J6.25
N32X12.0175Y6.25I12.0J6.25
N33X12.0Y6.2675I12.0J6.25
N34X11.9825Y6.25I12.0J6.25
N35X11.9913Y6.2413I11.9913J6.25
N36X12.0Y6.25I11.9913J6.25
N37G01X12.0Y6.25Z0.1
N38G00X12.0Y6.25Z5.0
N39S1000
N40X12.0Y7.0
N41X12.0Y7.0Z0.1
N42G01X12.0Y7.0Z-0.5
N43G03X11.9913Y7.0088I11.9913J7.0
N44X11.9825Y7.0I11.9913J7.0
N45X12.0Y6.9825I12.0J7.0
N46X12.0175Y7.0I12.0J7.0
N47X12.0Y7.0175I12.0J7.0
N48X11.9825Y7.0I12.0J7.0
N49X11.9913Y6.9913I11.9913J7.0
N50X12.0Y7.0I11.9913J7.0
N51G01X12.0Y7.0Z0.1
N52G00X12.0Y7.0Z5.0
N53S1000
N54X12.0Y7.75
N55X12.0Y7.75Z0.1
N56G01X12.0Y7.75Z-0.5
N57G03X11.9913Y7.7588I11.9913J7.75
N58X11.9825Y7.75I11.9913J7.75
N59X12.0Y7.7325I12.0J7.75
N60X12.0175Y7.75I12.0J7.75
N61X12.0Y7.7675I12.0J7.75
N62X11.9825Y7.75I12.0J7.75
N63X11.9913Y7.7413I11.9913J7.75
N64X12.0Y7.75I11.9913J7.75
N65G01X12.0Y7.75Z0.1
N66G00X12.0Y7.75Z5.0
N67S1000
N68X12.0Y8.5
N69X12.0Y8.5Z0.1
N70G01X12.0Y8.5Z-0.5
N71G03X11.9913Y8.5088I11.9913J8.5
N72X11.9825Y8.5I11.9913J8.5
N73X12.0Y8.4825I12.0J8.5
N74X12.0175Y8.5I12.0J8.5
N75X12.0Y8.5175I12.0J8.5
N76X11.9825Y8.5I12.0J8.5
N77X11.9913Y8.4913I11.9913J8.5
N78X12.0Y8.5I11.9913J8.5
N79G01X12.0Y8.5Z0.1
N80G00X12.0Y8.5Z5.0
N81M09
N82M30
%

[Dolphin USA]

Just out of curiousity... is there a reason that you are using the Level 1 Mach post? Are you doing everything inside Partmaster CAD, i.e. not using Partmaster CAM at all?

[antelnation]

Well, the simple answer is that there was a video tutorial on how to do this in DCAD. I could try to do it in CAM but I see no reason why it would generate a better g-code.

[antelnation]

I get a weird result. The post processor simulation that runs in Partmaster Cam looks perfect. The end mill does exactly what it is supposed to do.... it makes 0.16 inch holes that are 0.5 inches in depth.
However, when I load the g-code into Mach3, the code that is loaded does not reflect what was simulated in Partmaster Cam. Does anyone know what I am doing wrong.
I attached the .cnc and the .pun file that I made in Partmaster. Thanks.

[Mike Stevenson]

I do. In MACH3 under Config ----> General Config please note the IJ Mode in the second column on the page. It should be set to INC not ABS.

[Dolphin USA]

Mike, you were about 11 seconds to fast for me. About to say the same thing!

[Mike Stevenson]

Why MACH3 comes with this important IJ parameter set to ABS as the default is beyond me.

[antelnation]

Well, it was set to INC. So, I switched it to ABS and now it is working. Weird.
Thank you. Thank you. Thank you.

[Mike Stevenson]

Yes it was happy for me to see my K2CNC working the first time too. When I first loaded my G-code into the MACH3 software with the setting reversed my part looked like the many rings of Saturn in the plot window.