[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.

[metalworkz]

It is good that Mach3 displays the drawn part when loaded so when you see circles where arcs are should be you will know to change the IJ mode. I use several software packages to produce programs and just change the IJ mode accordingly. I guess I should be more ambitous and set all the software to generate the same, maybe someday. Glad you got your problem solved!
Regards,

[John S.]

The L1M_MACH3 post processor works in Abs and not Inc.

I did post in post #2 that you needs Abs arcs.

If you want an Inc post then just shout up.

John S.

[antelnation]

I am sure there is a simple fix for this but I can not figure it out. Say I just want to mill a 1 inch by 1 inch pocket that is 1 inch deep. When I draw this in DCAD and then bring it into DCAM, where can I control the depth (i.e. "z") of each pass.
With my Taig mill, I can only take small cuts in metal on each pass. I would prefer to make a 1 inch deep pocket in 20 passes ( .05 inch deep cut 20 times) but I cant figure out how to control the depth of cut. Can someone point me in the right direction. Thanks-Josh

[metalworkz]

Hi Josh,
There are a couple ways to set the depth of each pass.
1) When you define the tool you will use you can define the depth of the cut in that tool definition dialogue box. Then when you create the pocket etc and use the tool you defined it will not cut more than the depth it is defined with, so it will cut to the total depth in passes at the defined depth.
2)In the dialogue boxes for most of the machining operations there are boxes to fill in for the total depth and number of passes. If you designate a total dpeth of .50" and 10 passes it will cut at .050" a pass.
I can get a screen shot of these examples if needed, just let me know. Hope this helps you get it done.
Regards,

[IMG][/IMG]

[IMG][/IMG]

[antelnation]

Thanks. It is really easy once someone tells you how to do it . Tomorrow I hope to mill my first part!-Josh

[metalworkz]

Hi Josh,

You're welcome! I'm glad if I was of some help. When you get some parts milled we would enjoy seeing them!
Regards,