[galaxyman7]

Hi, I have been having trouble importing NC code into Mach 3 Mill. I generate the code with MasterCam X2 using the drill toolpath, and I copied the path over again using the transform toolpath. When I verify it in Master Cam, everything looks good (pic attached). Also, I opened it on a free NC viewer, and everything looked good (pic attached). But when I opened it in Mach 3, the viewer showed 2 holes missing (pic attached). When I ran the machine, it doesn't drill those two holes, plus it drills a few of them twice. It is almost like the machine forgot to move before drilling the hole.
Here is the G-code:

%
O0000
(PROGRAM NAME - TEST2 )
(DATE=DD-MM-YY - 27-11-10 TIME=HH:MM - 12:30 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/8 CENTERDRILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .125 )
N104 T1 M6
N106 G0 G90 G54 X-.8007 Y.3492 A0. S2139 M3
N108 G43 H1 Z.1
N110 G99 G81 Z-.5 R.1 F6.
N112 X.1552 Y.3316
N114 X-.8042 Y-.1975
N116 X.1834 Y-.2116
N118 G80
N120 X1.1993 Y.3492
N122 G99 G81 Z-.5 R.1 F6.
N124 X2.1552 Y.3316
N126 X1.1958 Y-.1975
N128 X2.1834 Y-.2116
N130 G80
N132 X-.8007 Y1.3492
N134 G99 G81 Z-.5 R.1 F6.
N136 X.1552 Y1.3316
N138 X-.8042 Y.8025
N140 X.1834 Y.7884
N142 G80
N144 X1.1993 Y1.3492
N146 G99 G81 Z-.5 R.1 F6.
N148 X2.1552 Y1.3316
N150 X1.1958 Y.8025
N152 X2.1834 Y.7884
N154 G80
N156 M5
N158 G91 G28 Z0.
N160 G28 X0. Y0. A0.
N162 M30
%

[galaxyman7]

Anyone know how to fix this?

[mactec54]

galaxyman7

Pm me you email, then, I will do a program for you, The one you have is not done right

[galaxyman7]

That is strange, because I made it in Master Cam. What is wrong with it, and how can I fix it?

[neilw20]

On the Mach3 screen see the rectangular border.
I believe some of the coordinates are outside of the soft limits.

How to check.

Scale down to half size and load it again.

Mach3 sometimes can be a little confusing when the program is outside of the soft limits.

I loaded in NCPlot and it looked OK

[galaxyman7]

The soft limits are generated by Mach 3 when I import the code. I am pretty sure all the points are within the limits. There are points missing that are inside of the limits. I know that Mach 3 is not reading the code correctly, because I have loaded it in an NC viewer program and everything looked fine.

I was clicking through the code to see the machine movements for each line, and on some of the coordinates it doesn't move at all. Is there some line of G code that is not compatible with Mach 3?

[galaxyman7]

I looked at the code and realized that Mach3 skipped the coordinate after every "G80" in the code. I took all of the G80's out, and now it gets all of the points. However, it still drills the first hole in each pattern twice. Any ideas why the G80 was screwing with Mach 3, and why it still drills some holes twice?

[mactec54]

galaxyman7

Just because MasterCam spits out your program, it does not meen it is correct, it's only as good as the post processor has been set up, for the G code you want to get out

Because your program is really just one canned cycle, that's all it needs to be, you have done it 4 times

You have used a G81 this will send your .125 centre drill straight to depth at .500 deep
that's very deep for a .125 centre drill to do in one shot, a G83 would be better to use

It does not matter what cam program you use if it's not set up right, & you don't no what the G code should look like, you will always have these problems


O0000
(PROGRAM NAME - TEST2 )
(DATE=DD-MM-YY - 27-11-10 TIME=HH:MM - 12:30 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/8 CENTERDRILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .125 )
G0Z0. (If you don't have a tool changer it's a safety to have a Z move at the start of the program)
T1 M6
G54
S2139M3
G90G0X-.8007Y.3492
G43H1Z.1
G73G98X-.8007Y.3492Z-.5R.1Q.030F6. (You could use a G73 or a G83)
X.1552Y.3316
X-.8042Y-.1975
X.1834Y-.2116
X1.1993Y.3492
X2.1552Y.3316
X1.1958Y-.1975
X2.1834Y-.2116
X-.8007Y1.3492
X.1552Y1.3316
X-.8042Y.8025
X.1834Y.7884
X1.1993Y1.3492
X2.1552Y1.3316
X1.1958Y.8025
X2.1834Y.7884
G80G0Z0.
M5
G28X0.Y0.
M30
%

[ger21]

What version of Mach are you using? It seems to run fine here on 3.42.040

[mactec54]

Gerry

Your Gui screen set looks great

[galaxyman7]

Obviously they must have fixed some bugs in the new one! I will look into it.
As for the depth of 0.5, its just a test code so it doesn't matter. I am not really going to use this to drill anything. I just needed to know how to fix the problem.

Mactec- I really don't want to have to sift through all the gcode that I make, when Master Cam should be compatible with Mach in the first place. Do you have any ideas on how to change the settings in Master Cam? That would make my life a lot easier.

[mactec54]

galaxyman7

No cam system out of the box is compatible with any controls, You have to find or ajust the post processor, to suit the control in most cases, Mach control is very good, as it can take quite a lot of poorly put together G code, as other controls will not

Contact MasterCam Tec, & they will help you to get your post processor set up, But you also have to know how the G code needs to be, or they won't be able to help you very much