I'm a total CAM newbie, but I'm watching some tutorials and starting to get the hang of it.

Not sure if the problem is with mastercam or mach3, but the rapid toolpath (which should be hovering the bit above the workpiece) cuts down deeper than the cutting toolpath. This leaves a nasty line through the workpiece.

Here is the beginning of the G-code:
N110 G54 G0 X99.286 Y-163.176
N112 S18000 M3
N114 G43 H1 Z162.837
N116 Z72.837
N118 G1 Z60.837 F2000.
N120 X173.225 F5000.
N122 X198.231 Y-153.286
N124 X76.091
N126 X60.648 Y-143.397
N128 X214.902
N130 X228.029 Y-133.508
N132 X48.676
N134 X38.924 Y-123.618
N136 X238.848
N138 G0 Z70.837
N140 Z160.837
N142 Z162.837
N144 X394.41 Y-113.729
N146 Z72.837
N148 G1 Z60.837 F2000.
N150 X345.861 F5000.
N152 G0 Z70.837

Also, you can see in the picture that some of the little curves/turnarounds are sharper than the rest. Any ideas what could be causing that? Also looks like I have it programmed for a bigger tool, but that's no biggie.

How do I convert the G-code from metric to inch in X editor?

Thanks soooo much.
-Ed

You dont want to convert your G-code. In Mastercam select an Inch configuration and it will update the units from MM to Inch. . Then just regenerate the operations and re-post the code.

Mike Mattera.

Not sure if the problem is with mastercam or mach3

Programmer!! LOL

Hi Ed,

the rapid toolpath (which should be hovering the bit above the workpiece) cuts down deeper than the cutting toolpath. This leaves a nasty line through the workpiece.

Check the Clearance, Retract, Top of Stock values on the setting parameters page
if this is good, check the transition settings on the pocketing parameter page, look at the "keep tool down" & "finish at nearest entity" boxes in the Finish contour section

Also, you can see in the picture that some of the little curves/turnarounds are sharper than the rest. Any ideas what could be causing that? Also looks like I have it programmed for a bigger tool, but that's no biggie.

Horizontal passes-- are controlled by "stepover"( % of Tool Dia, or a value )
eg
A 1" flat endmill with sharp corners , max stepover 100% or 1" =to clear a flat
area. ( normally 60-80% used)
A 1" bullnose with 1/4" corner rads( base dia = 1/2"), max stepover=.5". ( normally 60-80% of base diameter used)

A 1" ballnose will leave channels but say 0.03" stepover is a good finish

The "Turnarounds", are controlled by the stepover, the contour shape boundary, and a couple of other settings, these are removed when doing a finish pass around the shape
The gouge from the end of the clearing pass to the start of the finish contour is controlled by how you want the tool to behave, as described above ( if islands or walls, maybe retract between Z-levels )

Steve

Thanks for the replies. I'm also reading some of the PDF manuals that came with Mastercam.


Everything works fine when I verify it in Mastercam, but when I go to actually cut the part here's what happens:

The green line moves from 0,0,0 to the starting point of the program. Then the purple line moves Z up about 5 inches, Orange=Z down about 1". This is where the program starts cutting the piece, about 4 inches above the stock.

I'm needing to eliminate the purple line's 5 inches of upward Z movement.

Where is your geometry in Z that you have for the pocketing routine,
and have you set your depth to Incremental, if you use incremental values, they are in relation to the geometry you have selected, not from your origin

If your top face is set as Z0, anything Z+ is good and safe, Z- is below and could cut material, when you set-up like this, try using absolute values in the early stages as it would be easier to troubleshoot

Steve

Sounds to me like this is either one of a couple things. You have the Z depths, rapid and retract set inproperly or it could be an issue with the post itself.

I had an issue that verified great in X3, I sent it to the machine and ran a draw there and it freaked out and ran something toltally different. I contacted my reseller, sent them a zip2go and they ran my code on cimco, found the error, edited my post and sent it back...now no issues!!

Notice that your Clearance, Retract, Top, and Depth all have little options for Abs and Incr. (Absolute Positions and Incremental Positions). Sounds like you have them set to Incremental when you want them to be absolute (in reference to absolute Z zero).

Mike Mattera

Your turns and curve could be caused by the post. Not that the post is bad. You may need to set the Control Diffinition Manager. Set arcs to "break at quadrants" .
I'am not sure if this is the problem. I've had this too. All looks good in mastercam but not when milling.