Making Programs Shorter - How To?

[Bill H]

I use the 2D Dynamic Mill toolpath quite a bit and the G-code output can get crazy long.  In looking at this, I've seen twenty or thirty consecutive lines of code that are only X-axis moves.  Is there a setting or option that would eliminate some of this unnecessary code?  Thanks!

[Leon82]

Turn on the filter or make your tolerance Bigger

[Bill H]

Filter?  Please explain.

[Colin Gilchrist]

18 minutes ago, Bill H said:

Filter?  Please explain.

All Toolpaths in Mastercam have a Line/Arc Filter option. 2D Contour, 2D Dynamic, Flowline, Raster, Etc.

This is the page where you set the Total Tolerance, and then break that total tolerance up between the Cut Tolerance (accuracy of the tool position, relative to the geometry)  and the Line/Arc Filter. 

The Line/Arc Filter takes your path, and first applies a Linear Filter, which tries to combine linear moves within the given tolerance. Then, an Arc Filter is applied to the path, using the Tolerance specified in the Operation settings.

There are some radio buttons which control "us max tolerance value for lines and arcs", "bias the Filter toawrds creating only lines", or "bias the Filter to create only arcs".

Set your Total Tolerance to  10-20% of your Stock to Leave value. 

If you are leaving 0.040" Stock for your roughing, for example, I'd use 0.004" Total Tolerance. 

For roughing, I typically use a 50% split for Cut Tolerance and Filter Tolerance. Set the Min Arc Rad to 0.004, and the Max Arc Rad to 40.", with the top radio button option selected. 

Make sure XY, XZ, and YZ checkboxes are enabled. Also, turn on 'create arcs on entry motion' checkbox.

 

 

[CEMENTHEAD]

I also use Fixed segment length. when using dynamic paths and cutting splines sometimes you can get a series of breaks in a single axis move. this eliminates them quite well.

 

 
(WITHOUT FIXED SEGMENT LENGTH)
 
N1G17G98G40G49G80G90
N2G0X0.Y7.
N3T1M6
N4S1000M3
N5G0G90G54X-4.2745Y2.4416B0.
N6G43H1Z4.
N7M08
N8Y2.4415Z.1
N9G1Y2.4416Z0.F10.
N10G41D1X-4.2245
N11G2X-3.1005Y2.6916I.5898J0.
N12G1X-2.2949
N13X-1.2949
N14X-.2949
N15X.3784
N16X1.3784
N17X2.3784
N18X3.3784
N19X3.8539
N20G2X5.0489Y2.4416I.5714J-.25
N21G1G40X5.0989
N22G0Y2.4415Z4.
N23Y2.4416
N24M09
N25G0G28G53G49Z0.M19
N26G90X0.Y7.
N27M01
 
 (WITH FIXED SEGMENT LENGTH AT 44.00)
 
N28G17G98G40G49G80G90
N29T1M6
N30S1000M3
N31G0G90G54X-4.2745Y2.4416B0.
N32G43H1Z4.
N33M08
N34Y2.4415Z.1
N35G1Y2.4416Z0.F10.
N36G41D1X-4.2245
N37G2X-3.1005Y2.6916I.5898J0.
N38G1X3.8539
N39G2X5.0489Y2.4416I.5714J-.25
N40G1G40X5.0989
N41G0Y2.4415Z4.
N42Y2.4416
N43M09
N44G0G28G53G49Z0.M19
N45G90X0.Y7.
N46M30
%

[JB7280]

5 hours ago, Colin Gilchrist said:

All Toolpaths in Mastercam have a Line/Arc Filter option. 2D Contour, 2D Dynamic, Flowline, Raster, Etc.

This is the page where you set the Total Tolerance, and then break that total tolerance up between the Cut Tolerance (accuracy of the tool position, relative to the geometry)  and the Line/Arc Filter. 

The Line/Arc Filter takes your path, and first applies a Linear Filter, which tries to combine linear moves within the given tolerance. Then, an Arc Filter is applied to the path, using the Tolerance specified in the Operation settings.

There are some radio buttons which control "us max tolerance value for lines and arcs", "bias the Filter toawrds creating only lines", or "bias the Filter to create only arcs".

Set your Total Tolerance to  10-20% of your Stock to Leave value. 

If you are leaving 0.040" Stock for your roughing, for example, I'd use 0.004" Total Tolerance. 

For roughing, I typically use a 50% split for Cut Tolerance and Filter Tolerance. Set the Min Arc Rad to 0.004, and the Max Arc Rad to 40.", with the top radio button option selected. 

Make sure XY, XZ, and YZ checkboxes are enabled. Also, turn on 'create arcs on entry motion' checkbox.

 

 

One of the best arc filter explanations I've read.  

[Chally72]

Here's a video that, while a little lengthy, touches upon just about every field, toggle, and switch in arc filtering/tolerancing:

 

 

[Bill H]

Thanks to everyone for the replies!  I've got a better understanding now.