Hello.
I keep getting errors in the arc lines that my CAM software spits out and I'm not sure how to fix the post processor or Mach itself to get them to work. 

Here are the details:

CAM software is RhinoCAM using Mach3-Inch.spm post processor

In the circle tab I have the following options

Output Format
-I,J,K and Radius
-I,J,K only             <-----------this one is selected
-Radius only

Arc Center (I,J,K)
-Absolute         <----------------this one is selected
-Vector from Center to Start
-Vector from Start to Center
-Unsigned Vector from Start to Center

Here is the circle block format:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]

RhinoCAM also has the following options that can be checked:

-Output arcs as linear segments                   <-------------I have this one unchecked but I'm not sure what I should do with the other two.
-Output spiral motions as linear segments
-Output helix motions as linear segments


Now in Mach I tried both absolute and incremental  but I keep getting these two errors:



In IJ mode Absolute I get this error:

Zero radius arcLine 140

140:G03X-1.1733Y0.5598I-0.8561J0.9783



In IJ mode Incremetal I get this error:

Radius to end of arc differs from radius to startLine 942

942:G02X1.6663Y0.4917I0.3265J0.4175


These are just the first ones to pop up in reality almost every arc line gets an error.

Sorry can someone help me get this straightened out?

I would much rather cut arcs than line segments.
 

 

Do you have a setting to or can you find out what the setting is for precision.

Sometime, this can be only because you post output value like 2.1234 and the real value is 2.123

Normally, you would choose incremental value for center of arc.

Check the value in your cad or cam program and check what it is output by the post.


Jeff

Please post your G-code using the "Additional Options" when posting a reply.

Thanks for the tip, I think you may be right.  I remember someone telling me that the arc tolerance must be less than the global tolerance and I had it equal in a couple of places.  I set both the post processor and Mach to Absolute because the post processor didn't have incremental as an option for arcs, only for motion (G91), then I set the global tolerance to .0001 and the arc fitting tolerance to .001 and that seemed to do the trick.

Can Mach handle arcs in spiral or helix motions?  I had heard it was one or the other but I can't remember which.  Could it be both?

Now I'm getting a new error:

"K word given for arc in xy plane 9"

G00 G49 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing)
M6 T3G43 H3
S5000M03
G00Z0.2500
X0.1249Y-0.0042
G01Z-0.2960 F7.3
G17
G03X0.1250Y0.0000Z-0.5473I0.0000J0.0000K0.2500 F10.0

I can't seem to change anything in the settings that eliminates the K even when outputting all in linear segments.  Is this something I'm going to have to edit in the block format?

Helical Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]K[HELIX_LEAD]

Circular Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]Q[SPIRAL_LEAD]

K is for XZ plane.

I and J are for XY plane

Maybe you do not work on the right plane with your cam software.


Or is there a setting in the Cam software to not output arc on the XZ and YZ plane, only on the XY plane.

Just a tough, I don't use Rhino but I know Mastercam has that option.

Jeff

Thanks I found the setting I have spiral interpolation set to G17 XY plane but do I set Helical interpolation to G18 XZ plane or G19 YZ plane?  It seems to me a Helix is both XZ and YZ.

I'm thoroughly confused now.  I can't seem to get Mach to read the file with any of my settings.  I know that G17 followed by the K is causing problems but I can't seem to fix it so I'm going to post all the info I can and hopefully someone way smarter than me can spot the problem and tell what settings should be what.

Here is a sample toolpath that gives errors in Mach:
   

Here is the machining preferences settings in RhinoCAM:


Here are the relevant tabs in the post processor:




Here is the GenConfig page in Mach:


Here is the gcode produced:

G00 G49 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing)
M6 T3 G43 H3
S5000M03
G00Z0.2500
X0.1249Y-0.0042
G01Z-0.2960 F7.3
G17
G03X0.1250Y0.0000Z-0.5473I0.0000J0.0000R0.125K0.2500 F10.0
X0.1774Y-0.7284I0.0000J0.0000R0.7497Q0.3500
X-0.1774Y0.7284I0.0000J0.0000R0.7497
X0.1774Y-0.7284I0.0000J0.0000R0.7497
G01X0.1250Y0.0000
X0.1035Y0.0700
G03X0.1250Y0.0000Z-0.7737I0.0000J0.0000R0.125K0.2500
X0.1774Y-0.7284I0.0000J0.0000R0.7497Q0.3500
X-0.1774Y0.7284I0.0000J0.0000R0.7497
X0.1774Y-0.7284I0.0000J0.0000R0.7497
G01X0.1250Y0.0000
X0.1035Y0.0700
G03X0.1250Y0.0000Z-1.0000I0.0000J0.0000R0.125K0.2500
X0.1774Y-0.7284I0.0000J0.0000R0.7497Q0.3500
X-0.1774Y0.7284I0.0000J0.0000R0.7497
X0.1774Y-0.7284I0.0000J0.0000R0.7497
G01X0.1250Y0.0000
X0.0000
G00Z0.2500
M5 M9
M30

Ok the forum is not letting me edit the previous post but that is not the correct gcode to go with those settings.

This one is:



G00 G49 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing)
M6 T3 G43 H3
S5000M03
G00Z0.2500
X0.1249Y-0.0042
G01Z-0.2960 F7.3
G17
G03X0.1250Y0.0000Z-0.5473I0.0000J0.0000K0.2500 F10.0
X0.1774Y-0.7284I0.0000J0.0000Q0.3500
X-0.1774Y0.7284I0.0000J0.0000
X0.1774Y-0.7284I0.0000J0.0000
G01X0.1250Y0.0000
X0.1035Y0.0700
G03X0.1250Y0.0000Z-0.7737I0.0000J0.0000K0.2500
X0.1774Y-0.7284I0.0000J0.0000Q0.3500
X-0.1774Y0.7284I0.0000J0.0000
X0.1774Y-0.7284I0.0000J0.0000
G01X0.1250Y0.0000
X0.1035Y0.0700
G03X0.1250Y0.0000Z-1.0000I0.0000J0.0000K0.2500
X0.1774Y-0.7284I0.0000J0.0000Q0.3500
X-0.1774Y0.7284I0.0000J0.0000
X0.1774Y-0.7284I0.0000J0.0000
G01X0.1250Y0.0000
X0.0000
G00Z0.2500
M5 M9
M30

I believe if you want Incremental IJ, it would be  Vector from Center to Start.

I'd try changing these:

Helical Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]K[HELIX_LEAD]

Circular Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]Q[SPIRAL_LEAD]

To these:

Helical Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]

Circular Interpolation:
[CIR_PLANE]
[G_CODE][NEXT_X][NEXT_Y][NEXT_Z][NEXT_I][NEXT_J]

And the Helical plane should still be G17.

I've never used RhinoCAM, though.