MC is turning arcs into straight line moves

[WeGrok69]

I am running X5 MU1 I have a 12 inch dia plate with 11.8 dia. pocket and 12n lobes for tapped holes the inside radii are .25 - i am using a 1/4" endmill.

It spits out straight line moves on some of the radii. It does not do it with an 1/8" em or a 1/2" em but it starts at .498 dia. not sure when it stops but a 1/8" gives a good tool path so does .188 dia. but .200 gets me G01"s instead of G02"s on four arcs - at .250 dia i have 16 sets of G01"s some moves are one liners .010 long like it has small lines in the geometry.

This came from a SolidWorks x_t file so I drew it in MasterCam and i know it has no straight lines.

Has anyone seen this before - I haven't in the 15 years I've been using it - something in my settings maybe???

here is my X5 file...

GOOD GEOMETRY.MCX-5

[gcode]

I tried your file with a stock Generic Fanuc 3X mill machine def and I don't see any straight line output.

 

Can you post some of your code??

[gcode]

This is the output I got

 

%

O0999(TEMP)

(DATE=DD-MM-YY - 26-07-12 TIME=HH:MM - 17:27)

(MCX FILE - C:\JUNK\GOOD GEOMETRY.MCX-5)

(NC FILE - C:\DOCUMENTS AND SETTINGS\MY DOCUMENTS\MY MCAMX5\MILL\NC\TEMP.NC)

(MATERIAL - ALUMINUM INCH - 2024)

( T1 | | H1 | D1 | WEAR COMP | TOOL DIA. - .25 )

G20

G0 G17 G40 G49 G80 G90

T1 M6

G0 G90 G54 X0. Y5.725 S3333 M3

G43 H1 Z2.

Z.1

G1 Z0. F77.

G41 D1 X.0354 Y5.7604 F7.

G3 X0. Y5.775 R.0501

X-1.023 Y5.6837 R5.775

X-1.1254 Y5.5501 R.1251

G2 X-1.8004 Y5.3693 R.3551

G3 X-1.9559 Y5.4337 R.1251

X-3.7278 Y4.4107 R5.775

X-3.7497 Y4.2438 R.125

G2 X-4.2438 Y3.7497 R.355

G3 X-4.4107 Y3.7278 R.125

X-5.4337 Y1.9559 R5.775

X-5.3693 Y1.8004 R.125

G2 X-5.5501 Y1.1254 R.3549

G3 X-5.6837 Y1.023 R.1249

Y-1.023 R5.775

X-5.5501 Y-1.1254 R.1251

G2 X-5.3693 Y-1.8004 R.3551

G3 X-5.4337 Y-1.9559 R.1251

X-4.4107 Y-3.7278 R5.775

X-4.2438 Y-3.7497 R.125

G2 X-3.7497 Y-4.2438 R.355

G3 X-3.7278 Y-4.4107 R.125

X-1.9559 Y-5.4337 R5.775

X-1.8004 Y-5.3693 R.125

G2 X-1.1254 Y-5.5501 R.3549

G3 X-1.023 Y-5.6837 R.1249

X1.023 R5.775

X1.1254 Y-5.5501 R.1251

G2 X1.8004 Y-5.3693 R.3551

G3 X1.9559 Y-5.4337 R.1251

X3.7278 Y-4.4107 R5.775

X3.7497 Y-4.2438 R.125

G2 X4.2438 Y-3.7497 R.355

G3 X4.4107 Y-3.7278 R.125

X5.4337 Y-1.9559 R5.775

X5.3693 Y-1.8004 R.125

G2 X5.5501 Y-1.1254 R.3549

G3 X5.6837 Y-1.023 R.1249

Y1.023 R5.775

X5.5501 Y1.1254 R.1251

G2 X5.3693 Y1.8004 R.3551

G3 X5.4337 Y1.9559 R.1251

X4.4107 Y3.7278 R5.775

X4.2438 Y3.7497 R.125

G2 X3.7497 Y4.2438 R.355

G3 X3.7278 Y4.4107 R.125

X1.9559 Y5.4337 R5.775

X1.8004 Y5.3693 R.125

G2 X1.1254 Y5.5501 R.3549

G3 X1.023 Y5.6837 R.1249

X0. Y5.775 R5.775

X-.0354 Y5.7604 R.05

G1 G40 X0. Y5.725

G0 Z2.

M5

G91 G28 Z0.

G28 X0. Y0.

M30

%

[Rotary Ninja]

I posted using a generic Haas post and our modified Haas post and I get G01's as well. I then used a generic Fanuc post and got no G01's just as gcode did. I have never seen this either. Will mess with it more in a bit and see if I can figure this out.

[Rotary Ninja]

This is really weird. I have recreated the file from scratch. Used tools from my own library. And I get the G01's still. I have a couple more things I am going to try.

[Müřlıń®]

I posted using a generic Haas post and our modified Haas post and I get G01's as well. I then used a generic Fanuc post and got no G01's just as gcode did. I have never seen this either. Will mess with it more in a bit and see if I can figure this out.

 

My HAAS post outputs lines as well....

 

They really get ugly on a 24 inch diameter circle.

 

Yes it would be great to get this figured out.

[gcode]

I loaded the stock Haas 4X post and got line output..

 

went to the arcs page of the control def and turned End Point error checking off

 

Now it posts arcs ..

It was set to "Round end point- break arc on failure

 

so I'm thinking the arcs endpoints exceed the tolerances set on the Tolerance page of the Control Def

[gcode]

OK

 

I turned End Point Error checking back on

 

and on the Tolerance Page

 

I changed NC Precision from

 

.0001 to .00001 and I'm getting all G02/G03 output ..

 

My conclusion, the endpoints of the arcs are not quite right when rounded to 4 places

[Rotary Ninja]

Well, I offset the contour -.010" and rechained it and got all G03's

 

I thought now I am onto something! This wouldn't work of course because your part ID would be .020" small. But this was just a test. I then went into the toolpath parameters and on the contour paramaters page I changed the stock to leave on walls to -.010" so the tool would cut to the proper dimensions. I then got the G01's again I even chainged the arc filter total tolerance to .0002" thinking maybe that would fix it, but it didn't.

 

So I went back to your original program and the only thing I did differently was I changed the stock to leave on walls to .0020". The area that it posted with the G01's became a lot smaller. So I tried .0025". The G01's went away. So you could offset your tool -.005" on diameter and get a good part essentially.

 

That still doesn't explain why this is happening though

[Rotary Ninja]

gcode solved this in the middle of my reply lol.

[WeGrok69]

Thank you VERY much!!! I had changed everything in the config tolerance page to .00001 but I haven't played with the control def's before today.

There is a bunch of stuff in there that would probably make my life easier if only I knew what i was doing!

Well thanx again everyone and especially gcode.

-tim

[Müřlıń®]

OK

 

I turned End Point Error checking back on

 

and on the Tolerance Page

 

I changed NC Precision from

 

.0001 to .00001 and I'm getting all G02/G03 output ..

 

My conclusion, the endpoints of the arcs are not quite right when rounded to 4 places

 

Thank you G.

 

That was bugging the crap outa meh