What's new
What's new

polar rotating on fanuc equipped vmc

duginski2006

Plastic
Joined
Nov 21, 2011
Location
wisconsin , usa
I have a Kitamura mycenter3 I recently aquired. The programming manual is somewhat vague. I have used Tree's with dynapath controls and they have a very easy polar rotate command that works great for rotating complex pockets ect. around an axis and repeating them. I have never used a G16 command. How do they work or is this something I need a macro for?
Thanks
 
The programming manual is somewhat vague.

As is your post. If you want help with programming a CNC, how about saying which CNC is being discussed?:willy_nilly: There are lots of models of Fanuc, and we aren't there to see your machine!

A cartesian coordinate is the X and Y distance from origin that we're all familiar with using. A polar coordinate specifies a point relative to the origin by an angle and radius. The angle is standard geometry, that is, 0° is at the 3 o'clock position, and larger angles rotate counterclockwise from there. Another example would be 225° would be at the 7:30 position from the origin. The radius is from the origin to the point. Where this can be very useful is drilling a bolt-circle, where instead of figuring all the X and Y hole locations, you just change the angle from one hole to the next, with the same radius. It would be most useful on round features that are concentric with the part "zero" position.

You don't "need a macro for" it, although an internal macro does the calculating. You could use User Macro to do coordinate rotation if the control didn't have the rotation option.

EDIT: Just saw that I had replied to your other post asking how to remove a rotary table from the machine. You did state there it's an 11M. It helps a lot to be specific about model numbers, etc. because there are so many possibilities. Sometimes it really does make a difference.
 
The Dynopath "Rotate" feature isn't the same as a Fanuc "Polar" feature is it?



----------------

Think Snow Eh!
Ox
 
I wish it was Ox, I just pulled a detail of my Matt. and finished it on my Lagun kneemil wit a Dynapath so as I could mach. a tapered bore.
Gw
 
How about a G68 I think it is? G68 X0.0 Y0.0 R45.0 should rotate the x and y axis 45 degrees in the positive direction?

Fred t
 
Maybe it is an available parameter that just needs turned on. I am unable to help in that area but someone here should be able to give ya a hand with it.
Good Luck
Fred T
 
yup you are correct.the op description seemed like axis rotation would do what he is asking tho. I at the edge of my knowledge here.
Fred T
 
The OP is kind of talking about 2 different things. Now from what I know G16 will be in lines with polar rotation which will tie in with a rotary axis. This may or may not be similar to G12.1 for polar interpolation (Bill aka angelw) is going to know this cold.

However Fred is correct that G68 appears to be what the OP is looking for as stated in post #5. G68 will be an option that needs be active in the control so you may get an "improper G-code" alarm when trying to use it. If this happens send me a PM.

Now if this is the case then a macro or a looping sub program will be the best approach to program the typical shape around the part.

Stevo
 
The OP is kind of talking about 2 different things. Now from what I know G16 will be in lines with polar rotation which will tie in with a rotary axis. This may or may not be similar to G12.1 for polar interpolation (Bill aka angelw) is going to know this cold.

However Fred is correct that G68 appears to be what the OP is looking for as stated in post #5. G68 will be an option that needs be active in the control so you may get an "improper G-code" alarm when trying to use it. If this happens send me a PM.

Now if this is the case then a macro or a looping sub program will be the best approach to program the typical shape around the part.

Stevo

Hi Stevo,

Yes, I interpret the OP's thread as you do. If he wants to use the same NC data for a complex feature, indexed and repeated around an axis, then G68 is what he would use.

G16 is similar to G12.1 in that they both relate to angles, but in an opposite way. The difference between the two, is that G12.1 (Polar Coordinate Interpolation) is applied when a rotary axis is involved and the tool path is programmed with no consideration whatsoever to an angular command that would normally be applied to the rotary axis. Its a function that exercises contour control in converting a command programmed in a Cartesian Coordinate System to the movement of a linear axis and the movement of a rotary axis . Conversely, G16 allows slide positioning to be made via Polar Coordinate System, that is, coordinates defined by an angle and a distance. And as you know Stevo, you have to set linear and rotation axes for Polar Coordinate Interpolation in parameters beforehand, whereas with G16 you do not; there is no virtual axes swapping involved when using G16.

Following is an example of G16 being used in conjunction with a drilling cycle and Absolute mode.
N1 G17 G90 G16
G81 X100.0 Y30.0 Z–20.0 R–5.0 F200.0
Y150.0
Y270.0
G15 G80

In the above example, holes will be drilled at the Absolute angles of 30.0°,150.0°, and 270.0°, with a radius of 100.0mm from the Polar origin

The following example uses Incremental mode to specify the angle. Note that the first hole position is specified in Absolute mode to set the radius of the hole from the Polar origin and the Start angle . Subsequent angular moves are then made incrementally.

N1 G17 G90 G16;
G81 X100.0 Y30.0 Z–20.0 R–5.0 F200.0
G91 Y120.0
Y120.0
G15 G80

In the above example, holes will be drilled also at the Absolute angles of 30.0°,150.0°, and 270.0°, with a radius of 100.0mm from the Polar origin.

Regards,

Bill
 
Last edited:








 
Back
Top