G02 Faulty Arc Geometry

[DLDL]

I'm basically trying to make a ball end on a 3/4" shaft and keep running into an error about the G02 lines. The onboard fault checking program doesn't say what is wrong, just the line that has a problem. I've used both R and I, K syntax and still get the error. This control definitely wants I, K in absolute dimensions. I've fudged beginning X +.0005 off centerline to make sure that the start and end points are positively in the same quadrant.

I've used G02 and G03 just fine on this machine before and just can't figure out what the problem is if not just some dumb syntax that I'm too tired to see.

The machine is an old OmniTurn conversion. I'll pound sand if this is the type of thing you don't want here, just let me know.

Here it is the code - error lines in bold. Absolute origin is X=0 at centerline, Z=0 at 1" out from part face. There is a rouging pass .020 out from the final pass. Spaces added only for some readability

G90G94F100
T1
X.001Z-.9
G95F.005
Z-.9485
G02 X.853 Z-1.375 I.0005 K-1.375 (alternate R.4265)
G00X.9
Z-.9
X.001
G01Z-.9685
G02X.813 Z-1.375 I.0005 K-1.375 (alternate R.4065)
G00X.9
Z0
M30

Any insight is appreciated! Thanks!

 

[angelw]

This control definitely wants I, K in absolute dimensions

Not when you're programming in Diameter Mode (G72), which, judging from the X coordinates in your program, you are. In the case of Diameter Mode programming, Incremental values are used from the Start Coordinates of the Arc to describe the Arc Centre. Absolute values for the Arc Centre are used in Radius Mode programming.

Regards,

Bill

 

[sinha]

If you post the description of the error message, it would be easier to analyse it.

 

[VTM]

I'm basically trying to make a ball end on a 3/4" shaft and keep running into an error about the G02 lines. The onboard fault checking program doesn't say what is wrong, just the line that has a problem. I've used both R and I, K syntax and still get the error. This control definitely wants I, K in absolute dimensions. I've fudged beginning X +.0005 off centerline to make sure that the start and end points are positively in the same quadrant.

I've used G02 and G03 just fine on this machine before and just can't figure out what the problem is if not just some dumb syntax that I'm too tired to see.

The machine is an old OmniTurn conversion. I'll pound sand if this is the type of thing you don't want here, just let me know.

Here it is the code - error lines in bold. Absolute origin is X=0 at centerline, Z=0 at 1" out from part face. There is a rouging pass .020 out from the final pass. Spaces added only for some readability

G90G94F100
T1
X.001Z-.9
G95F.005
Z-.9485
G02 X.853 Z-1.375 I.0005 K-1.375 (alternate R.4265)
G00X.9
Z-.9
X.001
G01Z-.9685
G02X.813 Z-1.375 I.0005 K-1.375 (alternate R.4065)
G00X.9
Z0
M30

Any insight is appreciated! Thanks!

Is It not a G3 move? Maybe not since Its an omniturn. Guess It depends on what side of the spindle the tool is on. And your K Is from your Z0 Not from the start point of the arc?

G1Z-.9485F.008
G3X.853Z-1.375K-.4265

 

[VTM]

It depends on the physical configuration of the machine with the OmniTurn Control; G02 could be correct for this machine. But the most outstanding error in the OP's program, is that his program is written using Diameter X Coordinates and incorrectly specifying the Arc Centre in Absolute terms.

With the OmniTurn Control, the Control can be set programmatically to use either Radius Mode (G73) or Diameter Mode (G72). G73 is the default Mode and to program in Diameter, G72 must be specified at the start of the program. As the OP has only listed a snippet of the program, he may be in either Radius or Diameter Mode.

1. If in the default, Radius Mode (G73), the I and K values are correct, but the X coordinates are incorrectly specified as Diameter, resulting in an error being raised.

2. If Diameter Mode (G72) has been specified earlier in the program, then the X coordinates are correct, but the I and K values are incorrectly specified in Absolute, rather than the correct Incremental values from the Start of the Arc, again resulting in an error being raised.

Regards,

Bill.

Makes sense. I have no experience with an Omniturn so I wasn't aware of the G72. It would be helpful then If he posted his entire code.

 

[angelw]

Is It not a G3 move?

It depends on the physical configuration of the machine with the OmniTurn Control; G02 could be correct for this machine. But the most outstanding error in the OP's program, is that his program is written using Diameter X Coordinates and incorrectly specifying the Arc Centre in Absolute terms.

And your K Is from your Z0 Not from the start point of the arc?

With the OmniTurn Control, the Control can be set programmatically to use either Radius Mode (G73) or Diameter Mode (G72). G73 is the default Mode and to program in Diameter, G72 must be specified at the start of the program. As the OP has only listed a snippet of the program, he may be in either Radius or Diameter Mode.

1. If in the default, Radius Mode (G73), the I and K values are correct, but the X coordinates are incorrectly specified as Diameter, resulting in an error being raised.

2. If Diameter Mode (G72) has been specified earlier in the program, then the X coordinates are correct, but the I and K values are incorrectly specified in Absolute, rather than the correct Incremental values from the Start of the Arc, again resulting in an error being raised.

Regards,

Bill.

 

[angelw]

Makes sense. I have no experience with an Omniturn so I wasn't aware of the G72. It would be helpful then If he posted his entire code.

Yes, it would, but irrespective of what Mode he is using, his program will raise and error, for he is mixing Radius and Diameter format in the Arc moves.

Regards,

Bill

 

[DLDL]

Not when you're programming in Diameter Mode (G72), which, judging from the X coordinates in your program, you are. In the case of Diameter Mode programming, Incremental values are used from the Start Coordinates of the Arc to describe the Arc Centre. Absolute values for the Arc Centre are used in Radius Mode programming.

Regards,

Bill

This is it. I just was spending too much time on the manual machine and thinking about diameters, when on this machine it makes more sense to stick with the default G73 (radius mode). Changing all the X to radius values works now. I knew it would be something so simple I couldn't see it. Thanks.

To hit a couple of other replies in case it is interesting for anybody:

-That is the entire code, not a snippet. G73 is default and doesn't need to be called out. My whole mistake here is using diameter values while the control is expecting radius

-Bill's response is also correct that while in G90 + G72, the G02 syntax would require incremental values for I and K.

 

[angelw]

when on this machine it makes more sense to stick with the default G73 (radius mode).

In my opinion, it would make more sense to use Diameter mode. Its not an arduous task to include G72 in what should be a safety line at the start of every program to ensure that the control is in the correct modes, such as Absolute, Diameter More, Tool Nose Radius Comp cancelled, etc. You've already experienced as issue by transitioning from a Manual Lathe, that predominately works in Diameter, to a machine that defaults to Radius Mode..

The overwhelming range of Micrometers are calibrated in Diameter and their readings are much more relatable to the coordinates in the part program if the part program uses Diameter coordinates. Further, more often than not, a parts drawing for a turned part, uses diameter dimensions; accordingly, you only have to read the dimensions from the drawing when creating the part program.

Regards,

Bill