Help with program

[tc1]

We tried to run a program on our cnc over the weekend with a code generated with bobcad. I had a very experienced machinist helping me as this is our first adventure into cnc. If we tried a G02xyij, it would run okay, but if it followed a G01 move, it would flash an error 1084.

This code works:
G90G1X0.0Y0.0
G2X1.0Y-1.0I0.0J-1.0

This code does not
G90G0X0.0Y0.0
G1Y1.0
G2X1.0Y2.0I1.0J1.0
G1X2.0

Both codes ran correctly on a diferent machine. We are using a Fagor 8055i mc controller on our mill. If anyone has any suggestions it would be appreciated! The full code is attached if anyone wants to see how we got here, the program would stop with an error on N10

Travis

[angelw]

We tried to run a program on our cnc over the weekend with a code generated with bobcad. I had a very experienced machinist helping me as this is our first adventure into cnc. If we tried a G02xyij, it would run okay, but if it followed a G01 move, it would flash an error 1084.

This code works:
G90G1X0.0Y0.0
G2X1.0Y-1.0I0.0J-1.0

This code does not
G90G0X0.0Y0.0
G1Y1.0
G2X1.0Y2.0I1.0J1.0
G1X2.0

Both codes ran correctly on a diferent machine. We are using a Fagor 8055i mc controller on our mill. If anyone has any suggestions it would be appreciated! The full code is attached if anyone wants to see how we got here, the program would stop with an error on N10

Travis

Hi Travis,

Your BobCad program is outputting I and J as the Absolute coordinate of the Arc Centre. Whereas the Fagor control uses the format that describes the Arc Centre in terms of an incremental distance from the Arc start point.

In your above two examples, the first example will successfully cut the same path whether the control used Absolute or Incremental Arc Centre definition, hence the reason why it successfully executes. The second example will only run on a control that uses Absolute Arc Centre definition.

Try the following code, the centre of the Arc is defined as an Incremental distance from the Arc start point. It should follow a tool path as shown in the attached picture.

Regards,

Bill

G90G0X0.0Y0.0
G1Y1.0
G2X1.0Y2.0I1.0J0.0
G1X2.0

[tc1]

That would probably make a difference. I wonder if I can get a post- from bobcad to account for that difference. I will try that code tomorrow at the shop. Thank you for you help!

Travis

[sinha_nsit]

Why not use radius method which is simpler to use and works in most cases.

[angelw]

Why not use radius method which is simpler to use and works in most cases.

Hi Sinha,
As you pointed out some time back in another Forum, and Fanuc themselves make the statement in their manuals as follows:

"When an arc having a center angle approaching 180° is specified, the calculated center coordinates may contain an error. In such a case, specify the center of the arc with I, J, and K."

Accordingly, if you wanted to make sure that accurate work resulted, and use "R" format, you would need a Post that would swap to I,J, and K format when the arc approached 180deg. I think it would be simpler to just use I, J, and K format.

R Format can be useful in turning operations when trying to tune out taper, due to, for example, the workpiece flexing away from the cutting tool. But in Milling operations, this is seldom, if ever, a consideration.

For me, I see it as an added advantage of being able to program a complete circle with the one circular interpolation block. Also, because the control calculates an arc/circle centre based on the Start and End points passed via the NC Code, an erroneous tool path can result without it being obvious, if either of the passed points are incorrect. In this case, within reason, the control just shifts the centre to allow the circular trajectory to pass through the two points. When using I,J, and K format, any such error would cause an alarm to be raised.

Although a small point in the whole scheme of things, the Post for using "R" format is a little more difficult to write, as arcs greater than 180degs need to be determined and accommodated with an "-R" output.

Regards,

Bill

[annoying]

We tried to run a program on our cnc over the weekend with a code generated with bobcad. I had a very experienced machinist helping me as this is our first adventure into cnc. If we tried a G02xyij, it would run okay, but if it followed a G01 move, it would flash an error 1084.

This code works:
G90G1X0.0Y0.0
G2X1.0Y-1.0I0.0J-1.0

This code does not
G90G0X0.0Y0.0
G1Y1.0
G2X1.0Y2.0I1.0J1.0
G1X2.0

Both codes ran correctly on a diferent machine. We are using a Fagor 8055i mc controller on our mill. If anyone has any suggestions it would be appreciated! The full code is attached if anyone wants to see how we got here, the program would stop with an error on N10

Travis

The one thing I will say is, if you are in a learning process, learn your G-codes. It is easier than learning and dealing with CAM software... or so I think.

The second bit of code, as stated, looks like absolute center, nothing real uses that.

The attached file... approaching line N10, the end point of N9 and the arc point numbers in N10 just completely do NOT jive, whether you look at arc center as incremental or absolute, Unless I'm overlooking something

[angelw]

The one thing I will say is, if you are in a learning process, learn your G-codes. It is easier than learning and dealing with CAM software... or so I think.

The second bit of code, as stated, looks like absolute center, nothing real uses that.

The attached file... approaching line N10, the end point of N9 and the arc point numbers in N10 just completely do NOT jive, whether you look at arc center as incremental or absolute, Unless I'm overlooking something

Hi annoying,
Yes, I agree with learning how to program first with G codes etc, rather than putting blind faith in a CAM package.

The code is correct for a control that uses Absolute coordinates for the I and J. In this case I2.8743 J0.6875 is the centre of the arc in Absolute coordinates, that passes through points X2.8743 Y0.4375 and X2.6243 Y0.6875. The OP's resolve to this issue is to get a Post Processor application that output the I, J, and K as incremental rather than absolute values.

Regards,

Bill

[sinha_nsit]

One has to learn arithmetic first before trying to use a calculator.
The same applies to manual part programming and CAM software.