Fanuc lathe cutter compensation

[60rock]

I would like to know how many people use their lathe's cutter compensation funtion.

[txcncman]

I do for any parts with tolerances on diameters of +/-0.005 or less.

[dcoupar]

I use it any time there's an angle or radius in the profile.

[60rock]

Would either of you be willing to post a sample of the code you are using if it includes G41/G42 in the lathe setting? Also, being a Fanuc control, what setting you used in the tool data/offset page?

[dcoupar]

Would either of you be willing to post a sample of the code you are using if it includes G41/G42 in the lathe setting? Also, being a Fanuc control, what setting you used in the tool data/offset page?

Here's a finish pass from a Doosan Lynx program.

T07 geometry offset was set to R0.0156 T3

N7G0G40G99
G30U0
G30W0
T0707(VNM331 FINISH)
G97G42S2500X1.35Z.1M3
M8
G96S1500
X.18
G1Z0F.004
X.875,C.05
Z-.625
X1.125Z-1.334
Z-2.
X1.25,C.01
Z-2.15
X1.35
G0G40Z.1M9
G30U0W0M5
M1

[angelw]

I do for any parts with tolerances on diameters of +/-0.005 or less.

Why would the diameter tolerance be a criteria for the use or not of tool radius compensation? I don't get that.

tds11223
The only time I would consider using Tool Nose Radius Compensation on a lathe, is
1. if the profile was made up of a series of many linear and circular, elements and where the Tool Nose Radius will have a significant bearing on the size and relationship of those elements.
and
2. where the appropriate measuring equipment is available to be able to measure those elements. In a production environment that would mean either equipment at the machine, or periodic inspection away from the machine via a Shadow Graph or a CMM.


Tool Radius Compensation is practically mandatory with a machining centre, as that is the most convenient method of regulating the size of various features. However, with a Turning Centre, the diameter of the overwhelming majority of components is regulated by the X offset of the tool.

Although there are some version of the Multi Repetitive G71 cycle where Tool Nose Radius compensation can be used, the Series 10 for example, there are many where it can't. I haven't tested its viability on late Series controls, but the following extract from a Fanuc Manual for Series 18 would suggest not.

"The offset of the tool tip radius is not added to finishing allowances
Δu and Δw. In turning, the offset of the tool tip radius is assumed to be
zero."

Therefore, if a profile containing concave form is being roughed using the G71 cycle, the X finishing allowance would have to be substantial to avoid the part being over-cut by the trailing edge of the tool radius. If the profile is created with the Tool Nose Radius compensated for in code, so as to use the G71 cycle for roughing, then you have the profile for finishing without having to use Tool Nose Radius compensation at the control as well.

If a tool that has a large Tool Nose Radius, like a 10dia button, is used in roughing, and the roughing program has been created not using a roughing cycle, then, on the reverse direction move back to the start point ready for the next cut, you must remember to either:
1. Retract the tool far enough to avoid the tool plunging into the work due to the large TNR, because on the Return Path the tool is now on the Opposite Side of the profile compared to during the Cut Path.
2. Cancel TNR comp before returning for the same reason as in 1
3. Swap from G42 to G41 for the return path, again for the same reason as in 1

I've used such tools with larger Tool Nose Radii where there has been deep concave profiles using a technique similar to High Speed Machining on a machining centre, where small depth of cuts are made with very high feed rates.

I don't buy the argument that its easier to program using TNR comp on a turning project. Most drawings don't come with all the X,Z coordinates provided. Accordingly, if creating the program:
1. manually, you have to calculate the intersection and or tangent points. To make these calculations including the TNR is no more difficult.
2. using a CAM system, then there is certainly no argument that its more difficult to compensate for the TNR in the program as opposed to using TNR compensation at the control

In my opinion, there are more negatives to using TNR compensation on a lathe, at the control, than for not.

Regards,

Bill

[fordav11]

I don't buy the argument that its easier to program using TNR comp on a turning project. Most drawings don't come with all the X,Z coordinates provided. Accordingly, if creating the program:
1. manually, you have to calculate the intersection and or tangent points. To make these calculations including the TNR is no more difficult.
2. using a CAM system, then there is certainly no argument that its more difficult to compensate for the TNR in the program as opposed to using TNR compensation at the control

In my opinion, there are more negatives to using TNR compensation on a lathe, at the control, than for not.

there are more negatives sure. but if you don't have access to CAM package using TNRC is a must. Manually calculating anything but simple 90 degrees arcs is way too complex for most people unless they know their trigonometry well and how to calculate the TNRC manually (99% of machinists don't)
Using some form of TNRC is mandatory on ANY machine, especially on complex shaped parts with tapers and tangent arcs. Otherwise tapers and arcs will not be formed correctly.

p.s. on the original question... because of the negatives (listed above), because almost everything I do has complex curves and tangents and because I use conversational software to generate my program profiles, I never use G41/G42 on a CNC lathe. I prefer to let the software calculate the coordinates to include TNRC.

[angelw]

Manually calculating anything but simple 90 degrees arcs is way too complex for most people unless they know their trigonometry well and how to calculate the TNRC manually (99% of machinists don't)
Using some form of TNRC is mandatory on ANY machine, especially on complex shaped parts with tapers and tangent arcs. Otherwise tapers and arcs will not be formed correctly.

Where arcs less than quadrants, and angled lines tangent to or intersecting arcs are concerned, trigonometry is still required whether TNR compensation on the control is used or not. To include the calculations for the tool radius when calculating these coordinates is no big deal. Tapers and arcs will only be incorrect if the TNR is not compensated for in the code, and the calculations aren't really rocket science.

I don't see what the big issue is between calculating the coordinate for the apex of the Red triangle, to include the TNR comp, as opposed to the apex of the Grey triangle, to use TNR comp by the control (see the attached picture). And as you seem to confirm, to have a CAM (Conversational) system generate the program, there are no difficulties compensating to the TNR in the program.




Regards,

Bill

[fordav11]

My basic argument (addressing the OP's question) is using G41/G42 on a lathe is more trouble than it's worth but it's a necessary evil if conversational software isn't available (and yes trig is required also).

A simple example is cutting a 1mm radius on the OD of a piece of bar with a 1.2mm rad insert.
G0 X50.0 Z1.0
G1 Z0
G3 X52.0 Z-1.0 R1.0

Without TNRC the corner is left sharp (no radius is formed on the part).

With TNRC you will get a 1mm radius because the control adds on the required amount to compensate. The tool is essentially doing this.....
G0 X47.6 Z1.0
G1 Z0
G3 X52.0 Z-2.2 R2.2

Obviously the smaller the tool nose radius is the less important TNRC becomes and the simpler the part is the easier it is to work out compensated values manually.

If the part is complex the only way to write a program properly and achieve the correct profile is to use CAM software.

Having said that I know people who program parts without using TNRC or trig (they use the guess, cut, then manually adjust method) and they get away with the parts they make because the positions are not important. But if they had to make a tapered part to fit a hardened and ground gauge they would be in serious trouble with Quality Control

[angelw]

A simple example is cutting a 1mm radius on the OD of a piece of bar with a 1.2mm rad insert.
G0 X50.0 Z1.0
G1 Z0
G3 X52.0 Z-1.0 R1.0

Without TNRC the corner is left sharp (no radius is formed on the part).

With TNRC you will get a 1mm radius because the control adds on the required amount to compensate. The tool is essentially doing this.....
G0 X47.6 Z1.0
G1 Z0
G3 X52.0 Z-2.2 R2.2

If the part is complex the only way to write a program properly and achieve the correct profile is to use CAM software.

We'll have to agree to disagree on this Ford. I know the above example is simple, but the calcs to include the TNR compensation in the program don't even require a calculator. In my opinion, there would be more in ensuring that the G42/G40 were being applied correctly than there would in calculating the true position of the tool for the program.

What do you consider to be a complex profile? At the end of the day, you only have combinations of angled lines and arcs, either tangent with or intersecting each other. Many profiles can seem complex when viewed as a whole, but broken down into elements, as one must do even when manually calculating the tangent and intersecting point with no TNR considered, the calculation becomes no more difficult than in the picture attached in my previous Post.

Regards,

Bill

[fordav11]

Here's a quick hand-sketched example. The rads are marked with an R. I would write the program for this in about 10 minutes (this is a stylized example not an actual real part).
If you can manually calculate all the taper to arc and arc to arc intersections for each point where TNRC is required in less than 6 hours you win a lollypop. I'm not talking about trig, I'm talking about adjusting the coordinates to compensate for the tool radius.
I really don't care to argue with you about this example or whether TNRC is good or not.
My answer to the original question is 'no I don't use it I use software to generate the program including TNRC instead'

[angelw]

Here's a quick hand-sketched example. The rads are marked with an R. I would write the program for this in about 10 minutes (this is a stylized example not an actual real part).
If you can manually calculate all the taper to arc and arc to arc intersections for each point where TNRC is required in less than 6 hours you win a lollypop. I'm not talking about trig, I'm talking about adjusting the coordinates to compensate for the tool radius.
I really don't care to argue with you about this example or whether TNRC is good or not.
My answer to the original question is 'no I don't use it I use software to generate the program including TNRC instead'

Six hours? Sure I could; as could any programmer with half decent maths skills.

Your missing the point with regards to the difficulty comparing calculating the Tangent/Intersection points of your pictured part, with and without TNR compensation included. In all cases where trigonometry is concerned, the sides on the triangle only increase of decrease by the TNR, depending on whether, for example, if a radius is convex or concave. The only additional work required at each cutter location, once the centre of the TNR is found (up to that point, no difference in time between calculating the points with and without the TNR being considered), is the addition or subtraction (depends on the direction of travel and tool type) of TNR x 1 in Z and TNR x 2 in X (tool type 1,2,3 and 4). Now if a programmer is not up to that additional simple maths, he or she should be looking for a new line of work.

When I have to write NC programs nowadays, I also use a CAM package; my own. And I don't use TNR comp for all the reasons stated in my original post. But when comparing programming methods, CAM to CAM and Manual to Manual, I see the difference, in terms of difficulty, when creating code for use with and without TNR comp by the control, as none via a CAM system, and infinitesimally small via Manual calculations.

Regards,

Bill