Need Help!- Fanuc 21i-T Lathe, tool nose radius compensation

[tds11223]

Why, oh why, does the machine turn a diameter on size when I do not use the Imaginary tool nose data compensation? If I do not put in a compensation # then my turned diameters come out correct but my radii do not...

[angelw]

Originally Posted by tds11223 Why, oh why, does the machine turn a diameter on size when I do not use the Imaginary tool nose data compensation? If I do not put in a compensation # then my turned diameters come out correct but my radii do not...

Post the issue part of your program, the description of the tool being used and the number being used as the tool type in the tool offset registry.

Regards,

Bill

[sinha_nsit]

In straight turning and straight facing, there would be no error even if radius compensation is not used, except the small uncut part at the end.
This is because the center of the tip is not the reference point of the tool.
You touch a diameter and then a face in offset setting. This gives you what is called "imaginary tool tip" as the reference point of the tool.

[broby]

The answer is because the machine does not know the direction of the radius from the qualified edge to apply Tool Nose Radius compensation.
Parallel diameters and Straight faces (not tapers) will ALWAYS come out correct, providing your tool is set correctly, but as soon as you introduce tapers and radii into your program you need to "compensate" for the radius on the tip of the tool.
The program will use G41 or G42 to tell the machine which side of the profile the tool is on, but the machine needs to know what orientation the tip of the tool is also.
Bottom line is that to get the correct profile on any part, you need to set up the nose radius completely on your tool data page.
Regards
Brian.

PS this would apply to ANY controller/machine...

[tds11223]

Not sure what you mean by "Set up tool data completely" Broby. Please clarify..


All others....I will try to post the program completely but here's the deal....

I am running this part program off of the Fanuc control described earlier. The control allows me to run the program directly from the "conversational" portion of the control. I do have the option to convert it to G-code but I do not have to.

I will need to post the code out but if I remember correclty the machine doesn't generate a G41 or G42 when it does post a code....


Thanks for the help, please keep it coming

[angelw]

Originally Posted by tds11223 Not sure what you mean by "Set up tool data completely" Broby. Please clarify.. All others....I will try to post the program completely but here's the deal.... I am running this part program off of the Fanuc control described earlier. The control allows me to run the program directly from the "conversational" portion of the control. I do have the option to convert it to G-code but I do not have to. I will need to post the code out but if I remember correclty the machine doesn't generate a G41 or G42 when it does post a code.... Thanks for the help, please keep it coming

In the attached picture the circle with the labels 1 and 2 represents the tool radius of a typical OD, right hand turning tool. The points of the tool radius that will be tangent to the vertical face and horizontal OD surfaces are 1 and 2 respectively. and its these points that are programmed using such a tool. Accordingly, its irrelevant when turning parallel to the X and Z axis what tool radius is used, points 1 and 2 are always the tangent points irrespective of the tool radius.


When turning a taper, as shown in the attached drawing, if the tool starts at the dimensional coordinates of the start of the taper and sent to the dimensional coordinates at the end of the taper, the tool will follow the path shown by the green line, rather than the correct path shown in yellow.. To achieve the correct path the tool will be offset in an X minus direction at point 4 at the start of the taper and in Z minus at point 5 at the end of the taper.

When programming a radius, the tool path of the tool radius is calculated based on its center point. Once the start and end coordinates of the tool radius center have been calculated the coordinates of point 1 and 2 of the radius shown in the attached picture are easily obtained by adding or subtracting the radius of the tool radius. In X twice the radius will be used due to lathe programs mainly being programmed in terms of work diameter.

The part program can be created using dimensions directly from the part drawing if cutter radius compensation is used. Using this method, G41 and G42 will be used to tell the control which side of the programmed path the cutting tool is located. The control also needs to know the style of the tool and the tool radius being used. This information is applied in the Tool Offset registry pages. Typically, a right hand OD turning tool will be entered as a type 3 tool if point 1 and 2 as shown in the attached picture are used as the cutter location points.

If the code posted by your control does not contain G41 or G42 therein, it means that the control is calculating the true location of the tool based on the tool radius information supplied when the program was being created graphically. When cutter radius compensation (G41, G42) is used, the calculations for cutter location are made by the control on the fly. I'm not a fan of using cutter radius compensation (G41 , G42) on a lathe. Cutter Rad Comp is necessary on a machining center, as its required to adjust component feature size, but with a lathe, diameter size is controlled with the wear or geometry offsets.

Regards,

Bill

[broby]

When I say "Set up your tool data completely" I refer to the fact that you need to set up all the following items:
1. Tool offset X & Z
2. Size of the Nose Radius
3. Direction of the Nose Radius.
Obviously the Tool Offset values are a given, don't set them up and no chance of getting size on your job.
Size of the Nose Radius will tell the program how much to compensate the position of the tool to allow the edge of the radius to touch the profile. Refer to the post above.
The "Direction" of the Nose Radius refers to where the centre of the Nose Radius is relative to the X and Z axis offsets.
Hope that helps.
Brian.

[tds11223]

I believe to have the tool offset page set up correclty with the correct radius(per the insert) and direction according to the fanuc manual.

When doing this I have to offset the tool -x in order for it to cut a diameter and the radius correclty. The offset needed will relate directly to the diameter of the radius put in the tool offset page. Such a large wear offset really is cumbersome to work with. If I do not set up the radius and nose tip compensation then a large offset is not needed but the radii are out of tolerance by whatever nose radius the insert used has.

Is it possible to have the best of both worlds? A raduis compensation and direction according to the tool, little to no offset in the tool data wear and not changing the tool data geometry except for inital sizing?

I have programmed this manually and adjusted the part program to cut per the insert radius I selected. But with modern controllers(especially a conversational style) I don't know why I need to do this and would rather not.

Thanks again

[broby]

Sounds like you have a parameter incorrect...?
I can not help as I don't have a Fanuc machine to look at and fiddle with to test...
Sounds very strange to me the problem you are having.
Good luck.

[sinha_nsit]

You have both GEOMETRY and WEAR offsets for radius (in fact, for everything), so need not use large wear offset. And, you specify radius, not diameter.