Thread mill + cutter comp

[ISO86]

Went to do some thread milling today. Wrote my program out applied cutter comp outside of part ramped up and out of the job 1/4 of the pitch. All was good however on my G03 move after the cutter comp had been applied and engaged on the part (dry run first so no part so to speak) could cut the interpolation and ramp upwards in z at same time however when at the end of the arc would not have completely climbed up in Z axis and would sit there in XY whilst z climbed up. Was only .25mm or .010" but enough to no be right. I ended up just doing it by adding my radius along with tool radius together and not using cutter comp but is a pain to adjust any wear as you have to manually manipulate the whole program. Control is an anilam. Any ideas why when in cutter comp mode it would not completely climb in z as mentioned by the time it finished the arc?

[706jim]

Post your code. This will help us to analyze what you did.
For a thread, I would go to the hole center in G40 and then apply cutter compt to lead in. I would avoid applying cutter comp and then going somewhere for hole location as the position will be off by the compensated amount.

[ISO86]

External thread (METRIC)

G00 Z50
G40 X-60 Y-60
Z0
G01 Z-27.5 F1200
G42 X-40 Y-36.28 F400
G01 X0 Y-36.28 Z-27
G03 X0 Y-36.28 I0 J36.28 Z-25
G01 X40 Y-36.28 Z-24.5
G40 X60 Y-60
G00 Z50
X0 Y0
Z&P0 Y&P0 M09
M05
M02

[706jim]

How about:


G00 Z50
G40 X-40 Y-60
Z0
G01 Z-27. F1200
G42 X-5.0 Y-36.28 F400D01
G01 X0 Y-36.28
G03 X0 Y-36.28 I0 J36.28 Z-25
G01 X5.0
G40 X60 Y-60
G00 Z50
X0 Y0
Z&P0 Y&P0 M09
M05
M02

See if the absence of a vertical ramp makes any difference in the thread by making a simple, planar entry and exit.
I'm not familiar with your particular control.

[ISO86]

How does the planar entry affect thread form at entry and exit? It worked out fine in the end. Its the only real time we thread mill, for this 1 repair job we get maybe 4 times a year. However the supplies collar nut sometimes varies and using cutter comp would be nice to just be able to add a wear value to get the correct thread depth and fit.

[brian.pallas]

There are two basic ways of doing cutter comp. One we call "control" where you program to the #'s on the print and enter in the actual diameter of the tool in the appropriate offset entry. The second, and the one I use, I call "wear" compensation. Here you program the centerline of the tool, while still using G41 or G42 as the case may be. In your diameter offset you enter in the DEVIATION from the programed tool size. So if I program a 1/2" endmill and the operator has a reground one that measures .460 he would enter in "-.040" as the diameter offset. Since your lead on and off moves have to be equal to half your tool radius, "wear" basically allows .010 moves, or less, to turn comp on and off. Very handy for squeezing into tight spaces.

So if you wanted to program your thread in "wear" comp mode you would take the radius of your major dia. and subtract the radius of the tool and this will equal the programmed radius. Give yourself a .020 straight line move to turn comp on before threading and you should have wear adjustment through the offset page.

I switched from "control" to "wear" programming about 6 months after I started programming and for a few different reasons I like it much better. One big one is say you change jobs and what was a 3/4" EM in one job is now a 1/2" EM in the new job and the operator forgets to change the offset from .750 to .500, scrap part right? With "wear" both offsets would be 0.

[angelw]

There are two basic ways of doing cutter comp. One we call "control" where you program to the #'s on the print and enter in the actual diameter of the tool in the appropriate offset entry. The second, and the one I use, I call "wear" compensation. Here you program the centerline of the tool, while still using G41 or G42 as the case may be. In your diameter offset you enter in the DEVIATION from the programed tool size. So if I program a 1/2" endmill and the operator has a reground one that measures .460 he would enter in "-.040" as the diameter offset. Since your lead on and off moves have to be equal to half your tool radius, "wear" basically allows .010 moves, or less, to turn comp on and off. Very handy for squeezing into tight spaces.

The tight space argument is irrelevant. This scenario is covered whether Tool Radius (control), or Tool Wear Comp is used. The physical start location of the cutter's center, relative to the workpiece, can be the same whether "control" or "wear" cutter compensation methodology is used; only the programmed coordinates for the workpiece vary.

One big one is say you change jobs and what was a 3/4" EM in one job is now a 1/2" EM in the new job and the operator forgets to change the offset from .750 to .500, scrap part right? With "wear" both offsets would be 0.

There would be no scrap in the above example. Not changing the offset value from 0.750 to 0.500 will result in a metal on condition, if in fact the program executes past the block where the Cutter Radius Comp is applied. For the program to run, the program created for the 1/2" cutter in mind would have to have the cutter start point (tool center) before the Cutter Radius Comp is applied, more than 3/4" away from the move destination during Cutter Radius Compensation start up. If this is not the case, and the offset values not changed, then a Tool Radius interference error would occur. The inverse of your example will result in over cutting and probable scrap of the part. However, this scenario exist only if you have to change the physical tool and where the tool number used in each program is the same.

ISO86
You will generally have problems with Tool Radius Compensation (G41/G42) in simultaneous X,Y and Z linear moves unless the control is equipped with 3D tool comp options. Many controls baulk even when using G41/G42 with helical interpolation. If your control does handle Cutter Radius Comp in combination with helical milling, then you could replace the X,Y,Y linear move with a helical move through a quadrant, or part quadrant to ramp the cutter into contact with the workpiece. The Z component of this move will be the same percentage of the thread lead as the arc is a percentage of 360 degrees. Using this method with an OD thread will give you consistency in programming style as when programming an ID thread where an arc move is generally used to ramp into the workpiece surface.

Also, rather than starting at the bottom of the thread, which will necessitate conventional milling for a right hand OD thread, I would start one pitch up from the bottom, helical mill in a Clockwise direction, and use G41 so that climb milling is utilized.

Regards,

Bill

[ISO86]

Thanks Bill! Never thought to start up and helical move down to climb mill and maintain right hand thread. Even with upcut milling thread form and finish was excellent! I never iso program with cutter comp on a helical move so not sure but i know it will do it as it has a helical pocket canned cycle in the control (converstaional) that uses cutter comp effectively. Even if i used IJK or R method for interpolation it still had same result of a little z move at the end of that block.

[screensnot]

If you can't figure out how to make it work with G41/G42, you could add some macros to your program to do the offset for you, and have a toolpath that stays in G40.

You'd be able to adjust for wear using your comp tables, but not use G41/G42.