[ales1919]

Hello,
my name is Alex and I have a question. At work, we talked about use of cutter compensation. Some had opinion that one always has to program centerline of the tool, use g41/g42 and then put cutter radius value to offset registry (1/2 end mill = D-0.25.
Some suggested, that you can use this method when you program manually, but if using CAD/CAM you should use software to compensate the tool radius and enter 0. to offset registry. If not you can run in problems when programming complex 3D shapes, when you combine 2d and 3d tool paths.
What is your opinion about this? Is it OK to enter numbers already compensated, or enter numbers from drawing and compensate them by entering tool radius in offset registry?
Thanks a lot for your opinions, they are all welcomed

[dak1]

Hi Alex.
We have always used CAM for programming & have always programmed centerline of tool using cutter comp only for deflection & tool diameter compensation. (1.00 mill milling a 2.00 hole would be programmed with a 0.500 arc & 0 entered into comp register if using a new tool). Hole size would then be adjusted based on measurement and/or if tool is undersize (if tool is 0.980, enter -0.010 in register to start). We've also aquired manual programs that were programmed by feature size & required tool radius in the comp registry. I like the centerline method with CAM doing the math. The other is probably easier if manually programming, but I'm not an advocate of that. Here is something to consider. The most common issue we run into with comp application is this (Fanuc being the predominate controls). Errors are common if the length of the linear application motion is less than the ammount in the comp register. (If you have a -0.05 in the register & the motion to apply this is only a 0.04 long motion, expect the control to bark). We typically use a 0.100 motion length to apply comp. That being said, we do not do any 3D complex milling so I can't speak to that. Our stuff is simple 2D work including some thread milling (all inch mode). Hope this helps.

Dave

[dak1]

Another consideration. The fewer numbers you require the operator to enter at the control, the smaller the risk of typo's or just plain errors.

[txcncman]

Use the same method throughout the company.

[sinha_nsit]

If CAM software is being used, there is no need to use G41/G42. Based on the defined tool geometry, the software would automatically generate the compensated toolpath.

For a taper thread, use R-word in the second block of G76. Sign convention and taper amount match with those in G90.

[txcncman]

If CAM software is being used, there is no need to use G41/G42. Based on the defined tool geometry, the software would automatically generate the compensated toolpath.

For a taper thread, use R-word in the second block of G76. Sign convention and taper amount matches with G90.

Without G41/G42, tool path and part size are not "adjustable" at the machine. Not using G41/G42 might be ok for when the operator has the knowledge to use and access to the CAM software to "reprogram" parts at will. In most cases, it would be more beneficial to use G41/G42.

[sinha_nsit]

I have machined several complex 3D surfaces with a ballmill on a 3-axis milling machine, using a commercial CAM software (IDEAS). I only needed to define the tool geometry, and selected the proper reference point on the tool.

[Geof]

You can use a ballmill with CAM output that has the tool compensation incorporated in the code and not activate G41/G42 but the precision of the surface will not be any better than the precision of the tool. This is probably okay for a 3D surface which does not have to mate precisely with another surface.

If you are machining something that has IDs and ODs that must be more precise than the tool diameter then you have to activate G41/G42 with a tool diameter of 0. so that 'wear' can be used for the final tweaking of sizes.

[dak1]

If CAM software is being used, there is no need to use G41/G42. Based on the defined tool geometry, the software would automatically generate the compensated toolpath.

For a taper thread, use R-word in the second block of G76. Sign convention and taper amount match with those in G90.

I fail to understand why you would want to regenerate & reload a program each & every time you want to make a wear adjustment, which is what this suggests, even IF the operator had access to the CAM software. ALWAYS use comp so features can be EASILY tweaked at the machine. What this post suggests is that a 5 second process of entering a comp in the register be replaced with a minimum of a 5 minute process of regenerating & reloading a program. That's assuming a very small program also.

[sinha_nsit]

Geof has explained it properly; where to use, where not needed to use G41/G42.

[cogsman1]

For those shops that have setup people that always "forget" to enter the radius values when loading the tools, you can always do it from the program as long as you have "Macro" capability.

#2218=.0625
This statement would load .0625 into the "R" for the geometry offset #18.
Then the operator could make fine adjustments from the WEAR offset page and not have to edit the program.

[Geof]

That is what the G10 command is for.

[fordav11]

yes, but note G10 is also an option that not every machine has ;-)

G41/G42 is most useful on a mill when profiling a contour that needs minor adjustments to get toleranced dimensions.
Its less important on a lathe because G41/G42 can cause problems when machining pockets. it's really only useful for simple stepped shaft type parallel or taper machining operations if an operator wants to write a simple program at the control and he doesn't have any CAM/conversational software capability on the machine. if the part is complicated using G41/G42 won't help because the operator is not capable of writing such a program.... and if he is capable he can use CAM software to save time with calculations.

On our lathes we avoid it entirely in all programs across the entire company and use built-in compensation (generated in CAM s/w) and list the tool insert and radius in the program to force operators to use the tools and inserts we (the programmers) want them to use and this also has the benefit that there are no dig-in errors with machined pockets since all code is written long-hand. another benefit of writing the code long-hand is it stops novice operators messing with the program ;-)

[dak1]

Hello,
my name is Alex and I have a question. At work, we talked about use of cutter compensation. Some had opinion that one always has to program centerline of the tool, use g41/g42 and then put cutter radius value to offset registry (1/2 end mill = D-0.25.
Some suggested, that you can use this method when you program manually, but if using CAD/CAM you should use software to compensate the tool radius and enter 0. to offset registry. If not you can run in problems when programming complex 3D shapes, when you combine 2d and 3d tool paths.
What is your opinion about this? Is it OK to enter numbers already compensated, or enter numbers from drawing and compensate them by entering tool radius in offset registry?
Thanks a lot for your opinions, they are all welcomed

Just to clarify. The original post implied mill application to me, which was the assumption of my reply. We do not use G41/G42 comp on turned features except in very RARE cases (tight tolerance ball type features in our case). Almost all of what we do in turning mode can be tweaked easily with the X/Z wear oregisters. But all features contured on a mill or in milling mode (mill/turn apps) include the the G41/G42 comp functonality, regardless of tolerance.