[scottsss]

I'm taking a CNC course. The problem is they are having us write the programs manually. Which is a good thing since I seldom look at the code generated by CAM unless their is a problem.

My problem is with cutter compensation and circles. If I use a G42 it makes the circle to large. Which to me is funny since it should be to the right of the line. But if I switch over to a G41 the circle looks fine.

I figure that their is some simple but rule to this I've not been told, that once it is explained to me it will all make sense. Thanks.

[ger21]

Are you using G2 or G3. If G3, G42 will offset to the outside. G2 with G42 is offset to the inside.

[scottsss]

Hmmmm, I am going CCW. Do you know the rule that it follows to determin wether it is cutting on the outside or inside of the line?

[ger21]

G42 is the right side, G41 is the left side. If your going CCW (G3), then G42 will be on the outside (right), giving you a larger circle. Imagine walking along the toolpath, G42 puts the tool on your right, G41 on your left.

[CNCgr]

It's easier to remember it like this:
Conventional cut: G41 / Climb cut: G42

ger21 is right of course and this is what I was taught too, but you have to remember if you're going CW or CCW, inside or out.

Nikolas

[screensnot]

It's easier to remember it like this:
Conventional cut: G41 / Climb cut: G42

I believe you have that backwards. But that is the way I remember also. Of course, I'm thinking to myself:
Climb cut - use G41.
Conv. cut - use G42.

[CNCgr]

Nope! You made me take my books out but I was right.

[screensnot]

Using a 1.00" end mill, what size hole would you expect with this program:

T1 M6
M3
G70 G90
G0 X0 Y0
Z-1.0
G1 G41 X1.0 F10. D1
G3 I-1.0 J0
G1 G40 X0
G0 Z1.
M2

What dia. would you have put in the CDC table (1.00" or -1.00")?

What type of cut would you expect to see (conventional or climb)?

*edit: added M3

[scottsss]

Okay, wish the instructor mentioned this in his lector. I didn't find it i the reading either.

WHile I'm picking your brains. Anything else I should know about cutter comp.Going around a straight line, problem's etc.

The simple straight line programs I have written went smothly. But figure I'd ask while we are still on the subject.

[miljnor]

i don't know what Others do, but after I learned how to program and run cnc (awhile back) they put those handy little tool tables in the machine for the cutter diameter(or radius) and when programing by hand they were great..

Along comes cad cam. I found for me (not neccessarily for everyone, although all the guys I know) zero the tool size and only use the wear offset. Genrealy Ive found this causes less heartache. The cad programs often make cuttpaths that double back on them selves and some machines have issues with cutter comp interference telling you that you gouged the wall. Which is kind of annoying. Now you can turn the machine off but you still have the problem of the comp intiation and cancell moves that can be pretty dramatic when the tool gets larger.

All in all I find it easier to leave the diameter zero and use the offset like normal.

just my 2 cents.

[ger21]

Nope! You made me take my books out but I was right.

I don't think so. Conventional is G42, climb is G41.

[ghyman]

In the example program, it appears as though you are milling inside a round pocket (as opposed to milling outside a round boss).
Since you are cutting CCW (as the G3 shows), then your tool is to the LEFT side of the material (as viewed from the tool). In this case, you want to use a G41 cutter comp.
Now: Using a ø1.0" endmill, the value to put in the comp register is going to depend on the control. Most Fanuc and fanuc clones will use cutter RADIUS comp. Fadals use the acutal cutter DIAMETER. And, I am certain there is a parameter that will allow any machine to use diameter or radius.
But, for the purpose of this thread, I assume you are using a fanuc, in which case, you would put .500 (1/2 the cutter diameter) in your comp register.
And, I would expect it to cut a 2.00" hole.
As the tool wears, or is reground, then is will be smaller. You would then put a smaller value in the comp register, and the control will adjust the cut to compensate.

If you were willing around the outside of a boss using G3 (conventional milling), then the tool would still cut CCW, but now the tool is to the right of the material, so you would use a G42, but still use .500 in the comp register.
If you were climb cutting (G3 on the outside of a boss), then it would be a G41, but still with the .500 in the offset (comp register).

Imagine driving around a curvey road halfway up the side of a mountain. You are either on the left side of the rock wall, or the right. The endmill is doing the same thing, no matter if it climb- or conventional- cutting.

Here's how I learned it, hopefully it will work for you as well:
Clock-wise is 2 words, so it must be G2
Counter-clock-wise is 3 words, therefore G3
The tool is either to the left of the material, or it is to the right (as viewed from the tool). "L-e-f-t" has fewer letters than "R-i-g-h-t", so it uses the lower number (G41). I know it's a little silly, but I've never forgotten it, either.

Full cutter comp is what I have always called it when the actual dimension of the tool is put in the offset. This allows you to essentially program the contour using dimensions right off the print. It also allows you to change cutter sizes without editing the program.
Partial comp is when the program is already 'offset' for the tool, which allows you to keep your cutter comp offset at zero, and only adjust it as it wears. This is the only time you should use a negative value in your comp. Most CAM systems will output code that supports partial comp. However, if you want to change tool size for some reason, then the program will need edited, or you will have to have some funky numbers in your offset.

In either case, every time the G41 or G42 is called up, the tool must be able to move at least the amount in the cutter comp offset.
Either way works, but keep this in mind... every program you write should always use the same method (full or partial). If the next person who sets up the job doesn't know, and guesses wrong, there will be some wonderful surprises!!!

[screensnot]

Ghyman, you are right that it is milling inside of a hole.

No it won't alarm because the toolpath is for a 2" hole. Note the the move is 1.0" as the comp is applied. So this toolpath will work for any size tool that is <2.0" dia., or <1.0" radius.

And I always set my machines to use tool diameter, not radius. This includes my Fanuc machines. It just makes more sense to me to measure the tool and enter that size directly (instead of dividing by 2). That is why I call it a CDC table (cutter diameter compensation table), instead of a CRC table (cutter radius compensation table).

[screensnot]

I see you removed the part of your post about it alarming out.

[CNCgr]

I don't think so. Conventional is G42, climb is G41.

Well either my book is wrong or we have a different definition of climb and conventional cut

[ger21]

we have a different definition of climb and conventional cut

Yep, you have them mixed up.

[CNCgr]

Sorry, I must insist. On the top left example of the first picture you see the cutter turning CW with the workpiece on it's right. It has the tendency to "climb" or "roll" onto the work.

When the cutter turns CW and the workpiece is left of its path the teeth have the tendency to "dig in". That's the conventional milling.

[CNCgr]

Another reference

Yet another

[ger21]

Assuming your looking down in the picture, the top left one with the orange cutter would be a left handed tool, the blue one a right handed tool. Bringing left handed tooling into the picture makes it even more confusing.

Using right handed tooling, G42 is conventional, G41 is climb. Look carefully at all the examples you posted, and assume in the first examples that the tooling is right handed, and your looking down on the work.

[ger21]

The reference at digital-calipers you linked to shows the workpiece moving, not the tool, so the actual tool movement is opposite the arrows they show. Looking at the other link, it shows the same thing.

All the examples you've posted agree with what I'm saying, but you're interpreting them opposite.