How to use G70/G71 if I'm not programming with G42/G41

Hi all,

I am a new member to this forum and am also relatively new to machining. I have a question regarding G71/G70 when NOT using G42/G41 nose comp.

Some background info: We are using a 1998 Daewoo puma 200 2 axis lathe with Mitsubishi Meldas 500 controller. We typically program the lathe by hand. Anyway, I've been putting the G41/G42 in the G71 canned cycle so the G70 canned cycle can apply tool nose comp. I know that the G71 ignores tool nose comp.

However, I feel like the lathe can get a mind of its own sometimes when g42/g41 tool nose comp is used, so I want to get away from using it and instead incorporate the tool nose radius directly into my code. For example, I have always done G42/G41 like this:

Generating a .040" radius on the front of the outer diameter of 3.188":
....
G00 X4.65 Z.05
G71 U.065
G71 P101 Q102 U.004 W.001 F.008
N101 G42 G00 X3.108
G01 Z0.
G03 X3.188 Z-.04 R.04
....

Note: G71 is using a turning tool with No.2 .031" nose radius and G70 would use a turning tool with a No.1 .0156" nose radius.

But, instead of using G41/G42, I want to incorporate the finishing tool's No.1 nose radius into code which would be:

G00 X3.076 Z.050
G01 Z0. F.005
G03 X3.188 Z-.0556 R.0556

But this is where my question arises. If I put the above code with the No.1 nose radius into G71 (where a No.2 nose radius is used), will it overcut my part? My wish is to put this code into G71 so the G70 with the No.1 nose radius will read it and finish the part, but I am afraid that my part may be overcut from the No.2 radius in G71. Is this true? If it is, how will I get around it?

Would the solution be to incorporate the No.2 radius into the G71 code and then not use G70, instead opting for G01 moves with the No.1 nose radius to finish the part?

Sorry for the long post. I am just confused and need help. If there is a better way you guys do this, please chime in

Thanks,

Chris

The no.2 tool will leave additional stock running on chamfers and radii. Imagine putting the tool in a corner, the large nose radius tool will not reach into the corner as far as the sharper nose radius tool. When programming without G41/42 the path will run the corner of the box. Turning and facing will not be affected, however tapers will come out oversized, radii and complex(non-cylindrical) shapes Will come out distorted.

Can you just write straight g-code on this Jap abortion ?

If so, then it's simple. Draw up your part in a quick 2d program. Now make lines parallel to the finished dimensions, offset by the radius of whatever tool you will use. For me that was usually .0312".

At tangencies, where the lines go around corners or tapers, add arcs to connect. For burr-free parts you want the tool to never leave the part surface. Think of it as a circle rolling along the part surface. No hop, skip, or jumping allowed. Even a sharp corner would have a radius (.0312" if you use xx2 inserts) defining it.

Now pull the dims and bob's your uncle. You don't need any weird-ass "help-you" crap that just makes the whole process more complicated.

I usually DON'T use cutter comp on rough passes. So when I rough out a part using the cycles I leave .005/.01 for finishing.

For an OD:

X3.25 Z.12
G71 U.062
G71 P1 Q2 U.01 W.005 F.008
N1 G0 X2.75
G1 Z-.75
N2 X3.25


For an ID:

X1.25 Z.12
G71 U.05
G71 P1 Q2 U-.01 W.005 F.008
N1 G0 X2.875
G1 Z-.625
N2 X1.25

Then call up a finish tool and profile accordingly. The newer Fanuc controls will not even allow a G41/G42/G40 within the cycle anymore.

cgrim3 said:

G00 X3.076 Z.050
G01 Z0. F.005
G03 X3.188 Z-.0556 R.0556

But this is where my question arises. If I put the above code with the No.1 nose radius into G71 (where a No.2 nose radius is used), will it overcut my part? My wish is to put this code into G71 so the G70 with the No.1 nose radius will read it and finish the part, but I am afraid that my part may be overcut from the No.2 radius in G71. Is this true? If it is, how will I get around it?

Click to expand...

Hello Chris,


Your Code example when using G42, shown below, indicates that you're using G71 Type 1 and therefore the part profile must have monotonous direction moves, ie. no concave features anywhere in the profile.

G00 X4.65 Z.05
G71 U.065
G71 P101 Q102 U.004 W.001 F.008
N101 G42 G00 X3.108
G01 Z0.
G03 X3.188 Z-.04 R.04

In your second example shown below and assuming that the G00 X3.076 Z.050 block is your "P" referenced block, indicates that G71 Type 2 is used and therefore, your part profile may have non-monotonous moves downstream of the code you have listed.

G00 X3.076 Z.050
G01 Z0. F.005
G03 X3.188 Z-.0556 R.0556

1. In the case of a part profile where the moves are monotonous in direction and a larger TNR is used to rough the part profile that is specified with the geometry to suit a smaller radius, then no over cutting will occur; in fact, on all radius and angle features, more material will be left than if the TNR that the geometry of the part profile was created for had been used.

2. In the case of a part profile where the moves are non-monotonous in direction where the profile contains concave features and a larger TNR is used to rough the part profile that is specified with the geometry to suit a smaller radius, then over cutting will occur on elements of the profile that are cut with the trailing edge of the insert, and grossly so.

So you can use the part profile description that incorporates the compensation for a smaller TNR than will be used to rough with and have no over-cutting, but only if the profile is monotonous in direction.

Regards,

Bill