Rough boring parallel to taper.

I am boring a long taper and I would like to have my roughing passes parallel with the taper as apposed to parallel with the OD. Would this be a good application for a G73? Any help would be great!

lstewart3 said:

I am boring a long taper and I would like to have my roughing passes parallel with the taper as apposed to parallel with the OD. Would this be a good application for a G73? Any help would be great!

Click to expand...

Presumably you will be starting with a hole the sides of which are parallel; drilled hole for example. In this case, G73 will be very inefficient, as shown in the attached picture. The steeper the taper, the more inefficient of course.



Regards,

Bill

Cant you just include a x#.###+/-.#### in a g71? Or in a type 2 g71?

Sorry i meant x0.00 u+/-.0000, i was in okuma land there

james siffel said:

Sorry i meant x0.00 u+/-.0000, i was in okuma land there

Click to expand...

Hi James,
G71 cycle will still rough parallel with Z axis, irrespective of the profile shape, as shown in the attached picture.



Regards,

Bill

lstewart3 said:

I am boring a long taper and I would like to have my roughing passes parallel with the taper as apposed to parallel with the OD. Would this be a good application for a G73? Any help would be great!

Click to expand...

Is this so the last few passes are more predictable? In that case for speed you could run a regular boring cycle and leave enough for, say 3 finish passes to follow the roughing cycle

Use the G71, either the 1 line version or the 2 line version.
Its simple and should do the job fine.
Example for a G71:
The G71 turning-boring cycle:
This is a simple example, it turns a 4" diameter piece of 1018 steel down to a 2" diameter, 1" back from the face of the part.

O1000(Program number)
N1 G50 S2500(Max speed)
N2 T0101
N3G96 S600 M3(Speed in SFM for 1018 Steel)
N4 G0 X4.0 Z.1 M8(Rapid to OD of part, .1" away from face, turn coolant on)
N5 G71 U.15 R.02(U=cutting depth, R= pullaway distance after each cut)
N6 G71 P7 Q9 U.05 W.005 F.015(P7 tells the control to look at N7 and Q9 to look at N9, this is how we give the motions describing the part.
U is the amount of stock left for finishing on the OD, W is the amount left on the shoulder.
N7 G0 X2.0
N8 G1 Z-1.0
N9 X4.0
N10 G0 X6.0 Z6.0 M9(Rapid back to a position clear of the workpiece)
M30
Good luck, there are more examples on my website:
doccnc.com
Heinz.

Well I suppose you could just hand code it if need be but if you are going to go the G71 way I would try to use TYPE2 rouging if you have it available. So like in Heinz example...

Heinz R. Putz said:

O1000(Program number)
N1 G50 S2500(Max speed)
N2 T0101
N3G96 S600 M3(Speed in SFM for 1018 Steel)
N4 G0 X4.0 Z.1 M8(Rapid to OD of part, .1" away from face, turn coolant on)
N5 G71 U.15 R.02(U=cutting depth, R= pullaway distance after each cut)
N6 G71 P7 Q9 U.05 W.005 F.015(P7 tells the control to look at N7 and Q9 to look at N9, this is how we give the motions describing the part.
U is the amount of stock left for finishing on the OD, W is the amount left on the shoulder.
N7 G0 X2.0 W0.0 (NOTE)
N8 G1 Z-1.0
N9 X4.0
N10 G0 X6.0 Z6.0 M9(Rapid back to a position clear of the workpiece)
M30
Good luck, there are more examples on my website:
doccnc.com
Heinz.

Click to expand...

Hey, i was thinking about this, i have absolutely done what your saying on okumas lap cycles. I dont see why fanuc cannot handle it. G71 type 2, add the z or w move like the other guys said, you should be golden

james siffel said:

Hey, i was thinking about this, i have absolutely done what your saying on okumas lap cycles. I dont see why fanuc cannot handle it. G71 type 2, add the z or w move like the other guys said, you should be golden

Click to expand...

Hi James,
I agree with you that using G71 Type II would be the choice of Roughing Cycles to use, but if the OP wants to have the roughing cuts from start to finish parallel with the finished tapered surface, G71 Type I or II will not do this. Once the cutting path starts to intersect with the Taper, Type II will follow the Taper from the finish point of the current roughing cut to where the previous cut intersected with the Taper, but predominately, the roughing cuts will be parallel with the Z axis.

The OP doesn't give the Make or Model of the control, but if its a Fanuc pre 2 Block G71 Format, or a later control set to FS15 Format, then a Semi Finish cut, as well as a Finish allowance can be specified. In this, an amount for a Semi Finish Cut is left during roughing, and a Finish Allowance is left after the Semi Finish pass is made.

Regards,

Bill

Your right Bill, maybe he could create a custom macro for this, any takers?