Threading tapers on Fanuc control or Mitsubishi

[Tyler Durden]

I only know how to thread regular threads with no taper......

G76 P021060 Q0050 R0002
G76 X.92 Z-1.0 R.003 Q.010 F.0625

This is the only way I know how to thread, but now I need to know how to thread tapers. I found an example in a CNC book that goes like this......

For outside diameter taper threads, “I” will always be negative. For inside diameter taper threads, “I” will always be positive.
The actual value of “I” requires trigonometry to calculate. “I” will be equal to the tangent of the taper angle (usually 3.718 degrees) times the overall length in Z of the threading pass. This length must include the approach distance (as in this case, .200)
If for example, your external thread is 1.0” long and you have a .200 inch approach, the value of the “I” word will be -.0779 (Tangent of 3.718 times 1.2)


I know how to figure the "I". But how would I write this? It has a picture example showing K= Thread depth. D= first pass depth.A=angle. It doesn't give me examples of how to write this, only a picture showing what letters represent. I am used to telling how many passes to take but I don't see an example.
From what I understand it is telling me, it should be written like this.....

G00 X4.2 Z.2
G76 X3.826 Z-1.9 K.087 D0160 A60 F.500

How do I tell it how many passes to take if this is how you should write it? Is there more or less I should put in it?

Help please!!!!

[Kiwi]

Tyler

I cannot help with your G76 code. My controller is a Fagor and and don't believe it has a taper thread function.
I have a program that can generate a file with circular point to point coords.
If you want a file advise the Max Dia,TPI, Angle, Length/Depth and Cutter Dia. and I'll generate it for you.

Kiwi

[ErnieD]

Tyler,

My bobcad has the ability to write a program for a tapered thread. If you send the sizes etc. I will try and get you a program. Can you start at the bottom and feed up? If I do this it will be your responsibility to check the code to see if it is ok and to do a trial run in some manner so as to not crash the machine.

Ernie

[gripper]

Hi Tyler
I use G76 for threading on a fanuc machine both parallel and taper. This is what my G76 looks like for a 6mm parallel thread;
G76 P030060 Q75 R.05
G76 X4.773 Z-10. P613 Q100 F1.
And what it would look like for a taper thread
G76 P030060 Q75 R.05
G76 X4.773 Z-10. P613 Q100 R-.15 F1.
The "R" is the amount of taper per side and can be got from any thread tecnical book which tells you thread forms. The above example is not real as I'm at home and doing this from memory. If you want a real example let me know and I'll get it for you. please note that I'm using metric measurments. The example that you show for the book is the old fanuc single line threading and can still be read by some new machines using the 2 line G-code. I have this info some where but it will take a while to find it. The amount of passes is a perameter in the machine.

[Tyler Durden]

Originally Posted by gripper Hi Tyler I use G76 for threading on a fanuc machine both parallel and taper. This is what my G76 looks like for a 6mm parallel thread; G76 P030060 Q75 R.05 G76 X4.773 Z-10. P613 Q100 F1. And what it would look like for a taper thread G76 P030060 Q75 R.05 G76 X4.773 Z-10. P613 Q100 R-.15 F1. The "R" is the amount of taper per side and can be got from any thread tecnical book which tells you thread forms. The above example is not real as I'm at home and doing this from memory. If you want a real example let me know and I'll get it for you. please note that I'm using metric measurments. The example that you show for the book is the old fanuc single line threading and can still be read by some new machines using the 2 line G-code. I have this info some where but it will take a while to find it. The amount of passes is a perameter in the machine.

Yeah that worked, just had to basicly change the R value. Much easier than the nonsense I had in that CNC book. Thanks alot!