[himatech]

I want to make M60X4 double start thread on SS material on my CNC with Fonuc Oimate
Can any one help me out with programming and tips since I am a bsaic on NC programming

Thanks

[angelw]

I want to make M60X4 double start thread on SS material on my CNC with Fonuc Oimate
Can any one help me out with programming and tips since I am a bsaic on NC programming

Thanks

You're better off posting this thread in G-Code Programming or under the Fanuc forum; you will get more help there.

I can give you the basic way, but this will cut one start completely before starting the 2nd start. The draw back with this method is that the 2nd start is always machined with a threading insert that has more wear on it than it does for the 1st start. If you let me know if your control has the User Macro option, I can show you a method whereby one pass is cut on each start until the thread is finished.

First you need to understand the difference between the Lead and the Pitch of the thread, if you don't already know.

1. The Lead is the distance the thread advances in one 360degree rotation.
2. The Pitch is the distance from the point on one thread, to the corresponding point on the next thread. For example, the distance from the crest of one thread start to the crest of the next thread start.
3. The Lead is calculated by multiplying the Pitch by the number of starts.
4. The Pitch is calculated by dividing the Lead by the number of starts.
5. The Thread Lead is used as the Feed Rate in the threading cycle
6. The thread Pitch is used in calculating the depth of thread.

You write the threading cycle as if you were cutting a single start thread, but the full depth of thread will be calculated using the Pitch of the thread in the calculation and the Lead, or twice the Pitch will be used as the F value in the threading cycle.

When the first start is finished, you move the position from whence you started the threading cycle for the first start, by an amount equal to the thread Pitch. Lets say that the you started the thread cycle with the tool at Z5.000. If the Lead is 4mm and therefore the Pitch will be 2mm, then after the 1st start is finished, the threading tool is moved to Z7.000 and another threading cycle using the exact same inputs is programmed to cut the 2nd start. If it were a 3 start thread then the 1st start would be cut starting from Z5.000, the 2nd from Z7.000 and the 3rd from Z9.000

Post back if you want any further information, or if you post the major and minor diameter you plan to machine the part to,I'll give you example code for the threading part of your program.

Regards,

Bill