Newbie- Can Someone help a Threading Newb?

[Orbitalmovment]

I'm trying to figure out how to thread some Aluminum, problem is I've never machined metal and I've never threaded.

I'm trying to figure two block G76 code for M55 x 2.0. I've searched around and got the basic formula for G76 but I really don't understand whats all needed to make it work.

Any help would be greatly appreciated, this is what I have so far;
G76
P
?? - Number of finish passes, not sure how many I need, what is optimal?

10 - One thread pull out at end? I'm not really concerned how the end of the thread turns out or whether this is necessary.

60 - Thread angle or angle of tool bit? Both?.

Q?? - Minimum cutting depth. Not sure what it needs to be.

R?? - More finishing passes? I don't understand the difference between this and first finishing passes.

G76
X55 - I.D. threading so major diameter.

Z-55.8 - Threads 2 inches.

P10825 - Height of thread. Major diameter minus minor diameter,
divided by 2? 55 - 52.835 / 2 = 1.0825

Q?? - Depth of cut on the first pass. I'm not sure what a good first cut would be.

R00 - Taper, I don't need the thread to be tapered.

F.5 - Thread lead, 1 divided by the pitch? 1 / 2 = .5 Is this right?

I'm still searching around trying to fill in the blanks but it looks like some of it needs basic knowledge of machining aluminum which unfortunately I don't have. I also hope I didn't mix metric with standard as I tried to keep it metric.

Again any help would be greatly appreciated, Thanks.

[angelw]

Any help would be greatly appreciated, this is what I have so far;
G76
P
?? - Number of finish passes, not sure how many I need, what is optimal?
Basically it amounts to spring cuts and depends on the rigidity of the part. Normally one finish cut is sufficient. This designation is modal and is not changed until another value is specified.

10 - One thread pull out at end? I'm not really concerned how the end of the thread turns out or whether this is necessary.
More times than not you can set this at 00. This designation is also modals as stated for the previous point.

60 - Thread angle or angle of tool bit? Both?.
This is the angle of the tool tip, or the included angle of the thread. Also modal as above.

Q?? - Minimum cutting depth. Not sure what it needs to be.
As you may have already determined, the control progressively decreases the depth of cut. If no min depth of cut is specified, the depth of cut would continue to decrease to the minimum resolution of the control. Like dividing 1 by 2, and continuing to divide the result by 2, you will never get the answer to be zero. The result will get to a very small number, but it will never reach zero. It depends on the size of the thread. A coarse thread with a large thread depth will have substantial threading insert engagement when approaching full depth and accordingly will struggle with a large depth of cut. Its a bit 'suck it and see'. Too small a min depth and the cycle time will increase due to the many small depth cuts, too large a min depth and the cutting tool will suffer. Start with 0.1mm and vary either way based on observation. This parameter is also modal as above.

R?? - More finishing passes? I don't understand the difference between this and first finishing passes.
This is the finish allowance to be left for the finish cut. For example, 0.1mm can be set for min depth of cut, and will use this value as a min depth of cut until minor diameter for male thread, plus finish cut as specified in R is reached, then the amount set in R, say 0.05 R050 is taken as a finish pass. Modal as above.

G76
X55 - I.D. threading so major diameter.
Correct.
Z-55.8 - Threads 2 inches.
Correct if the end of the thread is Zero.
P10825 - Height of thread. Major diameter minus minor diameter,
divided by 2? 55 - 52.835 / 2 = 1.0825
Correct in calculating the depth based on the Minor Dia given, but the P value would be written as P1083 for metric configuration.
Q?? - Depth of cut on the first pass. I'm not sure what a good first cut would be.
Depends on the size and rigidity of the part. The smaller you make this value the greater the number of passes in the threading cycle as the control automatically decreases this value on each successive pass until the min depth of cut is reached. With an initial small depth of cut, the min depth will be reached at a larger diameter and accordingly, more cuts at min depth will be encountered. Too large an initial cut, the cutting insert and, or the thread may be damaged. On a 2mm pitch thread, and being aluminum, start with a first pass depth of 0.6 and vary based on observation.

R00 - Taper, I don't need the thread to be tapered.
If no taper required, set to 0

F.5 - Thread lead, 1 divided by the pitch? 1 / 2 = .5 Is this right?
This is incorrect. You stated that the thread being cut is M55 x 2.0. Unless the thread is a multi start thread, the pitch and the lead are the same, ie 2.0. Accordingly the F value will be F2.0. In all cases, the lead of the thread is programmed, which is not necessarily the same as the pitch. Accordingly, if the thread is a 2 start thread with a 2.0 pitch then the lead is calculated as Pitch x Number of Starts, in this case 2.0 x 2 = 4 lead; therefore F4.0. You have to be mindful of the rpm, because slide velocity is the product of the programmed lead and the rpm being used. Lets say you use 1500 to cut your 2.0 lead thread; the slide velocity would in this case be 3000mm per min. You must ensure that the resulting slide velocity does not exceed the maximum allowable feed rate of the machine. Also, as the slide velocity increases, error in the lead at the start and end of the thread also increases due to slide acceleration and deceleration. This error at the beginning of the thread can be illuminated by starting further away in Z so that the error due to acceleration is taken up in fresh air.

I hope this answers all you questions.

Regards,

Bill