SL-35 MF-T4 Threading

[kato]

Hi,
I want to perform a thread: M48x5 with modified flank infeed. And I have only used G76 in the past.
Sandvik gave me this information:

Threading OD Metric 60°, P=5 mm/thread
(D2,d2): 48 mm
(P): 5 mm/gänga
Leads: 1
(Ph): 5,00 mm/r
Angle: 1,9 °
(vc): 110 m/min
(n): 729 varv/min
(nap): 13
(ap): 3,05 mm

Inmatningsserie
passerinsteg ackumulerad
[mm] / [Tum] [mm] / [Tum]
1: 0,48 / 0,0189 0,48 / 0,019
2: 0,40 / 0,0157 0,88 / 0,035
3: 0,37 / 0,0146 1,25 / 0,049
4: 0,28 / 0,0110 1,53 / 0,060
5: 0,23 / 0,0091 1,76 / 0,069
6: 0,21 / 0,0083 1,97 / 0,078
7: 0,19 / 0,0075 2,16 / 0,085
8: 0,17 / 0,0067 2,33 / 0,092
9: 0,16 / 0,0063 2,49 / 0,098
10: 0,15 / 0,0059 2,64 / 0,104
11: 0,14 / 0,0055 2,78 / 0,109
12: 0,14 / 0,0055 2,92 / 0,115
13: 0,13 / 0,0051 3,05 / 0,120

Can anyone help me make this part of the program?
/Jim

[fordav11]

I had to look up 'modified flank infeed' to see what you meant. hehe!

you can do it with G76

G76 X41.506 Z-50.0 I0 K3.247 D250 F5.0 A60

The A is the thread angle so if you want to feed in a metric thread at 1 degrees less than the flank angle use A62.
Hmmmmm..... or maybe it's A58. It's one or the other

If your control needs 2 lines for G76 then use this one...

G76 P030060 Q250 R0.05
G76 X41.506 Z-50.0 R0 P3247 Q500 F5.0

On the 1st line P = number of finish passes (first 2 digits), threading chamfer amount (second 2 digits) and thread angle (third 2 digits... use 62/58 here)
Q = depth of roughing cuts (no decimal point allowed)
R = finishing allowance

On the 2nd line P = Depth of Thread and Q = Depth of first cut (no decimal point allowed for P or Q)
R = Taper amount in X.


However if your tool is 60 degrees and you feed in at a lesser angle the whole tip will cut on the side on the last cut with a really big cut (2 degrees). you really need to just feed in at 30 degrees (i.e. use A60)

Don't listen too carefully to what tooling sales guys say about that kind of thing. I get tooling guys tell me all kinds of bullsh*t. I filter it out, extract the protein and then toss whats left over down the toilet. then I do it my way

Also remember we speak mostly English here, the Swedish text doesn't make much sense even using Google Translate.....
input series passerinsteg accumulated and tum is inches. I assume 'passerinsteg' means depth of cut

If you really wanted to use that data you can do something like this (below) to control individual cuts as per your data but you won't get a modified infeed because using G92 you have no control over the infeed angle.

G0 T0101
G97 S300 M3
G00 X50.0 Z5.0 M8
G92 X47.04 Z-50.0 F5.0 (48 - 2*0.48)
X46.24 (= 48 - 2*0.88)
X45.5 (= 48 - 2*1.25)
X44.94 (= 48 - 2*1.53)
X44.48 (= 48 - 2*1.76)
X44.06 (= 48 - 2*1.97)
X43.68 (= 48 - 2*2.16)
X43.34 (= 48 - 2*2.33)
X43.02 (= 48 - 2*2.49)
X42.72 (= 48 - 2*2.64)
X42.44 (= 48 - 2*2.78)
X42.16 (= 48 - 2*2.92)
X41.9 (= 48 - 2*3.05)
G00 X200.0 Z200.0 M9
T0100 M5
M1
M30

well you *could* control the in-feed angle by doing something like this....
G92 X47.04 Z-50.0 F5.0 (48 - 2*0.48)
G00 W-0.1
G92 X46.24 Z-50.0
G00 W-0.1
G92 etc

But then it gets very messy because you're moving incrementally in Z to shift the start point and it's very easy to completely corrupt the proper thread profile without special care and special programming. Not for the faint-hearted

also technically the depth of thread is not right because for metric threads the depth of thread = 0.6495 * pitch.
which equals 3.247mm for a root diameter of 41.506mm

Using G76 is the best option. If your control has it there is another letter you can stick on the G76 line that makes the tool do zig-zag in-feed. So it cuts on the left side for one cut then the right side for the next cut and so on. that can help for deep threads but it might have been Fanuc 15/16/18/21 specific (you have an 0-TC which is your MF-T4). In this case, you must use the Fanuc 15-series format (one G76 line) and set parameter 0001 bit 1 (FCV) to 1. The G76 would be....
G76 X41.506 Z-50.0 I0 K3.247 D250 F5.0 A60 P2
The P2 tells it to zig-zag on in-feed.

Depending on the size of your machine and it's rigidity a 3.247mm deep thread is not really very difficult to cut using a regular G76 with normal in-feed