What's new
What's new

Emco lathe thread programming for Fanuc 31i

ChrisC_84

Plastic
Joined
Apr 4, 2020
Location
UK
I really hope someone can help with this because it's really holding me back.
I have to write a report on a turning project I was given at college as part of my machinist apprenticeship. One of the features of the part was a short threaded section with an M8x1.25 thread to be cut onto it. I am having difficulty in particular with a couple of the parameters on the 'THREADING(OUTER)' cycle. Can anybody explain to me the 'CUT TYPE' (S) Cut Number and Cut Depth parameters please?
The manual says that the CUT NUMBER parameter option is "Number of cuts for thread roughing". Am I correct in thinking that the total thread depth is divided by the number you input here?
The manual also says that the CUT DEPTH parameter option is "Cut depth per thread roughing process (radius value, positive value). The number of cuts is determined by the cut depth and by the machining method". I can't work out what this does.
Thanks in advance
 
Number of cuts is just that, the number of cuts it will take. Cut depth I believe is only good for the first pass. After that the machine calculates the depth of cut for the remaining passes depending on the number of cuts you told it to take.
 
I really hope someone can help with this because it's really holding me back.
I have to write a report on a turning project I was given at college as part of my machinist apprenticeship. One of the features of the part was a short threaded section with an M8x1.25 thread to be cut onto it. I am having difficulty in particular with a couple of the parameters on the 'THREADING(OUTER)' cycle. Can anybody explain to me the 'CUT TYPE' (S) Cut Number and Cut Depth parameters please?
The manual says that the CUT NUMBER parameter option is "Number of cuts for thread roughing". Am I correct in thinking that the total thread depth is divided by the number you input here?
The manual also says that the CUT DEPTH parameter option is "Cut depth per thread roughing process (radius value, positive value). The number of cuts is determined by the cut depth and by the machining method". I can't work out what this does.
Thanks in advance

Hello Chris,
You need to specify the Threading Cycle you're referring to; ie. G76, G92 etc. You make reference to The manual says that the CUT NUMBER parameter option is "Number of cuts for thread roughing".. I've never seen that statement in any Fanuc Manual.

With the Multi-repetitive Threading Cycle G76, there are two parameters that influence the number of cuts that are performed during the execution of roughing part of the Cycle; they being:

1. The Minimum DOC specified in the First G76 Block (Standard FS16 Format - default for the Fanuc 31i control)

and

2. The DOC for the First Pass of the Threading Cycle

Each successive DOC is calculated using the following algorithm:
DOC = d x SQR(N)
where:
d = DOC specified for the first Threading Pass in the second G76 Block
N = the Nth number of threading pass (1,2,3,4, etc)

The DOC for each successive pass is determined in this manner until the difference in DOC between the current calculated DOC and previous calculated DOC is =< than the specified Minimum DOC. From that point on, each DOC will be incremented by the Minimum DOC specified until the X Coordinate (Minor Diameter - Male Thread) specified in the second G76 Block is reached.

As you can see from the above, the smaller the value specified by the Minimum DOC parameter, the greater the number of Threading Passes.

In theory, if no Minimum DOC was specified, the tool would never quite get to the X coordinate specified. However, the Least Programmable Increment of the control will circumvent that happening. Its like the two Uni Graduates at the graduation party, one a Pure Math Graduate, the other a Mechanical Engineering graduate and each sitting a reasonable distance from a cute girl. Each had the strategy of halving the distance between themselves and the girl every half hour. After the first hour, the Math Graduate gave up considering that he was never going to get there. The Mechanical Engineering Graduate persisted, having the thought that he would get close enough for practical purposes.


Regards,

Bill
 
this sounds like an emco specific cycle they wrote, that follows along the siemens route. If I can remember correctly the cycle is going to have

thread type (1-4) and would be like inside or outside and constant infeed depth or constant volume or something like that

starting and ending x and z, along with runin and run out distances

thread depth / number of cuts, infeed depth calc'd by constant depth or volume / idle passes - spring cuts

infeed angle - and if you used a negative it would alternate leading and trailing edges

starting point angle - 0-360degrees

amount to leave for finish cut, not sure if it leaves that amount for another tool if you want or leaves that amount out of your roughing cycle for a finish pass within the current cycle and tool
 
Thanks for the input everyone.
pcasanova would appear to be right. It would seem to be an Emco specific threading cycle as it inputs two lines of code after specifying the parameters:
G1140 W2. B1. C0.08 K8. S1. P12. Z22. D1. L1. M1. Y1. ; <- This would be the Emco 'THREADING(OUTER)' cycle
G1461 W1. D8. Z-4. L1.25 M8. H0.767 C2. P1.25 ; <- This would be the Emco 'ZX-THREAD(METRIC)' cycle
TBH I would have preferred the more usual G76 threading as angelw described. I would have thought it would make more sense to train apprentice machinists in the more usual programming methods rather than manufacturer specific programming cycles.
We got there in the end though. Thanks again.
 








 
Back
Top