Fanuc code needs updating.

[Roberts]

I was originally going to title this post "Fanuc...Japanese for Retarded", but I didn't want my frustration of the moment to impugn everything Fanuc has done right.

My two issues are these: Why does Fanuc not have an equivilent of G13/G12 that Yasnac uses? This G code allows you to program an interpolated hole in a single line, with a spiral out, interpolate, spiral in. In our shop we use it a great deal, and now that we have a Fanuc control in the mix, we have to make edits to every single program we run, replacing a single line of code with 5 (!) to do a similar move on the Fanuc. This is pitiful.

Item 2, is the inability of the G76 Thread Cutting cycle to start on lead. In the case of a Swiss machine, where we want to cut a long thread as a series of progressive cycles, there is no provision for starting with an approach on lead. In use, this means the canned cycle destroys the thread at each start point, rendering it useless. The fix is to write a sub program with a conditional branching structure, i.e., a home-made 'canned cycle'. This, again, is pitiful.

Fanuc is a world leader in CNC control applications. It would be wonderful if they would spend a few dollars updating their fundamental CNC code. Why have we not seen improvements in this area?

[Chris D]

Originally Posted by Roberts I was originally going to title this post "Fanuc...Japanese for Retarded", but I didn't want my frustration of the moment to impugn everything Fanuc has done right. My two issues are these: Why does Fanuc not have an equivilent of G13/G12 that Yasnac uses? This G code allows you to program an interpolated hole in a single line, with a spiral out, interpolate, spiral in. In our shop we use it a great deal, and now that we have a Fanuc control in the mix, we have to make edits to every single program we run, replacing a single line of code with 5 (!) to do a similar move on the Fanuc. This is pitiful. Item 2, is the inability of the G76 Thread Cutting cycle to start on lead. In the case of a Swiss machine, where we want to cut a long thread as a series of progressive cycles, there is no provision for starting with an approach on lead. In use, this means the canned cycle destroys the thread at each start point, rendering it useless. The fix is to write a sub program with a conditional branching structure, i.e., a home-made 'canned cycle'. This, again, is pitiful. Fanuc is a world leader in CNC control applications. It would be wonderful if they would spend a few dollars updating their fundamental CNC code. Why have we not seen improvements in this area?

ITEM #1
You may want to check if that option is available for your control model. Fanuc often has plenty of features, it's the machine tool builder that selects which ones to install (and pay for). So, that cycle very well could be available, you just have to pay to have it installed - call Fanuc. Another option is to get the option of MACRO and write your own canned cycles for such things. I have found that having the MACRO option has been much more useful as it allows me to write a "Canned cycle" that can do just about anything I can dream up.

ITEM #2
Not sure at all what you are describing. I have very limitted experience with swiss style machines. Can you explain this again, perhaps relating the difference between threading with G76 on a regular lathe and a swiss style machine. I guess the part that has me confused is "Start on lead", not sure what you mean by this?


COMMENT
The code is all there, they are just options. As such, the machine tool builders select which options they want to put on their machines. So, in many cases where people complain about "Lack of features" on a FANUC control, it isn't Fanuc's fault that the machine tool builder didn't put them in the machine. However, perhaps Fanuc could lower their prices on many of those options too, then the decision wouldn't be so hard for a builder.

Chris

[Roberts]

Thanks for the response.
First of all, Fanuc has no option that performs like a g12/G13 cycle. Nothing even close, and I have talked directly to Fanuc about it. We have written a Macro to emulate the code, calling G113/G112 to replace the code and using the same inputs from that line to populate our Macro variables. F for feedrate, I for circle center, etc. It works, but G12/G13 would be so much nicer. Yasnac probably has a patent on the cycle, but Fanuc should license it from them. It is worth the cost.

Secondly, as threading relates to Swiss lathes, and in the case of a long thread: What you do is turn a short length, thread it, turn some more, thread that, turn some more, thread that, etc. This means you need to be able to come in on lead to pick up the previous thread and continue on. The G76 canned cycle has no provision for coming in on lead. What is does is drop straight down on diameter, and then follow the lead, which destroys the first thread of every fresh start. G76 does have a provision for 'chamfer out', and what it needs is a provision for 'chamfer in'. I have written a Macro for this using G32, but it is a complex and messy Macro, and not very universal as written. I am sure we can solve it, but why wouldn't Fanuc make this simple update?

[Chris D]

Hmm,

I never thought about threading on a swiss style machine, I can see where it is a bit of a problem on long threads. As there are so many swiss style machines out there, I would think that there has to be a workable solution to that - I am just stumped though, sorry. You did well though writing a macro to do it, that had to be pretty tough getting everything to pick up again in the right spot.

By chance, have you asked about this to the applications engineers from the machine tool builder (not Fanuc)? I would think they would have some sort of methods to do what you describe, but I can't come up with anything better than a macro.

[ghyman]

Just today, I threaded a five inch bone screw on a Star SR20R2. And yes, my subprogram is a mess.
Unfortunately, it is not just Fanuc who is lacking in the threading cycle options... Citizen and Tsugami also require a bit of jumping through hoops to achieve this.

On the plus side, I've developed a pretty cool library of "look what I can do!" subprograms over the years!

[chuy]

The canned cycle for the g12,g13 .... I believe is g17 there is a little more involved to programming it. not quite as easy as the yasnac...., but there is one...it's been a while
since i programmed manually....,but i know for fact that there is a cycle for that... your programming manual should say unless you have really old fanuc control...
even still Fanuc control sucks when compared to yasnac...

[oil]

Have you tried useing G32 as your thread cycle. It works great when you have have multiple threads on a part that have to stay in lead with each other. And who uses G76 anyway because you can have more flexability with G92.

[sinha_nsit]

G76 has a lot of flexibility, whereas G92 has none, compared to G76. The only thing is that you should know the exact function of all the parameters of G76.

[sinha_nsit]

Actually, it is recommended that at least 3-4 pitch lengths should be provided as run-in distance before thread cutting starts, to take care of any lag in the machine drive system, otherwise the first few threads may not have correct pitch. So, zero approach angle will not make any difference.

[psychomill]

Write a G112/G113 macro that uses the variables in the same manner as a Yasnac control. Even wrote one years ago that picks up a variable to spiral from "center out" for large diameters.

Everything is so "CAD/CAM" nowadays that the options like these aren't around much or pursued anymore (for Fanuc anyway... as well as some others)

[cogsman1]

Using the G76 is easy but does have its limits, below is a breakdown of the code and how to use it.
On a Swiss you CAN but an extended length "Guide Bushing" which will give up to 1.250" of length to allow for long threads. I use "Thread Whirling" for threads longer than that. Thread whirling is a slower process on short screws but if you need to do the turn, thread, turn , thread etc... it becomes much faster and eaiser to setup.




G76- Canned threading cycle

G76 P010060 Q.002 R.0005 (first G76 sets parameters for threading)
G76 X Z P Q F R (cuts the thread)

The first G76 isn't needed but is recommended.
- G76 P Q R

P010060 sets 3 things
- first 2 digits is the amount of finish passes - 01

- second 2 digits is % of the lead or pullout exiting the thread- 00
00 = almost no angle at pullout and 99 = 9.9 leads away start out

- third 2 digits are the angle of infeed - 60
0,29,30,55,60,80 are usable (0-90 is ok)

Q.005 sets the minimum cut amount during threading

R.0005 sets the cut amount of the last pass

The second G76 cuts the thread.
-G76 X.1876 Z.3 P.0302 Q.01 F.05 (R-.002) FOR 1/4-20

X.1876 =Minor Dia. of thread

Z.3 or (W) =The ending Z of the thread

P.0302 =Height of thread in radius (Maj-Min)/2

Q.01 =Amount of the first cut. All the rest of the cuts are calculated.

F.05 =Feed-rate 20 TPI 1/20=.05

R = R is optional for tapered threading. R is the amount of
difference in X from start to finish in Z. When cutting threads
moving Z and X in a positive direction R is a negative value.

[JonBoy]

HAAS Controls allow settings for either Yaznak or Fanuc.
Get a HAAS.