Now I have some tooling and want to start doing some threading on the new toy. Bridgeport Romi Centur 35.
Fanuc 0T control.
Any recomendations for cuttting some ID and OD NPT threads.
Remember I'm a greeny on a lathe.
I have been messing around a little but would like to avoid the hard lessons.
If maximum production is an issue then you really don't want to be single pointing any pipe threads for average applications. Taps and die heads will produce the most parts with the least headaches for pipe sizes of 1/2" and under.
The sizes that I am interested in are 1" and up. The ID thread is 1"npt. While we can tap it. It takes alot of torque for a somewhat delicate part. So single point seems like the best bet.
I'd suggest that you get VERY familiar with the Fanuc G76 threading canned cycle. A full description is in the Fanuc operator's manual.
With G76, you make all the threading passes with a one-block command. There are other "single pass" threading commands, but with these you have to manually program each pass. G76 will make a sequence of passes, and will finish the thread with a final "Finishing pass", all automatically. The G76 cycle also lets you specify the angle of the tool, so it can cut each pass so the chip is always on the same side of the tool.
Some small hints:
Start the threading cycle with the tool far enough away from the part so the Z axis servo has enough time to accelerate up to speed. Starting too close can cause small thread pitch errors on the first thread. Usually, .100 inch is enough.
Don't use CSS (Constant Surface Speed) while threading a taper. The spindle speed will change during the cutting pass, and the Z axis may not follow the speed increase exactly. CSS is turned off with a G97.
Make sure your spindle encoder is working properly. Most encoders are belt-driven off the spindle shaft, and these belts can get worn or loose. The spindle encoder has a "1-pulse per revolution" signal that triggers each threading pass. With a bad encoder, the G76 threading cycle may not work at all, or the pass may not line up with the previous passes.
You did not mention the material you'll be cutting, but as Fritz said, G76 is your friend in most cases.
Get familiar with your control, as some machines treat the D value differently. Also, depending on your machine the finish pass and min. cut depths may be settings controlled.
I'd say turn the OD on a few parts, and then start threding them with different G76 values and see what happens.
The parts are cast aluminum.
I will likely experiment with wood to start. Much easier on my tooling when I make a mistake.
No offense, but please tell me you didn't get your tooling from Toys-R-Us?
Cast aluminum, hell use that piece wood to thread it with.
As for making a mistake, nothing beats a chrash early in the learning curve to teach you to ALWAYS!!! dry run everything first.
No, I don't shop at toys R US for tools. I buy toys there.
I am a firm believer in dry run also but there is always that first time when things are not as they might seem. So wood is a good place to learn some things. [img]smile.gif[/img]
As for the cast aluminum. Have you machined much of it. Not like your average 6061 T6. This stuff eats tooling. Cuts easy but is very abrasive..
Not much of cast aluminum or cast anything actually, But my guess would be is to reduce the # of passes as much as possible. AL should cut just fine, so make couple of finish passes to reduce the burr, but cutting passes can be deep enough so less cutting passes less wear on the tool.
As for dry run, I actually run the complete program with normal feeds and speeds, no coolant, move Z 1" from the part, and use single step as needed. You can catch about 99% of screwups that way.
R- for OD pipe tapers
R+ for ID pipe tapers
R= amount of taper per side.
Think Snow Eh!
Sounds like a high silicon alloy....about like cutting a combination of aluminum and ground glass.
The silicon content on high Si castings tends to be real high at the surface, so its usually not nearly so bad once you're under the surface a bit.
I'd recommend using ring and plug gages to check your threads, particularly when changing an insert or making any offset change, etc. A fairly small change in the x offset can make the thread engagement too deep or too shallow, and since its tapered you can't check it with wires or a thd mic and learn much about where you are. There's a fair bit of variation in the engagement spec from min to max, so unless you're running something where the designer has called out a real tight engagement depth, your gages can be nothing more than some good quality fully machined pipe fittings as are typically used on hydraulic systems. If the spec is real tight, then the "real thing" thread gages are often required.
We use ring and plug gages now. Boy do they give those things away. Currently we thread mill these puppies. Takes alot longer than single point not to mention needing another machine.
With carbide this stuff is not to bad. But the analogy of ground glass covers it pretty well. Just wears the hell out of HSS.