Boreing Holes ?

There must be a better more automatic way !

I have a lathe, that I love dearly, I have added stepping motors to it so it's kinda CNC however one of the tasks I do is to use the dead center & manually drill a hole so that a boring bar can be used to bring it out to the required size.

I want to combine both steps into an automatic cycle, that runs without me turning the wheels.

My thought was to mount the drill bit on the carriage, lets call it a 1/2" drill bit 6" long. About 1" down from the cutting end, Tig weld a piece of HSS in the flute, sticking out maybe .050" as the drill enters the material " usually 2" aluminum 3 to 5 " long." After the first inch the HSS will also start cutting & opening up the hole further. Then pretending this is also a boring bar keep making passes until the desired ID is reached.

I assume that a drilling or pecking cycle would be used to get the bit through & keep the chips out.

What method do you use? Is there a tool for this kind of work?

I'm not concerned about speed, even .010" cuts as long as I can walk away are fine.

Helpful hints from real machinists are most welcome.

Thanks for listening

Peter

Reply to
Peter Kiproff
Loading thread data ...

formatting link

They make good tools for the job. I sell and service them if you need one.

Gunner

Liberals - Cosmopolitan critics, men who are the friends of every country save their own. Benjamin Disraeli

Reply to
Gunner

Gunner, we just bought a used GT 75 and got it set up and wired Wednesday. Came with a CNC Enhancements Hydro-turn bar feeder. First off, it had a bad fan in the controller power supply, and would error out the servos randomly as to X or Z. I took it apart and found the bad fan, replaced the fan, and it seems to run ok now. I felt right at home in that thing, being it's PC based. It ran cutting air all day Thursday without missing a beat. We normally run Brownies and Davenports, so this will be a new adventure for us. Any hints to stay out of trouble? Other than education?

RJ

Reply to
Backlash

Thank you for the link Gunner, nice looking machine. Is there a standard tool that can be used on a regular lathe?

or should I try to make a combination drill / boreing bar?

Peter

Reply to
Peter Kiproff

The only comment I could make here is, the fastest way to get fired from a CNC shop is to walk away from a machine while it's cutting. That was a real no-no in the place I worked.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Reply to
jim rozen

======================= Things change. These days, *many* CNC shops set up jobs that run all night unattended.

Joe

Reply to
Joe Way

Since it's Aluminum, you might get away with drilling a pilot hole and then a

2-fluted endmill used as a boring bar. Make sure you mount it so that the flutes are on center at the cutting edge.
Reply to
Matweier

There's a tool called a "K" drill or indexable drill. It has carbide inserts in the face. It requires no c-drill or spot. It also bores. Expensive though. It's a great tool.

Reply to
Matweier

Thank you Matweier

That's the kind of thing I'm looking for.

I think I've seen a flat drilling insert on the end of a holder, If the insert was wider than the holder it may just work.

Peter

Reply to
Peter Kiproff

Huh. What kind of place did you work in? The places I worked (Gear shop, mold shop) were exactly the other way. Once a program had run once without crashing, it ran unattended except for part changes, tool offsets, or whatever. Wasn't uncommon to have one person on two or three machines.

Chris The correct way to punctuate a sentence that starts: "Of course it is none of my business but--" is to place a period after the word "but." Don't use excessive force in supplying such moron with a period. Cutting his throat is only a momentary pleasure and is bound to get you talked about.

Reply to
Chris Cox

Nonsense ---I have 23 cnc machine that run nites and week ends with NOBODY in the shop Ray Mueller

Reply to
SMuel10363

Never had one of them crash? As I said, in the shop I worked in, the rule was when you were working one machine, you did not setup, run, or clean out another. The consequences of a crash there was devastating, and an observant operator could and did stop problems all the time before they became "machine down for repair, for a week."

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Reply to
jim rozen

No. For what you want..you need the whole machine.

Thats why CNC is so popular. You program the cycle and load the part and press Start. It does all the cutting and pecking and turning and whatnot without touching a thing during the cycle.

The closest tool to what you want that can run on a regular lathe is a CNC retrofit attachment.

Of course this can be done with air logic, or punched tape drives or microswitches or even cams and clockwork. But there is no easy way to do it yourself.

Hardinge AHCs are around a $1000 if you want to start out cheap.

Gunner

Liberals - Cosmopolitan critics, men who are the friends of every country save their own. Benjamin Disraeli

Reply to
Gunner

Unless you are tending the other 3 machines in the cell. Or its a 'lights out" operation, or you are bar feeding, or...

Depends on the shop, the job, etc etc. Most places the folks dont leave the machines simply because cycle times are so short that they have to keep feeding the machine to keep production up.

Chuckle..lots of shops I work in..have a card table in the middle of the shop. They play cards, etc etc. But they always are listening.....

Gunner

Liberals - Cosmopolitan critics, men who are the friends of every country save their own. Benjamin Disraeli

Reply to
Gunner

Lots of them. First of all is my cell phone number. 24/7 feel free to call.

805-732-5308. Ive got free incoming so call as long or as often as you like.

where are you located and when do you have your training scheduled for?

Hardware stuff...hummm make sure your encoder belt is in good condition. If you are going to be doing a lot of threading, get a spare belt. Call me or the factory. If the belt breaks..it wont thread. Period. They are like $12 or so. Inspect the pulley on the encoder and the spindle. If the encoder pulley is plastic and the machine is over 3 yrs old, order another pulley. Get the aluminum replacement. Its about $32 or so. And dont wear out.

Is this a C axis machine or a regular 5hp analog machine?

First big thing to remember about the OmniTurn..is it uses 'closest moves" Unlike a turret lathe, this gang tooled machine will make a move at a straight line. from one location to another. There is no pulling back, moving over. then back in with the next tool. If the next move happens to be though the next tool sticking out...your gonna bust a tool . Unless you program it to move out, and around.

A good thing to do, when writing your first program, is put on paper, the order in which each tool is gonna be called up. Then put them on the tool plate in that order. At first, keep them apart a bit, and as you start getting comfortable with the machine..then you can close them up.

300 IPM rapids dont leave you much time to hit the E stop if you missed a decimal point.

Atter writing your first program..or even on a turn key program, :

in Automatic mode: Load your program Press F4 (verify program) it will then give you estimated cycle time, then a menu choice of how to display the tool path. single step though the program, watching each move on the command line, and the tool path on the graphics. If you see a tool path move through the centerline of the part without being away from the end of the part..thats called a crash. Fix that. Continue till all booboos are fixed.

Remember..the machine will program in radius or diameter mode. Diameter mode is easiest, and you can program directly from the keyboard with a print in your hand.

First line is ALWAYS G90G72G94F300 G90 (absolute mode) G72 (diamter programing) G94(inches per minute) Feed Rate of 300 IPM

Dont try to cram as much stuff on a single line as you can. That way is madness when trying to debug a program.

Most modes are Modal. When you turn them on..they stay on until you either change it, or turn it off. Our first line set all rapids at 300 Ipm..they stay that way until you make another G94F100 (example) Fast is good. Fast up close to a part is bad. Dont make a 300ipm move to .001 from the part. The machine will handle it. It makes a difference if your part is long or short or out of size. Often this means a new insert.

G95 is inches per Revolution. This is good when you are up close and of course this is your cutting feed rate. Come up to .01 in rapid, then change to a G95F.006 (example for most steels) and make your cut. Pull out a couple thous, change to G94Fxxx and move to the next tool, or stay in G95 if you are making another feature with the same tool. You can change the feed rate at anytime..by simply calling G95F.xxx

When making a tool call T2 (example), remember that the NEXT line has to be a x or z move. It will error out and warn you as it prechecks the program before running. Usually. Almost always. 99% of the time.

There are lots of short cuts you can do..but when you are first starting out...dont get in the habit of using them as the next poor bastard who has to edit your program may not be as sharp as you and will take twice as long to figure out what went wrong.

Using a line per statement will not make the part run any slower and makes the editing go easier. Notice..there are no line numbers used.

Avoid long comment lines (Drill .045 at #3% for ABC Company 1-23-2004) NO punctuation in comment lines! It may run fine for months then go bonkers. If its on the top row of your keyboard..dont use them! decimal points and numbers and letters only! I make money on people who forget this and suddenly the machine nuts up. Usually will not break anything..but sizes get bigger and smaller, etc. It Will drive you nuts

Before running your first program..insert G10 z-3 in the second line of your program. This is called Work Shift. This means you run the whole program, but the tools are all offset 3" away from the part in Z axis. This allows you to watch where everything is going, without busting anything You can change that 3" to anything your little heart desires..just as long as its longer than the longest tool you have sticking out .

Before hitting the Start button on that first part...in automatic mode, with your program loaded..hit F10. This pops up a menu. Press F2 for

20% feed rate override. Hit escape.

You will now notice your feed rate is showing 20% up in the u pper right side of your screen. Every thing moves nice and slow from the very start of the program rather than the full 300 IPM. During a cycle..those F keys also work as feed rate override..F8=80% etc...EXCEPT during a canned cycle. So start slow. Hit S for single block, then with your tounge clamped firmly in the proper corner of your mouth, press the Green Start button, with your hand close to the Red Motion stop button. This is the final check of your program. It will slowly move through each line, with you hitting the cycle start button for each new line. With that work shift..you will not hit anything before you can kill it. If something looks like its gonna hit, hit motion stop, escape, and then go in and edit your program.

When every thing looks hunky dory, F10, F10 (full 300 IPM) and escape, Hit A for automatic, and hit the green button.

Yeehaw!!! Full bore, balls to the wall. If it still looks good, edit your program, remove the G10 work shift and run a part.

Measure each feature carefuly. If its too big or too small, look at which tool is making that feature, then go into F2 (offsets) and inter the amount its off. If its .003 too big in X, enter -.003. If its too small, enter .003. then hit enter or change the Z +/- and go on to the next feature/tool. Remember..tool 3 is offset #3, etc. You have 32 offsets to work with. Each phyical tool can have more than one tool number (more on that later ( chuckle)

Another thing to remember..if you are working on the back side of the part..or the far side of the centerline..lets say with a grooving tool, your x moves are in - numbers. This is REALLY important when you set your tools initially. I assume you have the manual? Read the section on touching off your tools carefuly. Then again until you are sure you know how it works.

OmniTurn has some really super tooling that allow two tools to be on the same holder, just opposite sides of the bar..really saves space and time. But they can screw you up if you use one on the far side of the centerline if Id boring if you didnt touch them off right from the start.

Hell..I can teach the class..but suspect my fingers will cramp before we get to constant surface feed LOL.

If you need any questions answered, feel free to call me

And good move. The GT75 is a good machine.

Im in So. California btw and service most of California, Aridzona and where ever you will pay me to fly.

Another good site is one I wrote much of, before going independent is

formatting link

Drop me an email with any questions about who/what/when/how or why.

Gunner

Liberals - Cosmopolitan critics, men who are the friends of every country save their own. Benjamin Disraeli

Reply to
Gunner

They are generally not adjustable in diameter (some very expensive ones are) and require a pretty rigid machine to run one.

Gunner

Liberals - Cosmopolitan critics, men who are the friends of every country save their own. Benjamin Disraeli

Reply to
Gunner

There were a *lot* of part changes, and the parts were pretty oversized for teh machines. Part ripouts from the chucks were not uncommon and could trash a machine in moments. [1] So the rule was that operators had to stand by watching at all times. The cycle times were quite short as well. These were not bar feeder operations.

[1] typical part: ten inch diameter, 14 inch long chunk of nylon, being turned at 3000 rpm.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Reply to
jim rozen

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.