[Vaughan]

Hi there, I am a new lister with a question.
I am drilling 10,000 deep holes with a .050 peck. Problem is after
retract the drill returns to a level .100 above previously drilled
surface then goes into feed for .150 thousandths so most of my time is not in material removal.

How do I decrease the .100 to say .030 or .050?(G83)
The controller is a Fanuc OM on a Johnford Milling center.

Thanks,

Vaughan

[mtlmnchr]

look in the CYCLES TO SIMPLIFY PROGRAMMING section of the manual. there will be a G73 cycle . it will give a parameter for gap between return and material remaining. adjust this parameter according to how much room you want. BE VERY CAUTIOUS when adjusting parameters, sometimes they do things you won't expect.

[HuFlungDung]

Hi Vaughan,

I don't have that controller, but would the peck return height exist as one of the parameters in your machine setup? Maybe you can edit the value?

[Rekd]

Or code it long hand..

'Rekd

[Vaughan]

I found a parameter to adjust under "Functions to simplify programming" in the manual(return amount d)

Thanks

[Scott_bob]

Vaughan,

With that many holes to drill, you are on the right track to adjust the "standard parameter" setting...

Be sure to let us all know just how much time you'll save!!!

Check out this thread:

http://www.cnczone.com/forums/showth...&threadid=2459

[Gunner]

Vaughan,
Just a suggestion. If cycle time is an issue I'd do an experiment once you have your canned cycle tuned the way you want it. With that many holes I'd suggest writing the code out. It usually takes more time for the control to read a canned cycle than a straight line program. You may end up getting more holes drilled by the end of the day using the straight line method.

[Vaughan]

Parameter 532 was the one to change. I had first overlooked because the manual associates it with G73 and I need G83. Thanks Scott_bob.

I figure the 20-30 secs saved per hole is worth 60 to 80 hours.

Writing the code with decreasing pecks as the drill goes would save more time. I guess I would post that as a subroutine. But I will do some more drill life studies first

Thanks again

[Scott_bob]

Vaughan,

Awesome, thats what I thought...

So, at a shop rate of $60.00 an hour, you have just saved: $4,000.00

You wanna pass that savings on to your customer, or just keep the money?

[Vaughan]

We are a research facility, so that means we make the next advance in science sooner!!!

[HuFlungDung]

I think a small donation towards cnczone is in order!

[Scott_bob]

Vaughan,

What kind of research?

Don't be shy! Tell us what you can...

[Vaughan]

The National High Magnetic Field Lab
http://www.magnet.fsu.edu/
The parts I am making are end plates for the worlds most powerful research magnets. The holes are for cooling. When these magnets are energized, they consume 10% of the electric load of Tallahassee.

[Scott_bob]

Vaughan,

Wow, that's very attractive...

I used to live in Colorado Springs, CO where the Tesla museum is.
Tesla was a contemporary of Thomas Eddison in the early 1900's.
He too did some strange science stuff...

[Shop Rag]

Vaughn
If you have that many holes to drill why not look at using a carbide drill with through the tool coolant. This would greatly decrease your cycle time and improve your part quality.

[Gunner]

Vaughan,
What type of material are you drilling, how deep do you have to drill or are you drilling all the way through the plate?

[Vaughan]

The material is C36500, a brass alloy with a machinability rating of 60%. The thickness is 1.25 inches with hole dia. .070(#50). Using a Chicago Latrobe deep hole taper drill the hole cycle is about 40 secs.
The hole is through but am milling off the back side to expose the hole to avoid breaking through. I am getting a surprising 150 holes per drill. Did try carbide, but I had breakage and as soon as a drill breaks
I have lost a lot of time. I do not Know if drills with coolant holes are practical with this diameter.

[Scott_bob]

True,

Mitsubishi makes even tiny drills with coolant holes...

[HuFlungDung]

Try grinding a perpendicular rake face inside the cutting edge of the flute. I've found that this works very well for brass in general because of the hogging in effect caused by the spiral of the regular twist drill.

[Vaughan]

Are you speaking of the geometry that creates a split point?