Rapid in and out of deep holes??

[tmalinski]

Being relatively new to Mastercam I’m stumped with what may be a pretty basic task.

I have a milling and drilling repair job that already has a boat-load of 3” dp counter-bored holes in a large steel plate. I need to c-bore all of the holes ½ deeper.

 

I’m using a G83 cycle

My “Retract” height is set to .1 above the stock to clear chips out of the hole as it pecks

My “Depth” is set to –3.5” for the new c-bore depth

My “Top of stock” height is –2.9

 

This is how I thought it should work!

Cutter rapids down inside of hole to top of stock value then cuts using the peck value

Cutter rapids up out of hole to retract value to clear chips

Cutter rapids back to previous cut depth minus peck clearance and cuts again

Repeats this until done!!

The problem I’m having is the tool doesn’t rapid down in between cuts. It starts it peck cycle at top of stock 0,0. This results in cutting air for 75% of the hole depth.

 

Could this possibly be a post issue? Or am I doing something wrong in Mastercam?

By the way, when I mill pockets the top of stock value works properly. It’s just drilling that’s broke!

Thanks for your help

Tom…

[connormac]

What I have had to do is set clearence at .5 or even .1 . then set the retract depth at the same as top of stock at -2.9 . try that and see if it works.

 

kyle

[MACHINEMASTERG]

i would set my r plane to .1 incremental top of stock -3. it wont clear to zo inbetween pecks but it wont cut air for all that time our haas has a setting that lets you add a value to come above the r plane by to do exactly what you want in the settings i would have 3.00 and in between pecks it will go to the r plane plus that value to get it out of the hole !!! what machine are you using and does it have this option in the controller

[tmalinski]

Thanks, I've tried that, but then is it never retracts within the G83 cycle to clear the chips out of the deep hole!!

[tmalinski]

Greg, we have a Fadal VMC. I don't think it will do what yours does

[Surface]

What about using a first-peck and subsequent peck value? If your machine won't suport the code, you could postit long-hand.

[tmalinski]

Thanks Surface, but we are using those values. They control how deep for each peck cut, but not the retract distance for clearing the chips.

[MACHINEMASTERG]

allright already write your own sudroutine and callit at each hole get what you want where you want it

[tmalinski]

Thanks, good idea

[jeff]

If you can't get the canned cycle to work,try using the long form drilling.

Hope you have enough memory in your control.

[Keith Graydon]

tmslinski,

i think that things are working correctly for the G83 cycle that you're running.

 

G83 Rapid to R-plane

peck down value/rapid back to R-plane

Rapid to last peck depth + clearance value

peck down value/rapid back to R-plane

Rapid to last peck depth + clearance value

rinse,repeat.............

 

G83 allways papids and returns to the same R-PLANE, Yes?

 

you're looking for an intermediate step. that I think isn't offered in a std. G83 canned cycle. try another cycle. Perhaps a G73 as "Surface" has mentioned in his post.

 

 

HTH

/KLG

[chris m]

I'm with Greg, write it as a longhand sub and keep calling it

 

C

[TheePres]

Sub is way to go...but Im almost certain that Fadal has drill cycle that allows for first peck to be different than remainder.

[Thad]

quote:

---

Sub is way to go...but Im almost certain that Fadal has drill cycle that allows for first peck to be different than remainder.

---

In a G83, you can also define I (initial peck), J (reducing value), and K (minimum peck.) This is not the most efficient way to do it because you still have to "drill" through 3 inches of air for each hole, but at least you're not peck drilling for those 3 inches. This method gets you drilling material in less time and also clears the part with each peck. I believe it would take a post modification to do this. If it's a rare occasion, I'd just edit the .NC file and run it.

 

Have you considered just using a G73? It's *only* a 1/2 inch deeper. Just a thought...

 

Thad

[Greg Williams]

Tom,

 

Makino use a macro (Visual basic I think) to do this operation. A Heidenhain uses a Q parameter for the same thing, Perhaps Fadal may have somthing similar imbedded into the control.

 

[ 03-14-2003, 05:10 AM: Message edited by: Budgie ]