Keep tool down in drilling cycle

[randommachinist]

Hey guys, very new to mastercam here and new to the forum also. Anyways, I have a 4.250 dia. hole that I have to bore out. Basically, I want to bore this hole 1.5 inches deep, have the tool dwell momentarily, and then stop. I do not want the tool to retract out of the hole, I prefer to do it manually. What's the best way to go about this in mastercam?

[soymilk]

if this is something you are going to do on a regular basis, then I would consider using a custom drill cycle.  If its a one time deal, i would just Gcode it.  

[duckdogers]

do you have to bore it(assuming your using a boring bar).I would helix bore then clean up with a new end mill

[randommachinist]

yes, I'm using a boring bar. I can also adjust it to whatever ID size I need to bore. So I was hoping to stop the program at the bottom of my cut, then adjust the boring bar so the insert doesn't drag on the walls when it retracts.

[BenK]

Using a boring bar I would stop and orient the spindle than shift it .005" in the appropriate direction than retract. No need to adjust the bore smaller just to retract. Also this can be done fully automated so there is no operator involvement. You would have to create a custom drill cycle for this if you do it a lot. Otherwise just hand edit it. 

 

Or you could just use the bore cycle that feeds in and out. That way you wouldn't have to make a drill cycle or hand edit anything.

[randommachinist]

Thanks for the replies guys. I just went in and hand edited the program. I'll have to try a custom drill cycle program next time and see if that works.

[MIL-TFP-41]

Point toolpath would work nicely for this.

[soymilk]

Does the machine have a fine bore drill cycle?  Its normally G76 on fanuc machines.  If so, then you should be able to use the Fine Bore drill cycle in mastercam.

 

If this is a fanuc machine, Just make sure the retract orientation is set up correctly in the parameters for the machine.  Parameter 5101 bit 4 and 5.  

 

 7 6 5 4 3 2 1 0

X X 0 0 X X X X        Retracts X+

X X 0 1 X X X X        Retracts X-

X X 1 0 X X X X        Retracts Y+

X X 1 1 X X X X        Retracts Y-

 

Gcode Cycle syntax should look like this = G76 Z [Depth] R [Feed Plane] Q [Retract Amount] F [Feed]

[FROZEN]

I use G76 on the Makino, or Feed in and out G85 for tool pressure.