[jderou]

We are currently drilling/tapping aluminum with combination drill/tap bits. Spindle speed for drilling is 7400 rpm with feed of 1876 mm/min, tapping speed is 2000 rpm - 5 mm tap. Is it safe to go any faster than this? Max spindle speed is 15000.

I am trying to shave precious seconds off a cycle time, can someone tell me if the following is worth the trouble. When going from one hole to the next, it goes straight up, over to the next, straight down. What if I changed this to make an arc in the vertical plane so that the z axis doesn't have to slow down before the horizontal starts moving. Would this make any difference?

Joe

[ctate2000]

You may want to try a tapping head. The tool change may scare you but reversing the spindle on numerous holes will gooble time. Good tapping head like Procunier will allow you to tap at 2500 and reverse at 2x the cut rate. You go in at 2000mm per min and come out at 4000 never reversing spindle. When you use rigid tapping the spindle probably never makes full programmed rpm anyway so going faster may only tax your drives and screws without producing results. I have tapped 3mmx.5 holes in this way and the machine looked like a sewing machine it was going so fast.

[jderou]

I would agree with you, but they said they tried it and it was actually slower. It actually reverses suprisingly fast, its a direct drive spindle. Think I am going to have to look elsewhere for time.

[ctate2000]

OK...can you give a little more info? Number of holes, distance between centers, other machining operations etc. How many parts on the table? Can you increase the number of parts in the fixture to decrease the total number of program starts and stops. Have considered not sending the tool to the home position between cycles. I have set up parts so that operator was actuallly loading while machine was in cycle. Not the safest routine and OSHA would slap you silly but it works. More info will help. I like these problems.

[ctate2000]

The maximum tap speed is the one that will give you the results you want. If your machine is capable of tapping at very high RPM like some of the Brothers use it. 5mm tap in aluminum should be ok at 6000 RPM or so. Coolant flow and mix is very critical at those speeds.

[jderou]

6 5mm and 2 8mm holes. over a circle about 10" diameter. Right now its about a 45 second cycle time. It is on a pallet changer so they are loading while it cycles. 45 seconds is the time from pallet change to pallet change. Coolant flow looks like a waterfall. It may be possible to change the home position, will look into it. If you think its ok to 6000 rpm I may try 4000 and see what happens. this is cast aluminum BTW.
Thanks

[Geof]

6 5mm and 2 8mm holes. over a circle about 10" diameter...

Is it a true circle? Are you using a bolt circle canned cycle or are the hole locations directly programmed. Canned cycles are sometimes slow because you have to move to center, do the circle then return to center; if you are going direct hole to hole it can be quicker. Also depending on the way your machine rapids you may be able to shave off a bit. Most times the rapid goes full speed on both axes until one hits position then just moves on the remaining axes until both are correct; the travel is a dog leg. Some machines allow you to changing a setting or parameter to 'interpolate in rapid' then it runs both axes at a rate to make a straight path between holes and it can take a very small amount less time.

[jderou]

Sorry, its not a bolt circle, I just meant the holes are spread out within the circle, hard to explain. They arent at the same height either.