What's new
What's new

24,000 6-32 holes to make, how fast can I go?

Volitan

Hot Rolled
Joined
Sep 16, 2006
Location
Long Island, New York
The material is 1/8" thick cold rolled. It came on a coil before it was stamped, it's pretty soft.
I have OSG Hypro cut taps. Last time I ran them at 2560 RPM, I think the Brother TC-31A machine is capable of tapping at up to 8000 rpm.

How fast can you push a 6-32 cut tap (drilling .110 dia.)?
 
I would wonder how fast the machine would actually accelerate and reverse in that short distance. Pretty sure there is a point where increasing the programmed RPM does nothing to decrease the cycle time. i would just call the machine builder and ask them.
 
I would wonder how fast the machine would actually accelerate and reverse in that short distance. Pretty sure there is a point where increasing the programmed RPM does nothing to decrease the cycle time. i would just call the machine builder and ask them.

I've noticed that with our older Haas's but the Brother gets up to speed in no time flat.
 
Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.

Cycle time will be way faster tapping. My S700 gets up to 6k-8k RPM in a fraction of a second, like literally a blink of an eye. I would estimate actual in-the-machine cycle time per tapped hole would be ~1 second.

Drilling accurately might be more challenging with tap vs. threadmill, but with 24K holes to do, I would be spending some time to dial in the hole size, then get on with it and tap.

Heck, I could add a tool break check, and still be faster tapping than threadmilling.

Regards.

Mike
 
I guess it depends on whether it's 24000 pcs with 1 tapped hole or 1 pc with 24000 tapped holes.
Or somewhere in between.
 
Do you need to drill and tap? Through hole right? The Brother has a drill/tap cycle G177 for DRAPs. A tap with a drill tip. I've used them on several occasions and this could be one of those 'right' applications. Cycle time with one of those around the 2 second range for drilling and tapping.
 
It's 6,000 pcs with 4 tapped holes in each.

The DRAP sounds interesting too. Yes it's a thru hole in a 1/8" part. I've seen those things before but the ones I saw were shit quality so I forgot about them. Maybe I'll look into a good brand after I get this thing running.

I like Larry Dickmans idea of using the max as a starting point :)
 
Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.

Great idea. And 6-32 could be cut in one pass. It would partially depend on the tightness and screw comp settings of your machine as to how fast you can run it and still maintain an acceptable amount of circularity. I mean small thread mills in small holes make for very small circular tool paths. Some machines are better at this then others.

If the holes are fairly close to to each other I suggest trying all your rapid moves, even in and out of the hole, in a high feed G1 instead. I do this when creating HSM tool paths. Keeping the return to start point, which at times can be very close, at a high feed rate in lieu of rapid.. (250-500ipm) My Fanuc driven Mori machine moves quicker like this and the motors seem to like it a lot better. It's actually how I discovered the concept. I was getting an overheat or overload error on the servos during an HSM path. I guess dumping all the power it had into trying to get up to full rapid in a quarter or half inch was too much to ask. The only thing I did to get rid of the alarming was switch all my G0s to high feed G1s and no more problems. It also seemed to run faster and smoother.

Ha... imagine producing a job with 24,000 tapped holes and never reversing the spindle. Sounds crazy but who knows? May be that the machine and overall program time would also like the idea.

I see this no reverse tapping story told to the right crowd at the right time will likely get you a free beer to boot. :-)

Dave
 
Never used a Brother. It would be interesting to see what the average rpm is while tapping

They are pretty insane when tapping. I'd be surprised if the average rpm isn't the programmed rpm or damn close to it.
I tap 8k holes every 2 months or so in 6061, #4-40 threads. And it doesn't mess around. There isn't a machine that compares to a Brother when tapping even our brand new Okuma mills don't even come close to the tapping efficiency.
 
Great idea. And 6-32 could be cut in one pass.

In cold-rolled steel? (I'm assuming that's what the OP meant when he said "It came on a coil".) 6-32 threadmill has a tensy tiny minor diameter, like .065". Not saying it can't be done single-pass, but I would predict that thread size consistency would be a challenge.

Regards.

Mike
 
Never used a Brother. It would be interesting to see what the average rpm is while tapping

I've used those tapmatics in a mid-90's vintage Fadal and they are the bees knees.
This Brother was made for this though. Even though it's an older 1999 model they made the spindle super light weight so the accel/decel and reversing of the spindle is damn near instant. It's like it's either on or off.
 
In cold-rolled steel? (I'm assuming that's what the OP meant when he said "It came on a coil".) 6-32 threadmill has a tensy tiny minor diameter, like .065". Not saying it can't be done single-pass, but I would predict that thread size consistency would be a challenge.

Regards.

Mike

Yes CRS, I can't get a number but I'm told it's "about 1/4 hard." It's really soft stuff.
 








 
Back
Top