What's new
What's new

M560V max tap speed

Captdave

Titanium
Joined
Sep 24, 2006
Location
Atlanta, GA
We have an ongoing job and tap 1,000,s of 3/8-16 through holes in 6016 a week. We have been tapping at 1,000 RPM and and would like to increase rpm for increased productivity.

Just curious if anyone has found a max RPM on these machines?

BTW it's a P300 control.
 
I think that you can tap at up to 4K RPM on the 560 but the biggest thing that seems to affect cycle time is wether or not you have the spindle commanded to orient before tapping (like if you are peck tapping) or not.
 
hy Captain :)

- combined tool : drill + tap
- "self feed holders" or even better : "tapmatic holders"
- increase bore before tapping, even a bit more than allowed :) thus raise a bit the maximum allowable tolerance
- tappers :
...... without straight helix
...... tappers with longer conicity in front, for smooth entrance
...... tappers short as possible, but not exagerated, since length changes of 0.5D won't counts as much as 2.5D
...... try different ones and keep those with better edge finish :) thus keep an eye on load monitor and how many parts / tap

- your cutting specs are yours to play with :)
 
I am sure you have a scrap piece of stock . . . try a few holes at 2k and check the threads. You may find acceleration / decel are taking more time than you spend at 2k rpm, but with that quantity of holes you are the best experimenter out there! Let us know!
 
I think that you can tap at up to 4K RPM on the 560 but the biggest thing that seems to affect cycle time is wether or not you have the spindle commanded to orient before tapping (like if you are peck tapping) or not.

Hi Micky,
Wasn't aware there was a code for that, we have just been using G84 cycle.

N1317 (3/8-16 TAP .375 SPRIAL FLUTE)
N1318 G116 TOOL=6
N1319 T43
N1320 G15 H1
N1321 G0 X0. Y-2.2874 M03 S1000
N1322 G00 G56 Z0.5 H6 M08
N1323 G00 X0. Y-2.2874 Z0.5
N1324 G84 Z-0.75 R0.3 F62.5
N1325 X-1.754 Y1.4682
N1326 X1.754
N1327 G0
N1328 G00 Z0.5
N1329 G00 X7.5 Y-2.2874 Z0.5
N1330 G84 Z-0.75 R0.3 F62.5
N1331 X5.746 Y1.4682
N1332 X9.254
N1333 G0
N1334 G00 Z0.5
N1335 G00 X15. Y-2.2874 Z0.5
N1336 G84 Z-0.75 R0.3 F62.5
N1337 X13.246 Y1.4682
N1338 X16.754
N1339 G0
N1340 G00 Z0.5
N1341 G00 X22.5 Y-2.2874 Z0.5
N1342 G84 Z-0.75 R0.3 F62.5
N1343 X20.746 Y1.4682
N1344 X24.254
N1345 G0
N1346 G00 Z0.5
N1347 G00 X30. Y-2.2874 Z0.5
N1348 G84 Z-0.75 R0.3 F62.5
N1349 X28.246 Y1.4682
N1350 X31.754
N1351 G0
N1352 G00 Z0.5
N1353 M5
N1354 G30 P1
N1355 M01(****************************)
 
why did u post that code ? :) please, review all this, so to optimize it :

... why 2nd line after each G84 moves X with 1.754 more ?
... why G0 repeats 3 times in a row ? ( N1333 > N13335 )
... why redundant Z0.5 ? ( N1328 N1329 )
... why R0.3 and clearance at Z0.5 ? why so big Z_start ? how much air do you cut ?
... modin / modout ? soubroutines ? " position + cut + loop "
... increased "in position window" for rapids, so to execute faster ?
... M08 before S, so to allow building coolant pressure ( even if in this case rapid is long enough )

you may gain some 10ths of a second / cycle :)

Wasn't aware there was a code for that ...

i don't know if there is a code for it, but you may check this by using an excentric knife / thread mill with 1 tooth / T mill inside a hole or outside a cilinder; cut a spiral only 0.1 .. 0.2 depth

dwell for a period which is not a multiple of "duration required to cut a pitch"

repeat cutting the spiral

if ok, than increase Z start with pitch/2 : see what happens :)

if still ok, change rpm, so to check syncro at different spindle speeds :)

if nothing but pecking is required, use holders with "hard start" ; kindly !
 
We tested 2,000 RPM and couldn't tell and difference with a thread gauge :D There are 5 parts with 3 tapped holes each and knocked off 20 seconds per cycle. One of the things that I noticed when the machine was new and still does it is that there is a 1-2 sec pause and an audible click before and after each tap cycle, maybe the orient signal?

A quick look at M codes didn't show anything, may have to dig deeper later.
 
Just the way the CAM post it, I think it has 1,000 block look ahead so doubt there is and appreciable delay with processing the code but thank for pointing it out.
 
Tapping head! It is much easier and faster to reverse 8 oz instead of 200 lbs.

A Tapmatic will pay for itself in short order given the quantity and aluminum. combine this with roll taps amd your productivity is going to quadruple easily.
 
There is a code to orient the spindle before tapping a hole, but I don't remember what it is offhand. If you use it the machine will start tapping each hole at the same spindle orientation so you can retap a hole or peck tap. It does slow down the tapping cycle like previously mentioned.
 
Captdave;2900574 said:
... and couldn't tell and difference with a thread gauge

hello Captain :) thread calibers say only "yes / no"; they can not "speak" about what happens when cutting specs change

other cutting specs generally changes dimensions a bit, but this 'bit' can not be inspected this way

Captdave;2900574 said:
I think it has 1,000 block look ahead so doubt there is an appreciable delay with processing the cod

"read ahead buffer" and "program execution" are a bit diffierent :) well, you know that :)

also, they both rely on each other, but not the way that results from that (your) statement

... (my) suggestions on code will spare 10th of a second ( even on a lower size read ahead buffer )
... (my) suggestions on tools will spare seconds
... your cutting specs will spare even more :)

if is possible, give it a try to self reverse holders; Tapmatic is not the only player on the market :)

if soft material, and fixtures permits, think of combined tool : drill + tapp

There is a code to orient the spindle before tapping a hole, but I don't remember ...

hy Edseter :) please, let us know if you discover something :)

It does slow down the tapping cycle like previously mentioned

if tapping starts each time at same Z, than it may be a chance to avoid time loss, if "absolute Z" and " rpm " are synced > involves knowing how the machine syncs :)

please check a suggestion for testing sync from few posts ago :) kindly !
 
I've tapped at 4000 rpm with 10-32 form taps in aluminum in my M560. Works fine. 1.5 deep is like a second a hole.
 
The audible clicks are air solenoids I think, I've been behind my 560 while it was tapping and the noises are solenoids of some type above the spindle oil reservoir. My best guess is it something to do with the spindle lube system?

I know exactly what you're talking about usually 2 or 3 clicks before the first tapped hole in a series. I think it is a spindle orient thing, but given that you don't typically turn the spindle after a tool change prior to arriving at the retract height...it seems kinda redundant. On my machine it only has that hesitation on the very first hole in the canned cycle.
 
Hi Micky,
Wasn't aware there was a code for that, we have just been using G84 cycle.

N1317 (3/8-16 TAP .375 SPRIAL FLUTE)
N1318 G116 TOOL=6
N1319 T43
N1320 G15 H1
N1321 G0 X0. Y-2.2874 M03 S1000
N1322 G00 G56 Z0.5 H6 M08
N1323 G00 X0. Y-2.2874 Z0.5
N1324 G84 Z-0.75 R0.3 F62.5
N1325 X-1.754 Y1.4682
N1326 X1.754
N1327 G0
N1328 G00 Z0.5
N1329 G00 X7.5 Y-2.2874 Z0.5
N1330 G84 Z-0.75 R0.3 F62.5
N1331 X5.746 Y1.4682
N1332 X9.254
N1333 G0
N1334 G00 Z0.5
N1335 G00 X15. Y-2.2874 Z0.5
N1336 G84 Z-0.75 R0.3 F62.5
N1337 X13.246 Y1.4682
N1338 X16.754
N1339 G0
N1340 G00 Z0.5
N1341 G00 X22.5 Y-2.2874 Z0.5
N1342 G84 Z-0.75 R0.3 F62.5
N1343 X20.746 Y1.4682
N1344 X24.254
N1345 G0
N1346 G00 Z0.5
N1347 G00 X30. Y-2.2874 Z0.5
N1348 G84 Z-0.75 R0.3 F62.5
N1349 X28.246 Y1.4682
N1350 X31.754
N1351 G0
N1352 G00 Z0.5
N1353 M5
N1354 G30 P1
N1355 M01(****************************)

Why so many duplicate tapping operations? I'd bet you cut out a bunch of time just compressing them all into one canned cycle since they are all the same otherwise.
 
Other then I'm lazy and just let CAM do it in a repeat at X intervals. If I drew the 5 parts and picked each hole then it would be all in one G84 cycle.
 
Why so many duplicate tapping operations? I'd bet you cut out a bunch of time just compressing them all into one canned cycle since they are all the same otherwise.

not everybody goes improving code, especially when it is CAM generated, and this because most time gain does not come from CAM, but from tools, fixtures, control, etc ...

is good to know and understand programs, but is not always worthy to improve them

also, another reason is that nobody checks a programmer work, but the part delivered from the cnc; most guys are comfortable with the fact that it works, and don't go improving because :
... there is no time
... there is no money
... improving with available resources will take too much to implement, and time gain will be little

improving a program is related to other things :) even if you can improve something, is not always required to do so :)
 
Scoured through the manuals today and didn't see anything remotely addressing cancelling spindle orientation. I could be wrong but didn't find anything.
 
not everybody goes improving code, especially when it is CAM generated, and this because most time gain does not come from CAM, but from tools, fixtures, control, etc ...

is good to know and understand programs, but is not always worthy to improve them

also, another reason is that nobody checks a programmer work, but the part delivered from the cnc; most guys are comfortable with the fact that it works, and don't go improving because :
... there is no time
... there is no money
... improving with available resources will take too much to implement, and time gain will be little

improving a program is related to other things :) even if you can improve something, is not always required to do so :)

I was asking Captdave in this specific instance. And he answered. Thanks.

Here's a comic for you:

is_it_worth_the_time.png
 








 
Back
Top