Printable View
hi all,
im turning a large, 6 start, internal acme thread in a V60R vertical lathe and an osp200L control. ive got my depth of cut set at only .005" and the spindle keeps momentarily "stalling" and trashing my tool.
i have the infeed angle set at 31° so that i am cutting with the tool tip only on infeed. i feel like this should be childs play but the spindle just doesnt seem to want to cooperate. any ideas?
Greetings,
Acme threads are 29 degrees, included angle.
Would not a 14 - 14 1/2 degree angular infeed be correct?
Also, a six start thread will need more flank clearance, if not already compensated for.
Cheers,
Dave
Hi Dave, thanks for the reply. im aware that an acme thread is 29° and i set the infeed angle at 31° as a way to ensure the tool is only contacting at the tool point, or, root of the thread (i am just roughing the thread at this time)
The reason i chose 31° is the description of infeed angle in my programming manual:
B: infeed angle (0° ? B <180°; 0 if no designation. normally it is equal to the cutter tip point angle.)
i have a custom tool that i am using with ample clearance on the "bottom" flank, i dont believe this is my issue.
first of all, I didn't got what kind of chuck ( spindle ? ) "stall" should happen there. In the any threading operation the Z is synchronized with spindle rotation and the tool tip should follow the thread path anyway even if spindle speed is varying.
What I would do - I would simulate the threading with safe X offset "in the air" in the one-step mode if necessary.
I would say some settings of the threading cycle are wrong: approach point X / retraction point X, tool tip offset or combination of these.
Does this lathe have multiple spindle gear ranges? Perhaps your RPM is too low for the gear range you are in and the spindle motor doesn't have enough torque at slow speed. I am only familiar with older stuff but I would look at M41/M42.
Dave in Ohio
Good morning Al, Dave.
this lathe has one gear only, this was my first thought as well.
Al, here are some pictures of the damaged part. the threading cycle is fine. it has been animated, and dry run without issue. in the pictures can see where the chuck stalls and the z axis continues to feed. this has happened twice, in two diferent locations (as shown). Also, here is a sample of the code. maybe you see something that i dont.
G00 X50.0 Z50.0
T070707
G50 S500
G97 S80 M3
G95
G00 X4.950
G00 Z0.5
G71 X6.040 Z-3.7 B31.0 D0.005 U0.005 H1.04 F6.0 Q6 M34 M74
G00 Z50.0
G00 X50.0
hy jay :) at 1st glance, pitch/spiral angle is way to aggresive, operation is more like a grooving/splining/or however you call it in english , and i would recomand c axis fur such
also, it may require a custom toolholder
your setup & code is ok for general threading, while in this part you don't even get a full revolution; it may not seem important to get a full revolution, because even when cutting oiling grooves a full revolution is more than enough, but in your case, the section is big, and even if you try to trick it with custom infeeds, it may not work, because a general threading insert is somehow perpendicular in the cross section, and this only applies for normal threading operations ( when pitch/spiral angle is normal ); when pitch/spiral angle is high, some other forces appear, that can be handled by a custom toolholder that keeps insert section perpendicular on pitch/spiral direction (+ custom cooling pipes), and also a code that uses G01 C Z instead of G71
all these is just a wild guess :)
for a more relevant idea, i need to see how&when the machine stalls on this code and tooling
for specific code, i need drawing and insert dimensions / kindly :)
ps1 : a quick fix should be a higher rpm and a lower doc, but this may break your insert
ps2 : D0.005 U0.005 H1.04 : 200+ passes, that's definetly not 'common' threading
I'm kind of at a loss.
I don't think it helps with the spindle stalling but with the M34 I think you are cutting with the back side of the tool. Another idea change M74 to M75. It will make a lot more passes but the amount per pass will be less, It will start with your 0.005 then be less each time after. It still probably won't help, but its worth a try.
Dave in Ohio
Sure, illustrations help very much to understand the situation. I would check the chucking first. Just simple mark with a sharp edge to see if workpiece is not moving in the jaws.
not really sure what to say guys. i appreciate all your replies. i think the error is coming from the drive belts between the motor and the chuck. it ran really well all morning and then all of the sudden this afternoon it messed up again. this time i saw the chuck physically slow down followed by the crunch of another custom tool....... is there a way to cut an acme thread in these machines WITHOUT using a form tool? could a program be written to slowly generate the thread form using a smaller tool to decrease the chances of this error happening?
sure it depends on depth of cut. It is really small in your case. Check other relevant points:
- if the cutting edge is sharp.
- if the cutting point is cooled well
- check with micrometer if the attack angle is not lifted.
Attack angle can be the issue, I think. The cut doesn't looks clean at your pictures, so this could be the case.
Static measurement can show very accurate setting. Then check measuring the cut - maybe there is significant decline when load on the tip increase.
on the other hand - check the tension of the belt.
The belt tension is always tricky, because the tensiometer is good for a new belt. Overtensed belt will loose very quick because of heat. Loosen belt is loose at the very beginning ...
I do the following. Make a small test program to increase the spindle rpm step by step. Use, let's say 20 steps to reach maximum rpm ( 8000 for instance ).
Launch the program and observe the belts. Belt should not play up-down ar travel to sides. On the steps increasing belt load, the belt twists a little. With stabile rpm the twist dissapears. Next rpm step - twist again. Twist should take place the same direction always. It is ideal ( Okuma case ) when double belt installation belts twist symetricaly - opposite directions each.
With maximum rpm the easy twist could be observed even when rpm is stable.
That's the best practical method to make good tension for used belts I know.
Hey Kitty,Quote:
Originally Posted by deadlykitten
Firstly, your point about the pitch/spiral angle is odd... the "Thread" has a 6 inch lead... did you note that the program is in imperial?
so a 6" lead is going to be "quite aggressive" anyway.
The desire to have a full revolution is from where? The part would have to be 6inches thick to get a full turn and maybe his part is not that thick?
The DOC is 0.005" (0.127mm) so quite reasonable, otherwise he will be there all day.
Definitely need to be looking at belt slippage as a possible problem area.
On the point of other methods, I have used a programming method that was "VERY" long handed way of doing things a very long time ago...
I programmed a series of points and used a G33 sub routine that cut the thread pass after moving to the next point on X and Z
i.e. used MODIN/MODOUT.
This did work, but the job took a long time to produce. Mind you, it was a big profile that used an involute profile on the sides of the "thread"... weird bugger for sure.
Don't have access to the work network at the moment to find that old program, at will not be back until Friday (4 days away).
You would need to make sure your tool point is set over at the correct helix angle to reduce the amount of "clearance" on the front edge for sure.
Will see if the memory works and I remember to look at work for the program on Friday.
Cheers
Brian.
I think it's either part slippage in the chuck or belt slippage.
What is PSI of chuck?
How much deflection can you induce when pushing on the belts? Are they multi-v or just v belts? PIC maybe showing deflection? I think this is the most likely cause.
hy broby, hy guys :)
jay dizzle's program is splinning at 12000mm/min, z travel 100, 200+passes, belts
i had been splinning at 21500mm/min, z travel 320, 150+passes, prex, for a few months, while i have encountered a few things, and i'll go over them as short as possible
*both setups are about intensive splining for long parts
Quote:
your point about the pitch/spiral angle is odd
i was trying to say that, when the angle is high, then the process is no longer a classical threading, but splining, and, just like you and others said, it requires the tool to be aligned with the helix ( insert midplane tangent to helix + y alignment ), and very good cooling ( like using at least 2 lolipop nozzles )
high helix angle = slow rpm = less spindle torque; i was refering to more spindle phase within same z travelQuote:
The desire to have a full revolution is from where?
most parts are short, while this one requires a longer z travel
feed > 50%rapid is common for such operations, and this requires signifiant more z travel for the axis to reach speed
as z travel increases, there are more chances for z axis to reach programmed feed, and, at this level, there is no more torque; in other words, when splining common short parts, machine won't reach programed feed, thus it will succumb ( longer cycle time, but more torque available), but it works, so everyone is happy
available torque will say how much stable is the machine for that splining process; longer axis acceleration requires torque for more time, leading to less resources available for cutting, and splining cutting diagram has high peeks, like no other operation
most parts are short, with normal grooves = normal tool, thus the machine should cut it
this part is long, with a big groove, thus the machine will try to reach and keep it's speed at a level where is less torque available to beat the cutting forces, and this means that the process is in a zone that is close to sudden failure ( like 99% it will work, while a small tool wear, or an endangled chip, or a colant nozzle moving, or something related to the machine will stop it; for example, after intensive splinning, the spindle will require more force to be turned; this may not damage the machine, only spindle resistance will increase, but it will require more force in order to sustain the same rpm, and how a belt mechanism has lower randament than a prex, it means that a belt will be subject to more stress )
if an insert breaks, or gets some wear, during :
... normal threading, the machine will finish the operation
... splining with high feed, machine could stop
is possible that jay dizzle's belts where ok until this setup, and they got messed up by this process, because of keeping the machine too long in this gray area, right under a failure threashold
please consider this comparisons :
... normal turning versus m63modal with low clearance : spindle needs a few tens of a second to ramp up using 160-180%, and in that time you may allready start cutting; if you are cutting a small diameter with low doc and with long z approach you will have more torque available, but, if you are cutting a big diameter with big doc and small z approach, you may block the machine
... start moving in a car that is not in a low gear
how to control the gray area ? load comparison between cutting air and real cuting, z & s variations as z travel increases ( to see how chip evacuation works ), and monitoring variations among entire process length, so to identify small load variations before they become big load variations; this approach works, or at least helps, but is not common, because most machining operations do not need such a level of control
aparently is ok, but for biger threads, what can really make a difference for insert lifespam is achieving constant load / each passQuote:
doc is 0.127mm, so quite reasonable
one way to do this is to use identical area engagement, thus target same chip section between passes, and use load monitor to fine tune-it
still there may be sudden insert failures, but, overall, there should be less such failures
if failure amount still seems high, simply add a few more passes ( sometime such variations are caused by low quality inserts )
everyone wants fast and yesterday :)Quote:
otherwise he will be there all day
another thing may appear : g71/g33 with high z feed rates may produce vanished threads ( 10 to 50 mm maybe; depends on machine cinematic ), thus x axis may move while z axis is cutting, and this can be fixed with g34 or m110 cz; off course, vanished threads may be tolerated, or won't appear if clearances are long enough, but otherwise, and especially when required z travel is almost equal to machine available z travel, then is a kind of another situation
also, using m110 cz, is possible to :
... create a low feed program, controled from potentiometer, used to check the part with a dial, before opening the chuck ( like to check vanish at both ends )
... create a program that will recut a re-clamped part
vanished threads are not equal at both ends, since x axis is in-position before z travel begins, while, near the end, x axis raises before z axis reaches in-position, and, for this reason, i recomand checking this before opening the chuck; again, this does not matter for most operations, but for z feeds > 10000 mm/min, may be a thing :)
programing should be cake, at least for someone like you :) i have coded similar parts using m110, because g33 will lose time, right before the cut, when x axis moves and waits to get in sync with spindle phase; when there are hundreds of passes, hundreds of parts, eliminating this delay required for syncing is worthy, but you can not think of this untill you fix the stallingQuote:
I have used a programming method that was "VERY" long handed
real deal is to locate the cause of failures, and, so far, is not known, maybe best guess is belt slipping, maybe belts are okey yet there is no torque ( thus belts are slipping not because they are loose, but because the machine is pushed - use a camera to record belt transmision ), maybe chips are skuished between tool and jaws near end z leading to premature tool wear
i can compute custom infeeds, gather monitor data, and still, sometimes i hit into materials and inserts quality variations, etc
a few days ago, we had to quote a relatively simple part, with a big thread : if it works, would be <1 hour, otherwise, place your bet ?! some rollers for the threading rolling machine took way longer than expected, and all these are much simpler than parts like jay_dizzle's
there is one more thing : for common stuff, rpm = [M/min] * 320 / dia, but for such parts the formula do no longer apply, since the helix has such a high angle, thus movement is much more linear than common threading; if you compute feed corectly, and/or if your z axis feed is maxxed and insert lifespam is okey, then it means that the insert can operate at a much greater feed than what the z axis is capable to output, thus the machine wasn't build for such operations : this is why live broaching toolholders exist ( their travel is too short for jay dizzle's part ), or you could design a x axis reversed milling head, to operate, for example, with an end-mill o8
of course : you could use some cheap stuff from your local market to rough your groove, then use a hss in-house insert to finish itQuote:
could a program be written to slowly generate the thread form using a smaller tool to decrease the chances of this error happening?
i am not sure if insert shape is the main cause for those failures, but it is worthy to rough with a cheaper&smaller insert
maybe is a good idea to spline that part like half-half, or 1/3 1/3 1/3, thus avoiding entire z travel in order to help with chip evacuation, and use a program with safe-position retreat on demand ( "/" ), like when hobbing
if you wish, i'll give you code / kindly :)
ps : use a camera to record belt transmision, and a marker to drag a continuous line on part and chuck, so to check if your part is rotating
Thanks for helping solve this task.
I also have the same problems. Thanks for solving and tips.