Holding a tenth all day on a high speed mill!

[vinny]

First of all, if you have no laser for tool pickup...move on. Read about the
arab crap instead.

Setup...2 fanuc makinos, 10 yrs old. Both have new spindles, and one has new
leadscrews.
machines run 24/7. Even holidays.
You will have to adapt this stuff to your setup obviously, but its universal
if you figure out how to do it on each brand.

This is a thread to throw some tips out there, if you disagree tell us why,
if you cant...again...go read arab posts.


First 4 tips! I have a bunch of em!

#1) First...add an orientation code to the tool change macro.
What this does is assure that every tool is picked up the same by the
spindle, helping repeatabilit.
Make sure and orientate when getting a tool and when putting it back.
You want the same conditions every time.


#2) Add a 30 second dwell to every finish tool to stabalize the spindle!..

#3) Try to group tools by rpm. Try to not have a big spead in rpm from one
tool to the other.

#4) Clean the spindle every setup.Clean every toolholder with a ruby stone,
keep the tools as short as possible.
And make sure everything is balanced, be anal about it. If you cut off a
cutter with a cutoff wheel, grind the end, it makes that'
much of a difference.

#5) Use the laser inteligently.
Do not do it manually one at a time.
Make a program, set eah cutter to laser at the rpm its programmed at.
Add a 120 second dwell to first tool, and a 60 second dwell to all others.
If you have to laser a single tool, make sure you laser them ALL again. It
must be done all together to get a perfect spread.
Keep people away from the machine when it's lasering.

6.)on a comparitor, map out bull cutter readii, measure the diameters,
etc...its called mapping out the cutters. Input this into your cad proggy.

7.) be sure your spindle oil is full if it cools the spindle. The more there
is the better the core temp will hold.
(hint...fanucs for the most part run the chiller when the spindle is turned,
even if just bumped by hand. So turn the spindle by hand it chill.)

8.) feedrates! Do a cut, watch the feed, if its slowing down in corners its
feeding too fast. What you want is a steady feed.
Corner control is great, variable feedrates SUCK. Learn how it can take a
corner,, and program feedrates as needed.
Remember, the rpm is not sycronised with the feed, So if ts slowing down in
corners, its not adjusting rpm...this just eats cutters like nothing else.

9) Holders. .0002 runout is the max. The coating is only a tenth deep, so
if you run out 3 tenths, it strips that flute of its coating, then wears
like crazy. if your using collets and think they are good enough...exit out
of your newsreader.

10) timing is everything.
You cant run non stop....go to lunch, and think it will be the same. It
wont.
try to pace yourself, same time between loads etc...

11) I got a bunch more...stay tuned for part 2.

[Alphonso]

Post by vinny
8.) feedrates! Do a cut, watch the feed, if its slowing down in corners
its feeding too fast. What you want is a steady feed.
Corner control is great, variable feedrates SUCK. Learn how it can take
a corner,, and program feedrates as needed.
Remember, the rpm is not sycronised with the feed, So if ts slowing down
in corners, its not adjusting rpm...this just eats cutters like nothing
else.

If you program IPR instead of IPM the feed and rpm are synchronised.

[vinny]

Post by Alphonso

Post by vinny
8.) feedrates! Do a cut, watch the feed, if its slowing down in corners
its feeding too fast. What you want is a steady feed.
Corner control is great, variable feedrates SUCK. Learn how it can take
a corner,, and program feedrates as needed.
Remember, the rpm is not sycronised with the feed, So if ts slowing down
in corners, its not adjusting rpm...this just eats cutters like nothing
else.

If you program IPR instead of IPM the feed and rpm are synchronised.

on a mill?

And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds and
feeds with corner control. Wow that would be awesome.

[Alphonso]

Post by vinny
on a mill?
And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds
and feeds with corner control. Wow that would be awesome.

Yes,on a mill. With IPR the FPT is synched to the spindle. I don't see why
you couldn't change the feed on corners or arcs and then go back to original
feed on straights.

I have a Reed Prentis WWII vintage mill that has the feeds in IPR. The first
time I ran a CNC mill I couldn't figure out why my feeds were all so slow
until I realized that the mill was in IPM.

[vinny]

Post by Alphonso

Post by vinny
on a mill?
And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds
and feeds with corner control. Wow that would be awesome.

Yes,on a mill. With IPR the FPT is synched to the spindle. I don't see why
you couldn't change the feed on corners or arcs and then go back to original
feed on straights.
I have a Reed Prentis WWII vintage mill that has the feeds in IPR. The first
time I ran a CNC mill I couldn't figure out why my feeds were all so slow
until I realized that the mill was in IPM.

Iv'e tried this on a haas, and the spindle couldnt change fast enough. The
machine jerked out from it.
Maybe on a higher end machine it could work ok?

[Gunner Asch]

Post by vinny

Post by Alphonso

Post by vinny
on a mill?
And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds
and feeds with corner control. Wow that would be awesome.

Yes,on a mill. With IPR the FPT is synched to the spindle. I don't see why
you couldn't change the feed on corners or arcs and then go back to original
feed on straights.
I have a Reed Prentis WWII vintage mill that has the feeds in IPR. The first
time I ran a CNC mill I couldn't figure out why my feeds were all so slow
until I realized that the mill was in IPM.

Iv'e tried this on a haas, and the spindle couldnt change fast enough. The
machine jerked out from it.
Maybe on a higher end machine it could work ok?

Just add some dwell after each spindle change, before the tool move


"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

[DanP]

Post by Gunner Asch
Just add some dwell after each spindle change, before the tool move

And get some dwell marks on profiles. If is a tough material you get work hardening too.

We get parts rejected if we have work hardening.


DanP

[DanP]

Post by vinny

Post by Alphonso
If you program IPR instead of IPM the feed and rpm are synchronised.

In IPR mode, does the control take into account the rad of the tool? I use IPR for 5 axis machining, never seen how it works on profiling.

Post by vinny
And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds and
feeds with corner control. Wow that would be awesome.

I do not see any need to change spindle speed, cutting speed must be kept constant. Load per tooth must be kept constant too, and feedrates must change for internal and external rads, but it depends on the rad of the tool.

I don't think the usual Fanuc controls can do it, and even if some do I would not use it, move the job to dumb one and the problem comes back. And one day an operator will forget to input the tool diameter into the control so I prefer the feedrates changed by CAM software.

Esprit gives you variable feedrates for corners, is one of the good points of this POS, together with cutting speed and load per tooth.


DanP

[vinny]

Post by vinny

Post by Alphonso
If you program IPR instead of IPM the feed and rpm are synchronised.

In IPR mode, does the control take into account the rad of the tool? I use
IPR for 5 axis machining, never seen how it works on profiling.

Post by vinny
And if yes, can the spindle changes keep up with the feed changes?
Because this is the dream of all high speed millers, syncronised speeds and
feeds with corner control. Wow that would be awesome.

I do not see any need to change spindle speed, cutting speed must be kept
constant. Load per tooth must be kept constant too, and feedrates must
change for internal and external rads, but it depends on the rad of the
tool.

I don't think the usual Fanuc controls can do it, and even if some do I
would not use it, move the job to dumb one and the problem comes back. And
one day an operator will forget to input the tool diameter into the control
so I prefer the feedrates changed by CAM software.

Esprit gives you variable feedrates for corners, is one of the good points
of this POS, together with cutting speed and load per tooth.


DanP

**************
Mastercam 9 came with a chook proggy that was just what your talking about.
You could tell the software to slow down on corners with a certain angle or
a certain gforce.
It worked way better than fanuc corner control because you could tweak it
over time for a particular machine.
However, you still couldnt control the rpm, and not that it mattered, the
machine could not speed up or especially slow down
fast enough to matter.

The option now is at the machine, turn down the feed/rpm until corner
control is bearly changing the feedrates.