Drilling Problem? Haas VF-2 Problem?

[The R in SPR]

Hello all.
I read this newsgroup a few times a year and have posted once or twice.
I just started trying to use our new VF-2. (IMTS booth machine, 10K rpm)
I had a re-order job that I'd ran previously on our 2-year old VF-2 (Brand
new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making chips
and break my .070" drill.
Break a few more, (standard drills, spot drilled holes). I'm thinking bad
drills, find old drill (short drill, split point) break old drill. Find
another older drill, reduce feed rate and drill a few holes.
When I inspect holes, they are big towards the top. (.073 pin starts in
hole, .070 goes through).
Now I suspect something else.
I take spot drill/.070 drill in chuck from new machine to old machine, drill
with same tooling/drilling parameters etc. .070 pin is tight, .069 pin goes
like nice, like it has for thousands of times.
Haas service comes out, checks out new mill says everything is good
mechanically.
Now they request machine parameters to compare new vs old.
I've checked the obvious things I can think of.
Please help!

Thanks,
Scott

[Garlicdude]

Post by The R in SPR
Hello all.
I've checked the obvious things I can think of.
Please help!
Thanks,
Scott

Check for spindle runout by putting a .070 gage pin in the
same holder and collet and check both machines?

Best,
Steve

[The R in SPR]

The Haas tech did runout check on the 40 taper spindle with indicator.
He also had a 1 1/4 dia. or so ground bar with integral 40 taper (one
piece).
Both machine were .0002" tir at 6" gage length. (less closer to spindle)
I'm driving the drill with a Jacobs 0 drill chuck.

Post by The R in SPR
Hello all.
I've checked the obvious things I can think of.
Please help!
Thanks,
Scott

Check for spindle runout by putting a .070 gage pin in the same holder and
collet and check both machines?
Best,
Steve
--
Regards,
Steve Saling
aka The Garlic Dude ©
Gilroy, CA
The Garlic Capital of The World
http://www.pulsareng.com/

[PrecisionMachinisT]

Post by The R in SPR
The Haas tech did runout check on the 40 taper spindle with indicator.
He also had a 1 1/4 dia. or so ground bar with integral 40 taper (one
piece).
Both machine were .0002" tir at 6" gage length. (less closer to spindle)
I'm driving the drill with a Jacobs 0 drill chuck.

Okay, but Steve was telling YOU to check YOUR cutting tool / holder assembly
for possible runout....

BTW: After that, throw the Jacobs chuck into the trashcan.

--

SVL

[The R in SPR]

Same drill in same chuck in same cat 40 holder, different machine.How would
runout matter?
The jacobs chucks work sufficiently.

Scott

Post by PrecisionMachinisT

Post by The R in SPR
The Haas tech did runout check on the 40 taper spindle with indicator.
He also had a 1 1/4 dia. or so ground bar with integral 40 taper (one
piece).
Both machine were .0002" tir at 6" gage length. (less closer to spindle)
I'm driving the drill with a Jacobs 0 drill chuck.

Okay, but Steve was telling YOU to check YOUR cutting tool / holder assembly
for possible runout....
BTW: After that, throw the Jacobs chuck into the trashcan.
--
SVL

[PrecisionMachinisT]

Post by The R in SPR
Same drill in same chuck in same cat 40 holder, different machine.How would
runout matter?

Okay, I musta missed that part. ...

Post by The R in SPR
The jacobs chucks work sufficiently.

Personally, I would still toss the jabobs chuck into the dumpster, along
with both Hass machines....but that's just me...

==

Suggest should check out your machine alignment...z to c axis in
particular--sounds kinda like the spindle bearings may not be sufficiently
parallel to the slide.

Easy check is to indicate a hole xy location with your indicater hanging
from a long bar...then indicate it again using a short bar ( with the z
slide moved downward a bunch )--if all is well then you should pick it up at
the same xy reading...

If not, then you'll probably need to shim the cartridge underneath the
flange where it bolts onto the head...

--

SVL

[The R in SPR]

Amongst other checks tonight-oh its tomorrow- I swept a 6 or 7 inch radius
with an indicator clamped to toolholder and saw that thespindle is
perpendicular to the table within .001" TIR.
Yesterday the facory tech shimmed the cartridge you mention and claimed
.0004" TIR.
I'm wondering if it is something happening at speed as PV mentioned.

A lot of people bad mouth the Haas stuff. I've found that with sound
practices they perform well within the specs I'm required to work to.
Granted +-.005" milling aluminum and drilling/tapping is not the toughest
and most challenging work on man or machine. My first VF2 has brought good
return on investment.

I think I'm gonna put the new one to some pocketing when I get back here
later and see what that uncovers
Thanks all and good night,
Scott

Post by PrecisionMachinisT

Post by The R in SPR
Same drill in same chuck in same cat 40 holder, different machine.How

would

Post by The R in SPR
runout matter?

Okay, I musta missed that part. ...

Post by The R in SPR
The jacobs chucks work sufficiently.

Personally, I would still toss the jabobs chuck into the dumpster, along
with both Hass machines....but that's just me...
==
Suggest should check out your machine alignment...z to c axis in
particular--sounds kinda like the spindle bearings may not be sufficiently
parallel to the slide.
Easy check is to indicate a hole xy location with your indicater hanging
from a long bar...then indicate it again using a short bar ( with the z
slide moved downward a bunch )--if all is well then you should pick it up at
the same xy reading...
If not, then you'll probably need to shim the cartridge underneath the
flange where it bolts onto the head...
--
SVL

[Dave Lyon]

Post by The R in SPR
A lot of people bad mouth the Haas stuff. I've found that with sound
practices they perform well within the specs I'm required to work to.
Granted +-.005" milling aluminum and drilling/tapping is not the toughest
and most challenging work on man or machine. My first VF2 has brought good
return on investment.

I'm sorry, but that's much to sensible of an approach to actually work. All
tool shops should buy high speed machines capable of insane feed rates and
RPMs, even if they only use the machine a couple of times a year. :)

[r***@msn.com]

I'm intrested to see the outcome of this!!
I gots no real answer!

hhhmmmmm,,,
Coolant differences, older machine may be "richer" than new mix,
therefore having more lubricity?

Check concentration on refractometer

Maybe try applying same cutting fluid from older mill directly to tool?

fwiw I think an hss .070 drill would have enough flex to not break
with a few thou of angularity or mis-alignment, I've watched them "go
around corners" in my bridgeport days, (a really long time ago!!)

"D"

[The R in SPR]

EFFING COOLANT!
So I swap the coolant tanks and drill holes with old e206 coolant, viola,
good holes again.
Even with the old shitty jacobs chuck.
Well, I'm off to clean up and cover the table with vises again. Time will be
the ultimate test but I'm thinking this new 270 coolant that was recommended
to fix the foaming is the problem.
I've checked with refractometer and it's 8%, but maybe I'm still missing
something there. If not, I hope someone at the chemical place shits in their
pants today.
Thanks again all,
Scott

Post by r***@msn.com
I'm intrested to see the outcome of this!!
I gots no real answer!
hhhmmmmm,,,
Coolant differences, older machine may be "richer" than new mix,
therefore having more lubricity?
Check concentration on refractometer
Maybe try applying same cutting fluid from older mill directly to tool?
fwiw I think an hss .070 drill would have enough flex to not break
with a few thou of angularity or mis-alignment, I've watched them "go
around corners" in my bridgeport days, (a really long time ago!!)
"D"

[F. George McDuffee]

Thanks for "closing the loop" and letting the group know what you
found.



On Wed, 25 Oct 2006 11:59:36 -0400, "The R in SPR"

Post by The R in SPR
EFFING COOLANT!
So I swap the coolant tanks and drill holes with old e206 coolant, viola,
good holes again.
Even with the old shitty jacobs chuck.
Well, I'm off to clean up and cover the table with vises again. Time will be
the ultimate test but I'm thinking this new 270 coolant that was recommended
to fix the foaming is the problem.
I've checked with refractometer and it's 8%, but maybe I'm still missing
something there. If not, I hope someone at the chemical place shits in their
pants today.
Thanks again all,
Scott

Post by r***@msn.com
I'm intrested to see the outcome of this!!
I gots no real answer!
hhhmmmmm,,,
Coolant differences, older machine may be "richer" than new mix,
therefore having more lubricity?
Check concentration on refractometer
Maybe try applying same cutting fluid from older mill directly to tool?
fwiw I think an hss .070 drill would have enough flex to not break
with a few thou of angularity or mis-alignment, I've watched them "go
around corners" in my bridgeport days, (a really long time ago!!)
"D"

Unka' George (George McDuffee)
..............................
Only in Britain could it be thought
a defect to be "too clever by half."
The probability is that too many people
are too stupid by three-quarters.

John Major (b. 1943),
British Conservative politician, prime minister.
Quoted in: Observer (London, 7 July 1991).

[Dave Lyon]

Post by The R in SPR
EFFING COOLANT!
So I swap the coolant tanks and drill holes with old e206 coolant, viola,
good holes again.
Even with the old shitty jacobs chuck.
Well, I'm off to clean up and cover the table with vises again. Time will be
the ultimate test but I'm thinking this new 270 coolant that was recommended
to fix the foaming is the problem.
I've checked with refractometer and it's 8%, but maybe I'm still missing
something there. If not, I hope someone at the chemical place shits in their
pants today.
Thanks again all,
Scott

I'm sorry for all your trouble, but I'm grateful for the on topic posts and
giving me an education.
Thanks for letting us see all the steps it took to find the cure.

[c***@lycos.com]

Post by The R in SPR
EFFING COOLANT!
So I swap the coolant tanks and drill holes with old e206 coolant, viola,
good holes again.

Glad you found a solution and shared it with us. It was very
interesting to read the thought processes of those that came up with
ideas of what to check and why.

Wes S

[Cliff]

Post by c***@lycos.com

Post by The R in SPR
EFFING COOLANT!
So I swap the coolant tanks and drill holes with old e206 coolant, viola,
good holes again.

Glad you found a solution and shared it with us. It was very
interesting to read the thought processes of those that came up with
ideas of what to check and why.

Something else may have changed at the same time ...

[The R in SPR]

Okay SVL,

I indicate the shank of the drill in #0 jacobs chuck and see .002 TIR.
I install 0.140 gage pin in newer 180DA 9/64 dia collet and chuck and see
.0015 TIR
I install 1/8" shank solid carbide endmill in older 1/8" collet and see
.0015 TIR
I install same 1/8" shank endmill in set screw style endmill holder and see
.0001 TIR
I install 1/8" drill bit in same set screw style endmill holder and see
.0001 TIR at shank of drill.
I'm thinking pay dirt now, so I spot and drill a series of 28 holes with
drill in endmill holder. (1/2 x 3 1/2" 6061-T651)
g99g83z-0.56 r0.1 q0.05 f20.0 for the drill.
Upon inspection, 0.126 pin goes through, 0.129 pin goes in about 0.10".
While drilling, I observe the drill chattering as it rapids into the hole.
There is a polygonal chattery raised burr at the entry to each hole.

Post by PrecisionMachinisT

Post by The R in SPR
The Haas tech did runout check on the 40 taper spindle with indicator.
He also had a 1 1/4 dia. or so ground bar with integral 40 taper (one
piece).
Both machine were .0002" tir at 6" gage length. (less closer to spindle)
I'm driving the drill with a Jacobs 0 drill chuck.

Okay, but Steve was telling YOU to check YOUR cutting tool / holder assembly
for possible runout....
BTW: After that, throw the Jacobs chuck into the trashcan.
--
SVL

[Anthony]

Post by The R in SPR
Okay SVL,
I indicate the shank of the drill in #0 jacobs chuck and see .002 TIR.
I install 0.140 gage pin in newer 180DA 9/64 dia collet and chuck and
see .0015 TIR
I install 1/8" shank solid carbide endmill in older 1/8" collet and
see .0015 TIR
I install same 1/8" shank endmill in set screw style endmill holder
and see .0001 TIR
I install 1/8" drill bit in same set screw style endmill holder and
see .0001 TIR at shank of drill.
I'm thinking pay dirt now, so I spot and drill a series of 28 holes
with drill in endmill holder. (1/2 x 3 1/2" 6061-T651)
g99g83z-0.56 r0.1 q0.05 f20.0 for the drill.
Upon inspection, 0.126 pin goes through, 0.129 pin goes in about
0.10". While drilling, I observe the drill chattering as it rapids
into the hole. There is a polygonal chattery raised burr at the entry
to each hole.

*something* is loose, somewhere. It seems to appear when a load is first
put on the spindle, from your descriptions.
So, try this test:
Mount a large EM or pin (3/4" or so) in a holder and put it in the
spindle. Set up an indicator on the flange of the holder in the Z
direction. Place a second indicator on the front of the spindle (Y axis
direction) near the tool holder. Place a third on the spindle near the
tool holder in the X axis direction. Get a couple blocks of wood and a
short 2x4 to use as a catelever. Use the wood to press up on the end of
the EM/pin and see how much deflection you get on the indicators.
If there is deflection, then you have to narrow it down to the source
from there. There would be 3 main possible culprits, a) bearings/gibs of
the Z axis, b) spindle thrust bearings or preload and c) something in the
tool clamping or a taper mismatch issue.

[Proctologically Violated©®]

Sort of along the lines I was driving at.

Mebbe use one of them heavy plastic ballpein hammers w/ the screw off tips.
Proly would jar the indicators in any machine, but since he has two similar
Haas', mebbe he can do the same speriment on both, and watch for different
behaviors in the indicators.

Or, put some stops on the table, and *carefully*, in .001 jog, drive the
tool holder into the table, perhaps w/ an aluminum block as a buffer for
some shock.
Compare the indicator behavior on both Haas'.

I think the tool holder is shifting in the spindle at high rpm.
--
Mr. P.V.'d (formerly Droll Troll), Yonkers, NY
Ever-preparing for The Grand Insertion
Party Nominee, IPPVM
Independent Party of the Proctologically Violated®© (M)asses
"That's proly not a hemorrhoid you're feeling.... "
entropic3.14decay at optonline2.718 dot net; remove pi and e to reply--ie,
all d'numbuhs

Post by Anthony

Post by The R in SPR
Okay SVL,
I indicate the shank of the drill in #0 jacobs chuck and see .002 TIR.
I install 0.140 gage pin in newer 180DA 9/64 dia collet and chuck and
see .0015 TIR
I install 1/8" shank solid carbide endmill in older 1/8" collet and
see .0015 TIR
I install same 1/8" shank endmill in set screw style endmill holder
and see .0001 TIR
I install 1/8" drill bit in same set screw style endmill holder and
see .0001 TIR at shank of drill.
I'm thinking pay dirt now, so I spot and drill a series of 28 holes
with drill in endmill holder. (1/2 x 3 1/2" 6061-T651)
g99g83z-0.56 r0.1 q0.05 f20.0 for the drill.
Upon inspection, 0.126 pin goes through, 0.129 pin goes in about
0.10". While drilling, I observe the drill chattering as it rapids
into the hole. There is a polygonal chattery raised burr at the entry
to each hole.

*something* is loose, somewhere. It seems to appear when a load is first
put on the spindle, from your descriptions.
Mount a large EM or pin (3/4" or so) in a holder and put it in the
spindle. Set up an indicator on the flange of the holder in the Z
direction. Place a second indicator on the front of the spindle (Y axis
direction) near the tool holder. Place a third on the spindle near the
tool holder in the X axis direction. Get a couple blocks of wood and a
short 2x4 to use as a catelever. Use the wood to press up on the end of
the EM/pin and see how much deflection you get on the indicators.
If there is deflection, then you have to narrow it down to the source
from there. There would be 3 main possible culprits, a) bearings/gibs of
the Z axis, b) spindle thrust bearings or preload and c) something in the
tool clamping or a taper mismatch issue.
--
Anthony
You can't 'idiot proof' anything....every time you try, they just make
better idiots.
Remove sp to reply via email

[Charlie Gary]

Post by The R in SPR
Hello all.
I read this newsgroup a few times a year and have posted once or twice.
I just started trying to use our new VF-2. (IMTS booth machine, 10K rpm)
I had a re-order job that I'd ran previously on our 2-year old VF-2 (Brand
new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making chips
and break my .070" drill.

<<Snip>>

Post by The R in SPR
I've checked the obvious things I can think of.
Please help!

Does the machine have linear ways on the z axis? Do you have something
very flat that can be used to check z-axis runout, as in run an
indicator up and down on an angle plate? Your linear ways might be a
little out of whack in one spot, causing your head to jog a little to
the side as it goes up and down. Sure is hard on those little drills.

Later,

Charlie

[The R in SPR]

Thanks, I'm gonna try that.

Scott

Post by Charlie Gary

Post by The R in SPR
Hello all.
I read this newsgroup a few times a year and have posted once or twice.
I just started trying to use our new VF-2. (IMTS booth machine, 10K rpm)
I had a re-order job that I'd ran previously on our 2-year old VF-2 (Brand
new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making chips
and break my .070" drill.

<<Snip>>

Post by The R in SPR
I've checked the obvious things I can think of.
Please help!

Does the machine have linear ways on the z axis? Do you have something
very flat that can be used to check z-axis runout, as in run an
indicator up and down on an angle plate? Your linear ways might be a
little out of whack in one spot, causing your head to jog a little to
the side as it goes up and down. Sure is hard on those little drills.
Later,
Charlie

[The R in SPR]

Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.

Scott

Post by Charlie Gary

Post by The R in SPR
Hello all.
I read this newsgroup a few times a year and have posted once or twice.
I just started trying to use our new VF-2. (IMTS booth machine, 10K rpm)
I had a re-order job that I'd ran previously on our 2-year old VF-2 (Brand
new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making chips
and break my .070" drill.

<<Snip>>

Post by The R in SPR
I've checked the obvious things I can think of.
Please help!

Does the machine have linear ways on the z axis? Do you have something
very flat that can be used to check z-axis runout, as in run an
indicator up and down on an angle plate? Your linear ways might be a
little out of whack in one spot, causing your head to jog a little to
the side as it goes up and down. Sure is hard on those little drills.
Later,
Charlie

[Charlie Gary]

Post by The R in SPR
Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.
Scott

Is the wiggle very gradual, or concentrated in one area?

Later,

Charlie

[Charlie Gary]

Post by Charlie Gary

Post by The R in SPR
Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.
Scott

Is the wiggle very gradual, or concentrated in one area?

Also, is the plane of the angle plate face perpindicular or parallel to
the plane that would be parallel to the ways? Either way, rotate it
90 degrees and check the runout again.

Later,

Charlie

[r***@msn.com]

Was the old machine 10k rpm's too?
if it is a 7500 machine, and now you are running 10k, with that drill
chuck, you may be "throwing" the driil out, switch to an ER16 or ER11
collet.

Maybe?

Darrell

[The R in SPR]

Yes it is 10k,
I know I may be better served to drill from collets, but I still use chucks
and why the different results?
I mean same drill in same chuck in same cat 40 holder but in different
machine?
I don't get it

Thanks
Scott

Post by r***@msn.com
Was the old machine 10k rpm's too?
if it is a 7500 machine, and now you are running 10k, with that drill
chuck, you may be "throwing" the driil out, switch to an ER16 or ER11
collet.
Maybe?
Darrell

[Anthony]

Post by The R in SPR
Yes it is 10k,
I know I may be better served to drill from collets, but I still use
chucks and why the different results?
I mean same drill in same chuck in same cat 40 holder but in different
machine?
I don't get it

Scott,
To explain a bit:
If you go up 2500 rpm (from 7500 to 10k), that may be enough to make the
drill come out of center due to centrifugal force. This would explain the
tapered hole very well. A longer drill would be worse. Take a short
carbide drill and drill the same hole and see if the taper goes away.
We have some 60k RPM spindles, 15k is minimum speed. If you put a HSS or
any normal steel drill in it, the drill will never make it to the part.
The centrifugal force will spin the drill out of center so bad it will
break at spindle ramp-up. Gotta use carbide only in those (and short
ones at that).

[r***@msn.com]

what is the "r" plane in the program?

"D"

[The R in SPR]

g99 g83 z-0.55 r0.1 q0.05

Post by r***@msn.com
what is the "r" plane in the program?
"D"

[The R in SPR]

Both machines are 10K. I should have been clearer about that from the
beginning.

Post by Anthony

Post by The R in SPR
Yes it is 10k,
I know I may be better served to drill from collets, but I still use
chucks and why the different results?
I mean same drill in same chuck in same cat 40 holder but in different
machine?
I don't get it

Scott,
If you go up 2500 rpm (from 7500 to 10k), that may be enough to make the
drill come out of center due to centrifugal force. This would explain the
tapered hole very well. A longer drill would be worse. Take a short
carbide drill and drill the same hole and see if the taper goes away.
We have some 60k RPM spindles, 15k is minimum speed. If you put a HSS or
any normal steel drill in it, the drill will never make it to the part.
The centrifugal force will spin the drill out of center so bad it will
break at spindle ramp-up. Gotta use carbide only in those (and short
ones at that).
--
Anthony
You can't 'idiot proof' anything....every time you try, they just make
better idiots.
Remove sp to reply via email

[Gary]

On Tue, 24 Oct 2006 22:45:48 -0400, "The R in SPR"

Post by The R in SPR
Both machines are 10K. I should have been clearer about that from the
beginning.

I may have missed this in an earlier message; but, are the coolants
identical?

[The R in SPR]

We have been using trim E206 for a few years, but sometimes have a foam
issue.
So we're trying trim 270 in this mill, so no.

Scott

Post by Gary
On Tue, 24 Oct 2006 22:45:48 -0400, "The R in SPR"

Post by The R in SPR
Both machines are 10K. I should have been clearer about that from the
beginning.

I may have missed this in an earlier message; but, are the coolants
identical?
--
Gary B.

[Dave Lyon]

Post by The R in SPR
We have been using trim E206 for a few years, but sometimes have a foam
issue.
So we're trying trim 270 in this mill, so no.
Scott

I've had issues tapping aluminum where the coolant meant the difference
between a broken tap and a good hole. You've checked enough stuff to make
this issue seem important.

[Why]

Post by The R in SPR
We have been using trim E206 for a few years, but sometimes have a foam
issue.
So we're trying trim 270 in this mill, so no.
Scott

New Toilet water in new mill, old E-206 Toilet water in old mill.
Old mill worked new mill don't, Hmm.

[The R in SPR]

Yeah,
After I lugged plate off machine, I decided I should have checked each 90
degree.
So I'll do that first thing tomorrow.
Thanks

Post by Charlie Gary

Post by Charlie Gary

Post by The R in SPR
Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.
Scott

Is the wiggle very gradual, or concentrated in one area?

Also, is the plane of the angle plate face perpindicular or parallel to
the plane that would be parallel to the ways? Either way, rotate it
90 degrees and check the runout again.
Later,
Charlie

[Gary H. Lucas]

Post by The R in SPR
Yeah,
After I lugged plate off machine, I decided I should have checked each 90
degree.
So I'll do that first thing tomorrow.
Thanks

This may sound silly, but are you sure you aren't overfeeding the drill? I
had a problem like you describe at lower speeds simply from pushing too hard
and bowing the drill bit out of column. There may be a difference in feed
rates between old machine and new.

Gary H. Lucas

[The R in SPR]

The original feedrate from old program was 30 IPM. (.070/0.149 dia. drills
10000 rpm 6061-t651 bar stock .003 ipr I don't think is too much)
When a started having troubles, the first thing I did was back the feedrate
to 15IPM.
In running tests from mill to mill I used the same 15 IPM feedrate.
Could the machine be feeding faster than commanded? the overrides are all at
100 percent. I'm certain of that.

Scott

Post by Gary H. Lucas

Post by The R in SPR
Yeah,
After I lugged plate off machine, I decided I should have checked each
90 degree.
So I'll do that first thing tomorrow.
Thanks

This may sound silly, but are you sure you aren't overfeeding the drill?
I had a problem like you describe at lower speeds simply from pushing too
hard and bowing the drill bit out of column. There may be a difference in
feed rates between old machine and new.
Gary H. Lucas

[D Murphy]

Post by The R in SPR
The original feedrate from old program was 30 IPM. (.070/0.149 dia.
drills 10000 rpm 6061-t651 bar stock .003 ipr I don't think is too
much) When a started having troubles, the first thing I did was back
the feedrate to 15IPM.
In running tests from mill to mill I used the same 15 IPM feedrate.
Could the machine be feeding faster than commanded? the overrides are
all at 100 percent. I'm certain of that.

Program a 5" long G1 Z move at 15 IPM. Time it, it should take 20 seconds.

[The R in SPR]

I haven't a watch on now, but I command both machines as you say, press
cycle start, walk to other machine, press cycle start and they finish as
expected.

Scott

Post by D Murphy

Post by The R in SPR
The original feedrate from old program was 30 IPM. (.070/0.149 dia.
drills 10000 rpm 6061-t651 bar stock .003 ipr I don't think is too
much) When a started having troubles, the first thing I did was back
the feedrate to 15IPM.
In running tests from mill to mill I used the same 15 IPM feedrate.
Could the machine be feeding faster than commanded? the overrides are
all at 100 percent. I'm certain of that.

Program a 5" long G1 Z move at 15 IPM. Time it, it should take 20 seconds.
--
Dan
Scopulus est usquequaque nefas

[D Murphy]

Post by The R in SPR
I haven't a watch on now, but I command both machines as you say, press
cycle start, walk to other machine, press cycle start and they finish as
expected.

I'm thinking that the head isn't square on the slide or the ways aren't
perpendicular to the table. I think that you checked an angle block with an
indicator mounted in the spindle, jogging Z up and down. That would tell
you if the Z axis ways are perpendicular.

I would put a mag base indicator on the table and tram a test bar in the
spindle while jogging Z up and down.

Next Sweep the table with an indicator mounted in the spindle.

I would also put the indicator in various places and push and pull on all
axes to check for slop.

Something is out of square or loose.

[Steve A]

Post by The R in SPR
The original feedrate from old program was 30 IPM. (.070/0.149 dia. drills
10000 rpm 6061-t651 bar stock .003 ipr I don't think is too much)
When a started having troubles, the first thing I did was back the feedrate
to 15IPM.
In running tests from mill to mill I used the same 15 IPM feedrate.
Could the machine be feeding faster than commanded? the overrides are all at
100 percent. I'm certain of that.
Scott

Since you're already cutting the feed 50%, why not try cutting the
spindle speed 50%? This will keep your original feed per rev. If there
is a problem at max speed, perhaps the drawbar pull force is below spec,
then this might cure it. Or if there's no improvement, it just
eliminates high speed as a problem.

SteveA

[Garlicdude]

Post by Charlie Gary

Post by The R in SPR
Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.
Scott

Is the wiggle very gradual, or concentrated in one area?
Later,
Charlie

Gotta be a joke in there somewhere.

[S***@flashlight.net]

Post by Garlicdude

Post by Charlie Gary

Post by The R in SPR
Charlie,
It is w/in .0005 over 11" of z travel. 12 x 16 stock suburban tool angle
plate.
Scott

Is the wiggle very gradual, or concentrated in one area?
Later,
Charlie

Gotta be a joke in there somewhere.

Somewhere

----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
http://www.newsfeeds.com The #1 Newsgroup Service in the World! 120,000+ Newsgroups
----= East and West-Coast Server Farms - Total Privacy via Encryption =----

[Proctologically Violated©®]

Sumpn no one mentioned, from what I read:
Mebbe the spindle receiving the cat40 tool holder, or the retention knob or
sumpn ain't fitting right, which wouldn't show up in static-type tests, but
would under high rpm.
At very high rpm, the cat 40 holder might be cocked, w/ so much centrifugal
force that you won't hear a rattle.
Mebbe chuck up something a little eccentrically mounted in the holder in
question, and slowly ramp up the rpm, mebbe you'll hit a resonant frequency
and hear a telltale sound or rattle or sumpn.

It's possible in some machines that the tool holder was half-assed in the
spindle/rention knob holder, rattled around for a while, and fucked up the
spindle.
Of course, at 1,000 rpm and 10 ipm, I would never notice such things. :)
--
Mr. P.V.'d (formerly Droll Troll)
Ever-preparing for The Grand Insertion
Party Nominee, IPPVM
Independent Party of the Proctologically Violated®© (M)asses
"That's proly not a hemorrhoid you're feeling.... "
entropic3.14decay at optonline2.718 dot net; remove pi and e to reply--ie,
all d'numbuhs

Post by The R in SPR
Hello all.
I read this newsgroup a few times a year and have posted once or twice.
I just started trying to use our new VF-2. (IMTS booth machine, 10K rpm)
I had a re-order job that I'd ran previously on our 2-year old VF-2 (Brand
new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making
chips and break my .070" drill.
Break a few more, (standard drills, spot drilled holes). I'm thinking bad
drills, find old drill (short drill, split point) break old drill. Find
another older drill, reduce feed rate and drill a few holes.
When I inspect holes, they are big towards the top. (.073 pin starts in
hole, .070 goes through).
Now I suspect something else.
I take spot drill/.070 drill in chuck from new machine to old machine,
drill with same tooling/drilling parameters etc. .070 pin is tight, .069
pin goes like nice, like it has for thousands of times.
Haas service comes out, checks out new mill says everything is good
mechanically.
Now they request machine parameters to compare new vs old.
I've checked the obvious things I can think of.
Please help!
Thanks,
Scott

[steve bellamy]

Post by The R in SPR
Hello all.
I read this newsgroup a few times a year and have posted once or
twice. I just started trying to use our new VF-2. (IMTS booth machine,
10K rpm) I had a re-order job that I'd ran previously on our 2-year
old VF-2 (Brand new from factory)
Parts have 24 or so #2-56 holes. I load up the programs, start making
chips and break my .070" drill.
Break a few more, (standard drills, spot drilled holes). I'm thinking
bad drills, find old drill (short drill, split point) break old drill.
Find another older drill, reduce feed rate and drill a few holes.
When I inspect holes, they are big towards the top. (.073 pin starts
in hole, .070 goes through).
Now I suspect something else.
I take spot drill/.070 drill in chuck from new machine to old machine,
drill with same tooling/drilling parameters etc. .070 pin is tight,
.069 pin goes like nice, like it has for thousands of times.
Haas service comes out, checks out new mill says everything is good
mechanically.
Now they request machine parameters to compare new vs old.
I've checked the obvious things I can think of.
Please help!
Thanks,
Scott

The Haas VF0E we had for four years started breaking big carbide drills
(12mm and 16mm) a couple of years ago, giving the impression of a sudden
surge on the Z axis, and Haas reckoned the software needed updating. So
we had the new software after moaning at the price (450 pounds) but it
did the trick and has been okay since.
We wanted to know why the machine would suddenly start breaking drills
but they had no answer to that.Possibly electronic components getting old
and out of spec that new software would accommodate.
Anyway, probably not related to your problem unless you've got a dodgy
drivecard or something.
Best of luck with it!

Steve Bellamy