G61.1 on a Mazak

[Bob]

The firm I work for has recently got 2 Mazak variaxis 630's with fusion controls.

When machining complex toolpaths with high feed rates using ISO programs in 2d or 3d, we currently
use G61.1. But this seems to slow the machine feed down a lot in small corners, complex contours
etc, far more than we would expect, and a lot more than our other 5 machines do.

The only mention of G61.1 we can find in the manual refers to being used in conjunction with G05,
we cant find any mention of using it on its own. But this is what the machine selects when running
a mazatrol programs.

We've just tried G05 and G61.1 once and it made no difference in cycle time, and it doesn't seem to
work with G54.2 active, which we use all the time. But we are still looking into this at the
moment.

We tried using G64, this kept the feed up, but rounded corners off too much to hold drawing limits.
We've tried putting a K value after the G61.1, K1 made no difference to cycle time, where as K100
slowed it down even more. We also tried M830 to M821, but I don't think we have this option on, and
it made no difference. G61 slowed it down way to much as well.

As an example, one toolpath at 6000mm/min feedrate take 9 mins using G64, looks good, very smooth,
but part scrap as all corners have bigs rads on them.

Using G61.1 the same toolpath takes 14 mins, and the motion seems very 'stop start'. Everything
else tried was slower too.

Is this just the limits of the machine, or is there a way to improve things, maybe parameters to
change to loosen up the tolerance of the machine a bit, or acceleration and deceleration values?

We have noticed that when ramping down the outside of a closed profile, say 4mm deep every time
round, until 40mm deep. Then doing a final pass at depth, the 'ramping' passes are a lot smoother
and faster than the 'final' (constant Z depth pass).

I know our DMG 5 axis machines using Heidenhain contols can use a 'tolerance' command to speed
thing up for roughing or open tolerance parts etc. But even if not using this, they are a lot
faster and smoother than the new Mazaks, tho they are a lot smaller machine.

Any advice would be welcome.

Cheers.

[LillardMfg]

Post by Bob
When machining complex toolpaths with high feed rates using ISO programs in
2d or 3d, we currently
use G61.1. But this seems to slow the machine feed down a lot in small
corners, complex contours
etc, far more than we would expect, and a lot more than our other 5 machines do.

I've been wondering about these same issues. I have a PFH5800, which has a much
higher accel/decel rate than the Variaxis, so it manages to hold the corners a
lot better at high feedrates with no G61.1. If I enter a G05 in the program, I
just get an alarm telling me I don't have that option.

I clearly recall seeing the G61.1 parameters in one of the manuals, and there's
definitely a way to loosen up the tolerances. I want to say it's in the
Operators manual. I know it's not in the Mazatrol manual.

Other than the feed issue, are you satisfied with the overall performance of
the machine?

[Bob]

Post by LillardMfg

Post by Bob
When machining complex toolpaths with high feed rates using ISO programs in
2d or 3d, we currently
use G61.1. But this seems to slow the machine feed down a lot in small
corners, complex contours
etc, far more than we would expect, and a lot more than our other 5 machines do.

I've been wondering about these same issues. I have a PFH5800, which has a much
higher accel/decel rate than the Variaxis, so it manages to hold the corners a
lot better at high feedrates with no G61.1. If I enter a G05 in the program, I
just get an alarm telling me I don't have that option.
I clearly recall seeing the G61.1 parameters in one of the manuals, and there's
definitely a way to loosen up the tolerances. I want to say it's in the
Operators manual. I know it's not in the Mazatrol manual.
Other than the feed issue, are you satisfied with the overall performance of
the machine?

The feed issue is a major problem at the moment, as the machines are just not as fast as our
current machines, which is not what was hoped for when we bought them.

We also have had a couple of pallet changing issues...

I'll reserve judgement on the machines until after we get this sorted.

Cheers.

[JJ]

Call Mazak and see what they have to say about your other machines being
faster.

Post by Bob

Post by LillardMfg

Post by Bob
When machining complex toolpaths with high feed rates using ISO programs in
2d or 3d, we currently
use G61.1. But this seems to slow the machine feed down a lot in small
corners, complex contours
etc, far more than we would expect, and a lot more than our other 5
machines
do.

I've been wondering about these same issues. I have a PFH5800, which has a much
higher accel/decel rate than the Variaxis, so it manages to hold the corners a
lot better at high feedrates with no G61.1. If I enter a G05 in the program, I
just get an alarm telling me I don't have that option.
I clearly recall seeing the G61.1 parameters in one of the manuals, and there's
definitely a way to loosen up the tolerances. I want to say it's in the
Operators manual. I know it's not in the Mazatrol manual.
Other than the feed issue, are you satisfied with the overall performance of
the machine?

The feed issue is a major problem at the moment, as the machines are just
not as fast as our
current machines, which is not what was hoped for when we bought them.
We also have had a couple of pallet changing issues...
I'll reserve judgement on the machines until after we get this sorted.
Cheers.

---
Outgoing mail is certified Virus Free.
Checked by AVG anti-virus system (http://www.grisoft.com).
Version: 6.0.806 / Virus Database: 548 - Release Date: 05/12/2004

[Anthony]

Post by Bob
The firm I work for has recently got 2 Mazak variaxis 630's with fusion controls.
When machining complex toolpaths with high feed rates using ISO
programs in 2d or 3d, we currently use G61.1. But this seems to slow
the machine feed down a lot in small corners, complex contours etc,
far more than we would expect, and a lot more than our other 5
machines do.
The only mention of G61.1 we can find in the manual refers to being
used in conjunction with G05, we cant find any mention of using it on
its own. But this is what the machine selects when running a mazatrol
programs.
We've just tried G05 and G61.1 once and it made no difference in cycle
time, and it doesn't seem to work with G54.2 active, which we use all
the time. But we are still looking into this at the moment.
We tried using G64, this kept the feed up, but rounded corners off too
much to hold drawing limits. We've tried putting a K value after the
G61.1, K1 made no difference to cycle time, where as K100 slowed it
down even more. We also tried M830 to M821, but I don't think we have
this option on, and it made no difference. G61 slowed it down way to
much as well.
As an example, one toolpath at 6000mm/min feedrate take 9 mins using
G64, looks good, very smooth, but part scrap as all corners have bigs
rads on them.
Using G61.1 the same toolpath takes 14 mins, and the motion seems very
'stop start'. Everything else tried was slower too.
Is this just the limits of the machine, or is there a way to improve
things, maybe parameters to change to loosen up the tolerance of the
machine a bit, or acceleration and deceleration values?
We have noticed that when ramping down the outside of a closed
profile, say 4mm deep every time round, until 40mm deep. Then doing a
final pass at depth, the 'ramping' passes are a lot smoother and
faster than the 'final' (constant Z depth pass).
I know our DMG 5 axis machines using Heidenhain contols can use a
'tolerance' command to speed thing up for roughing or open tolerance
parts etc. But even if not using this, they are a lot faster and
smoother than the new Mazaks, tho they are a lot smaller machine.
Any advice would be welcome.
Cheers.

What you may wish to use instead of G64 is G62 (if available....not sure
which code set you are using). Whereas G64 is block change without
feedrate reduction, G62 is block change with feedrate reduction. The
reduced feedrate is generally set in a machine parameter.
There are three methods for attacking this problem..
If G62 is a valid command in your code set, you can set the feed at block
change parameter to one that suits your cycle time and quality
requirements.
The other option, and I strongly suggest you try this first, is to
tighten up the positioning tolerance for G64. This is set in a parameter
also. I do not have any Mazak books here at the house. Be aware, if you
set it too tight, and your feedrates are too high, the machine may not
physically be able to follow the path described. You may notice
excessive jerk at corners, which may effect quality.
You can also change the feed in the corner moves, while still using G64.
Note that G64 is described as block change without feedrate reduction,
however, that does not mean you cannot change feedrates between blocks,
it means that the machine will not decelerate to 0 feed at block change.
It will change the feedrate in a linear manner starting at the normal
deceleration point of the end of the current block, and ending with the
normal acceleration endpoint of the following block. This is effective
for exiting a corner also.

[Anthony]

Post by Anthony
What you may wish to use instead of G64 is G62 (if available....not
sure which code set you are using). Whereas G64 is block change
without feedrate reduction, G62 is block change with feedrate
reduction. The reduced feedrate is generally set in a machine
parameter. There are three methods for attacking this problem..
If G62 is a valid command in your code set, you can set the feed at
block change parameter to one that suits your cycle time and quality
requirements.
The other option, and I strongly suggest you try this first, is to
tighten up the positioning tolerance for G64. This is set in a
parameter also. I do not have any Mazak books here at the house. Be
aware, if you set it too tight, and your feedrates are too high, the
machine may not physically be able to follow the path described. You
may notice excessive jerk at corners, which may effect quality.
You can also change the feed in the corner moves, while still using
G64. Note that G64 is described as block change without feedrate
reduction, however, that does not mean you cannot change feedrates
between blocks, it means that the machine will not decelerate to 0
feed at block change. It will change the feedrate in a linear manner
starting at the normal deceleration point of the end of the current
block, and ending with the normal acceleration endpoint of the
following block. This is effective for exiting a corner also.

Look at parameters K7 and U48
K7 is the deceleration percentage for automatic corner override, U48 is
the deceleration approach distance for automatic corner override.
Please check your Parameter and Alarm List book for further info.

[Bob]

Post by Anthony

Post by Bob
The firm I work for has recently got 2 Mazak variaxis 630's with fusion controls.
When machining complex toolpaths with high feed rates using ISO
programs in 2d or 3d, we currently use G61.1. But this seems to slow
the machine feed down a lot in small corners, complex contours etc,
far more than we would expect, and a lot more than our other 5
machines do.
The only mention of G61.1 we can find in the manual refers to being
used in conjunction with G05, we cant find any mention of using it on
its own. But this is what the machine selects when running a mazatrol
programs.
We've just tried G05 and G61.1 once and it made no difference in cycle
time, and it doesn't seem to work with G54.2 active, which we use all
the time. But we are still looking into this at the moment.
We tried using G64, this kept the feed up, but rounded corners off too
much to hold drawing limits. We've tried putting a K value after the
G61.1, K1 made no difference to cycle time, where as K100 slowed it
down even more. We also tried M830 to M821, but I don't think we have
this option on, and it made no difference. G61 slowed it down way to
much as well.
As an example, one toolpath at 6000mm/min feedrate take 9 mins using
G64, looks good, very smooth, but part scrap as all corners have bigs
rads on them.
Using G61.1 the same toolpath takes 14 mins, and the motion seems very
'stop start'. Everything else tried was slower too.
Is this just the limits of the machine, or is there a way to improve
things, maybe parameters to change to loosen up the tolerance of the
machine a bit, or acceleration and deceleration values?
We have noticed that when ramping down the outside of a closed
profile, say 4mm deep every time round, until 40mm deep. Then doing a
final pass at depth, the 'ramping' passes are a lot smoother and
faster than the 'final' (constant Z depth pass).
I know our DMG 5 axis machines using Heidenhain contols can use a
'tolerance' command to speed thing up for roughing or open tolerance
parts etc. But even if not using this, they are a lot faster and
smoother than the new Mazaks, tho they are a lot smaller machine.
Any advice would be welcome.
Cheers.

What you may wish to use instead of G64 is G62 (if available....not sure
which code set you are using). Whereas G64 is block change without
feedrate reduction, G62 is block change with feedrate reduction. The
reduced feedrate is generally set in a machine parameter.
There are three methods for attacking this problem..
If G62 is a valid command in your code set, you can set the feed at block
change parameter to one that suits your cycle time and quality
requirements.
The other option, and I strongly suggest you try this first, is to
tighten up the positioning tolerance for G64. This is set in a parameter
also. I do not have any Mazak books here at the house. Be aware, if you
set it too tight, and your feedrates are too high, the machine may not
physically be able to follow the path described. You may notice
excessive jerk at corners, which may effect quality.
You can also change the feed in the corner moves, while still using G64.
Note that G64 is described as block change without feedrate reduction,
however, that does not mean you cannot change feedrates between blocks,
it means that the machine will not decelerate to 0 feed at block change.
It will change the feedrate in a linear manner starting at the normal
deceleration point of the end of the current block, and ending with the
normal acceleration endpoint of the following block. This is effective
for exiting a corner also.

Thanks for the info, I thought G62 was only for internal corners, and its external corners we have
trouble with, being rounded to much at high feed rates. I will give it a try tomorrow at work.

As you say, I think getting G64 to work to a tighter tolerance is the way to go, I will look into
this also, tho the parameter meanings are often as clear as mud.

We found out today G61.1 only works for 2d, which is why the machine is faster when ramping down.
But we don't seem to have the corner rounding problem when ramping?

Do you know what G61.1 actually does, as in the manual the only reference we can see is 'shape
correction' when using G05, which we are not. But it does do something when used alone?

Cheers.

[ff]

Post by Bob
Thanks for the info, I thought G62 was only for internal corners, and its external corners we have
trouble with, being rounded to much at high feed rates. I will give it a try tomorrow at work.
As you say, I think getting G64 to work to a tighter tolerance is the way to go, I will look into
this also, tho the parameter meanings are often as clear as mud.
We found out today G61.1 only works for 2d, which is why the machine is faster when ramping down.
But we don't seem to have the corner rounding problem when ramping?
Do you know what G61.1 actually does, as in the manual the only reference we can see is 'shape
correction' when using G05, which we are not. But it does do something when used alone?
Cheers.

Try different values of K with G61.1 Without looking it up, I believe
a value of 6 or 7 will give acceptable corners
without slowing the feedrate excessively.

fred

[ff]

Post by ff

Post by Bob
Thanks for the info, I thought G62 was only for internal corners, and
its external corners we have trouble with, being rounded to much at
high feed rates. I will give it a try tomorrow at work.
As you say, I think getting G64 to work to a tighter tolerance is the
way to go, I will look into this also, tho the parameter meanings are
often as clear as mud.
We found out today G61.1 only works for 2d, which is why the machine
is faster when ramping down. But we don't seem to have the corner
rounding problem when ramping?
Do you know what G61.1 actually does, as in the manual the only
reference we can see is 'shape correction' when using G05, which we
are not. But it does do something when used alone?
Cheers.

Try different values of K with G61.1 Without looking it up, I
believe a value of 6 or 7 will give acceptable corners
without slowing the feedrate excessively.
fred

Oops, that should have read "a value of 60 to 70"
Sorry about that, can't trust the memory anymore.

fred

[Bob]

Post by ff

Post by ff
Try different values of K with G61.1 Without looking it up, I
believe a value of 6 or 7 will give acceptable corners
without slowing the feedrate excessively.
fred

Oops, that should have read "a value of 60 to 70"
Sorry about that, can't trust the memory anymore.
fred

The bigger the K value, the slower it is round the corners, with 1 being the same and 100 being
very slow.

Cheers.