& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:00
Tool and work offsets.
00:02
After completing this video, you will be able to
00:05
assemble tools and tool holders
00:08
promptly set up tool offsets
00:10
properly. Locate G 54
00:13
in front of us are the tools and work pieces necessary.
00:16
In order to create our caliper pistons,
00:19
the setup sheet told us we'd be using a quarter inch Cher tool.
00:22
We have our T seven, our half inch and melt
00:25
and we have our work pieces which are 1.5 inches square and one inch tall.
00:31
Now, we have also loaded our workpiece,
00:33
the stock that will become our part into a vice on the table,
00:37
just like our setup sheet said to
00:39
the ho
00:40
control needs to know where that part is in the machine's larger work envelope.
00:45
The control also needs to know how long each
00:47
of our tools are and sometimes a tool's diameter.
00:50
All of these lengths and positions are collectively known as offsets
00:54
and are stored on the controls, offset pages.
00:57
Now we have an offset page for tools and another for our work, our work pieces.
01:03
Now, before we can set those offsets, we have to assemble and load our tools and,
01:08
and both of these tools will be held in, er, style call it holders.
01:13
Now these er, style holders make use of calls
01:16
that allow them to hold any size tool within a certain range.
01:21
Er, 16 holders can hold tools up to about 3/8 of an inch, er,
01:29
And er,
01:33
to three quarter inch or about 20 millimeters.
01:36
Larger diameter, er, holders have better grip strength,
01:39
smaller holders offer better clearance.
01:43
Long holders offer better reach, shorter.
01:45
Holders are more rigid and less likely to chatter
01:48
for these reasons.
01:49
On this part, we're going to go with two shorter, er,
01:57
Our quarter inch champer tool will need to call it that
01:60
is labeled one quarter inch or 6 to 7 millimeters.
02:03
Our half inch and mill will use a half inch or 12 to 13 millimeter col
02:08
and all of these pieces in our er, holder
02:10
need to be clean and dry before assembly.
02:15
Our colts snap into our call it nuts first before we thread the nut onto the holder
02:22
and place it in our tool holder fixture.
02:29
A shorter tool exposure is usually better,
02:32
less likely to chatter but on a champ or tool like this,
02:35
it really doesn't matter much.
02:37
Our setup sheet says that our champ or tool only needs to go Z minus 0.13 inches deep.
02:43
So, if the tool is sticking out, at least that far from the holder,
02:47
nothing should hit.
02:48
But I know I'm gonna be using this champ or tool for other jobs.
02:51
So I'm gonna set this tool stick out
02:54
to be one inch to be safe.
02:58
Now, our half inch end mill is going to a minimum Z depth of Z minus 0.715 inches.
03:06
If our tool isn't sticking out from the face of our holder by at least that amount
03:12
our holder could hit our part and we don't want that.
03:16
Now, we do not want to clamp
03:18
on a tool's flutes,
03:20
can't do that at all.
03:22
So this is about as far as we can
03:25
put the tool into the holder.
03:27
This is it.
03:27
Now,
03:28
this is much greater than the 0.715 inches of
03:31
tool exposure from the holder that we need.
03:33
This is closer to 1.8 inches, but that's just fine.
03:37
We're not gonna go any shorter with this
03:38
holder because we cannot clamp on those gullets,
03:41
those flutes.
03:43
Now, these tools are sharp, so we want to handle them like knives very carefully
03:50
from our setup sheet. We know that our champ or tool is tool two
03:55
and our half inch and mill is tool seven.
03:58
Now, we're gonna get these guys in the machine at
04:01
the machine. We need to enter MD I mode.
04:04
So we're gonna press the MD I button.
04:08
And then we'll call tool two into the spindle by pressing T two
04:13
A TC forward
04:18
MD I stands for manual data input.
04:21
And it's just a kind of scratch pad that we can use to control the machine
04:25
without having to write a real program.
04:28
Now, if that spindle is kind of out of reach for us, if we want to put a tool in,
04:32
we can jog that spindle down by pressing the handle, jog button,
04:37
choosing the 0.01 jog increment,
04:41
selecting which axis we want to jog
04:43
the Z in this case
04:45
and using the hand jog wheel.
04:48
Now, if there was already a tool in the spindle, we'd remove it. Our spindle is empty
04:53
and the control confirms that tool too is in the spindle.
04:57
So we will press and hold the tool release button on the
05:00
spindle with one hand while loading up our tool with the other.
05:03
When inserting the tool,
05:05
we have to align the gaps on our holder with the drive dogs on our spindle,
05:09
making sure that our fingers are clear of that gap between the spindle and holder.
05:14
We don't want to get pinched.
05:15
We will firmly hold the tool in that position.
05:18
As we let go of the tool release button,
05:21
we will continue to hold the tool in position for a few moments
05:24
until we have heard and felt the spindle finish the clamping process.
05:29
Now, if we made a mistake somewhere along the lines. Let's say we didn't get those,
05:33
those uh dog ears aligned with our tool holder. That's fine. Just stop
05:38
and repeat the entire process.
05:40
Now, from MD I, we'll call up tool seven T seven A TC forward,
05:46
align the tools to the spindle press and hold the
05:49
tool release button while pushing the holder into the spindle,
05:52
release the tool release button.
05:53
Wait for the spindle to fully clamp and withdraw our hand.
05:58
Well, that is it. We've got both of our tools all loaded up in the machine.
06:02
Now it's time for us to touch them off to set our tool links on the offset page.
06:07
And I want to do this in order we're gonna go back to tool two and then
06:11
set tool seven. So from MD I,
06:14
we're gonna press T two A TC forward
06:18
hand jog 0.01 increment,
06:20
we will jog our tool down just above our part jogging the appropriate XY and Z axis.
06:27
Now there are lots of advanced ways to set our tool and work offsets. In this video.
06:32
On this part running a single vice,
06:34
we're gonna set our tool offsets using the manual paper method
06:38
from our setup sheet. We know that our Z zero is the top of our part.
06:43
So that is where we are gonna set our tools.
06:45
We'll jog our tool down just above the top of our part
06:49
before switching to a slower jog increment 0.001 we will use a piece
06:54
of paper as our touch off tool will slowly rotate the jog wheel,
06:58
moving it down one click at a time while moving our paper back and forth.
07:03
When we feel the paper drag,
07:04
we know the paper is being pinched between our tool and our part,
07:09
we'll stop and go to our tool offset page by pressing the offset button.
07:13
Now, like we saw earlier, we have a tool, offset page and a work offset page
07:19
on newer
07:20
house controls, we will press the F four key to move between the two on older ho
07:25
controls. We'll just press the offset key multiple times
07:29
to switch between those offset tabs.
07:31
Tool two is in our spindle. So offset two
07:34
should be highlighted. If not, we can use the cursor keys to highlight T two.
07:39
And you can see here, it actually says spindle, which is what we want
07:44
with offset two highlighted. We'll press the tool offset measure button
07:48
and the control will save our current position as our tool length offset.
07:52
That's it.
07:53
We can jog away and navigate to tool seven.
07:56
We'll again jog a tool above our part and then reduce our jog increment to 0.001
08:01
and slowly jog our end milk towards our part
08:05
while shuffling our paper until we feel it drag,
08:08
we'll stop. Go to our tool offset page.
08:12
Make sure offset seven is highlighted
08:14
and press the tool offset measure button to record this tool's length offset.
08:20
Congratulations.
08:21
Our tool offsets are now set, we can now move on and set our work offsets.
08:26
Now, our setup sheet tells us that our part origin,
08:30
the reference zero for all of our part machining is
08:33
at the back left and top corner of our stock.
08:37
The far left column on our work offset page lists
08:39
all of the possible work coordinate systems we can use
08:43
a common practice is to just use G 54.
08:46
If we're only running a single part, a single operation and a single vice.
08:50
Now, if we're running multiple vices,
08:53
lots of different parts or lots of different operations,
08:55
we need a different work offset for each one of those setups.
08:59
So we might use G 54 for a first operation in vice one,
09:04
G 55 for another operation in vice two.
09:07
You get the idea.
09:08
So how do we know which work offset to use? Our setup sheet tells us we are using W CS one
09:15
that is work coordinate system one.
09:17
When WC SS one is selected in fusion 360 it will output a G 54
09:23
in the G code program.
09:24
Now, we can also check our G code program and look and see what work
09:28
s that we are using and we will do that. But that's a future lesson.
09:32
We need to let the control know that our G 54 location is right there on our part
09:38
to set this manually. We're gonna use our Hoss
09:41
Heimer 3D sensor. We'll load up our 3D sensor into an empty pocket in our machine
09:46
and jog it down above our part,
09:49
we'll then set each axis one at a time.
09:51
And by the way, this tool gets its name 3D sensor because it can work in any direction.
09:57
Like XY and Z,
09:59
we will slowly jog our sensor against our part moving along the
10:02
X axis until both our indicator needles large and small read zero.
10:08
Now, for more precise adjustments, we can switch our jog increment
10:12
to 0.0001. Once we're close to zero
10:17
from this front view, we can see that our indicator tip is bent
10:21
angled off to one side.
10:22
Now, this tool has been perfectly calibrated so that when it reads zero,
10:27
the center line of our spindle is directly aligned with the edge of our part.
10:32
This will be the G 54 X zero. For our part,
10:37
we can go to our work
10:38
offset page, highlight our G 54 X axis cell
10:43
and press the part zero set button. Part zero set.
10:47
The control will record this X machine position for us.
10:50
Saving it for later to be recalled from inside of our G code program.
10:54
We'll repeat this process for our Y axis
10:58
jogging towards the back edge of our part until our sensor reads zero,
11:04
then highlighting our G 54 Y axis
11:07
and pressing part zero set
11:09
done.
11:11
Now with this simple set up, we wanna make sure that our G 54 Z value is set to zero.
11:16
And this is why
11:17
our work off set Z is actually the distance from where we,
11:21
where we touched off our parts
11:23
to the top of our parts.
11:25
And in this case, we, we touched off our tools
11:28
right on top of our parts. So the distance between those two is zero,
11:34
that's why we kept things simple, set our tools on top of our raw stock.
11:39
That is it. We have told our control where our part is setting our work offset.
11:44
And we've told our hos
11:45
machine how long our tools are by setting our tool offsets.
11:49
Now, for this setup,
11:51
we chose to set our tool and work offsets manually using paper and the heimer,
11:57
that's just the way we did it. But if your machine has a probe on it,
12:01
then be sure to use it. It's much easier and faster.
12:05
You just go to the
12:06
offset pages, follow some instructions, fill in some blanks
12:10
and the control will set
12:12
our,
12:13
our offsets for us.
12:14
Uh But in this case,
12:16
you cannot. And this is the rule to remember.
12:19
You cannot mix and match the way we set tools and work offsets.
12:23
They use completely different systems.
12:24
So if you set
12:26
tool two manually,
12:28
you cannot set tool seven with the probing system,
12:31
you're gonna have problems so never mix and
12:33
match your method for setting tool offsets.
12:36
Keep things simple
12:38
and you might have noticed that we did not
12:39
cover checking our offsets just yet and that's fine
12:43
because we're gonna cover that
12:44
in an upcoming lesson.
00:00
Tool and work offsets.
00:02
After completing this video, you will be able to
00:05
assemble tools and tool holders
00:08
promptly set up tool offsets
00:10
properly. Locate G 54
00:13
in front of us are the tools and work pieces necessary.
00:16
In order to create our caliper pistons,
00:19
the setup sheet told us we'd be using a quarter inch Cher tool.
00:22
We have our T seven, our half inch and melt
00:25
and we have our work pieces which are 1.5 inches square and one inch tall.
00:31
Now, we have also loaded our workpiece,
00:33
the stock that will become our part into a vice on the table,
00:37
just like our setup sheet said to
00:39
the ho
00:40
control needs to know where that part is in the machine's larger work envelope.
00:45
The control also needs to know how long each
00:47
of our tools are and sometimes a tool's diameter.
00:50
All of these lengths and positions are collectively known as offsets
00:54
and are stored on the controls, offset pages.
00:57
Now we have an offset page for tools and another for our work, our work pieces.
01:03
Now, before we can set those offsets, we have to assemble and load our tools and,
01:08
and both of these tools will be held in, er, style call it holders.
01:13
Now these er, style holders make use of calls
01:16
that allow them to hold any size tool within a certain range.
01:21
Er, 16 holders can hold tools up to about 3/8 of an inch, er,
01:29
And er,
01:33
to three quarter inch or about 20 millimeters.
01:36
Larger diameter, er, holders have better grip strength,
01:39
smaller holders offer better clearance.
01:43
Long holders offer better reach, shorter.
01:45
Holders are more rigid and less likely to chatter
01:48
for these reasons.
01:49
On this part, we're going to go with two shorter, er,
01:57
Our quarter inch champer tool will need to call it that
01:60
is labeled one quarter inch or 6 to 7 millimeters.
02:03
Our half inch and mill will use a half inch or 12 to 13 millimeter col
02:08
and all of these pieces in our er, holder
02:10
need to be clean and dry before assembly.
02:15
Our colts snap into our call it nuts first before we thread the nut onto the holder
02:22
and place it in our tool holder fixture.
02:29
A shorter tool exposure is usually better,
02:32
less likely to chatter but on a champ or tool like this,
02:35
it really doesn't matter much.
02:37
Our setup sheet says that our champ or tool only needs to go Z minus 0.13 inches deep.
02:43
So, if the tool is sticking out, at least that far from the holder,
02:47
nothing should hit.
02:48
But I know I'm gonna be using this champ or tool for other jobs.
02:51
So I'm gonna set this tool stick out
02:54
to be one inch to be safe.
02:58
Now, our half inch end mill is going to a minimum Z depth of Z minus 0.715 inches.
03:06
If our tool isn't sticking out from the face of our holder by at least that amount
03:12
our holder could hit our part and we don't want that.
03:16
Now, we do not want to clamp
03:18
on a tool's flutes,
03:20
can't do that at all.
03:22
So this is about as far as we can
03:25
put the tool into the holder.
03:27
This is it.
03:27
Now,
03:28
this is much greater than the 0.715 inches of
03:31
tool exposure from the holder that we need.
03:33
This is closer to 1.8 inches, but that's just fine.
03:37
We're not gonna go any shorter with this
03:38
holder because we cannot clamp on those gullets,
03:41
those flutes.
03:43
Now, these tools are sharp, so we want to handle them like knives very carefully
03:50
from our setup sheet. We know that our champ or tool is tool two
03:55
and our half inch and mill is tool seven.
03:58
Now, we're gonna get these guys in the machine at
04:01
the machine. We need to enter MD I mode.
04:04
So we're gonna press the MD I button.
04:08
And then we'll call tool two into the spindle by pressing T two
04:13
A TC forward
04:18
MD I stands for manual data input.
04:21
And it's just a kind of scratch pad that we can use to control the machine
04:25
without having to write a real program.
04:28
Now, if that spindle is kind of out of reach for us, if we want to put a tool in,
04:32
we can jog that spindle down by pressing the handle, jog button,
04:37
choosing the 0.01 jog increment,
04:41
selecting which axis we want to jog
04:43
the Z in this case
04:45
and using the hand jog wheel.
04:48
Now, if there was already a tool in the spindle, we'd remove it. Our spindle is empty
04:53
and the control confirms that tool too is in the spindle.
04:57
So we will press and hold the tool release button on the
05:00
spindle with one hand while loading up our tool with the other.
05:03
When inserting the tool,
05:05
we have to align the gaps on our holder with the drive dogs on our spindle,
05:09
making sure that our fingers are clear of that gap between the spindle and holder.
05:14
We don't want to get pinched.
05:15
We will firmly hold the tool in that position.
05:18
As we let go of the tool release button,
05:21
we will continue to hold the tool in position for a few moments
05:24
until we have heard and felt the spindle finish the clamping process.
05:29
Now, if we made a mistake somewhere along the lines. Let's say we didn't get those,
05:33
those uh dog ears aligned with our tool holder. That's fine. Just stop
05:38
and repeat the entire process.
05:40
Now, from MD I, we'll call up tool seven T seven A TC forward,
05:46
align the tools to the spindle press and hold the
05:49
tool release button while pushing the holder into the spindle,
05:52
release the tool release button.
05:53
Wait for the spindle to fully clamp and withdraw our hand.
05:58
Well, that is it. We've got both of our tools all loaded up in the machine.
06:02
Now it's time for us to touch them off to set our tool links on the offset page.
06:07
And I want to do this in order we're gonna go back to tool two and then
06:11
set tool seven. So from MD I,
06:14
we're gonna press T two A TC forward
06:18
hand jog 0.01 increment,
06:20
we will jog our tool down just above our part jogging the appropriate XY and Z axis.
06:27
Now there are lots of advanced ways to set our tool and work offsets. In this video.
06:32
On this part running a single vice,
06:34
we're gonna set our tool offsets using the manual paper method
06:38
from our setup sheet. We know that our Z zero is the top of our part.
06:43
So that is where we are gonna set our tools.
06:45
We'll jog our tool down just above the top of our part
06:49
before switching to a slower jog increment 0.001 we will use a piece
06:54
of paper as our touch off tool will slowly rotate the jog wheel,
06:58
moving it down one click at a time while moving our paper back and forth.
07:03
When we feel the paper drag,
07:04
we know the paper is being pinched between our tool and our part,
07:09
we'll stop and go to our tool offset page by pressing the offset button.
07:13
Now, like we saw earlier, we have a tool, offset page and a work offset page
07:19
on newer
07:20
house controls, we will press the F four key to move between the two on older ho
07:25
controls. We'll just press the offset key multiple times
07:29
to switch between those offset tabs.
07:31
Tool two is in our spindle. So offset two
07:34
should be highlighted. If not, we can use the cursor keys to highlight T two.
07:39
And you can see here, it actually says spindle, which is what we want
07:44
with offset two highlighted. We'll press the tool offset measure button
07:48
and the control will save our current position as our tool length offset.
07:52
That's it.
07:53
We can jog away and navigate to tool seven.
07:56
We'll again jog a tool above our part and then reduce our jog increment to 0.001
08:01
and slowly jog our end milk towards our part
08:05
while shuffling our paper until we feel it drag,
08:08
we'll stop. Go to our tool offset page.
08:12
Make sure offset seven is highlighted
08:14
and press the tool offset measure button to record this tool's length offset.
08:20
Congratulations.
08:21
Our tool offsets are now set, we can now move on and set our work offsets.
08:26
Now, our setup sheet tells us that our part origin,
08:30
the reference zero for all of our part machining is
08:33
at the back left and top corner of our stock.
08:37
The far left column on our work offset page lists
08:39
all of the possible work coordinate systems we can use
08:43
a common practice is to just use G 54.
08:46
If we're only running a single part, a single operation and a single vice.
08:50
Now, if we're running multiple vices,
08:53
lots of different parts or lots of different operations,
08:55
we need a different work offset for each one of those setups.
08:59
So we might use G 54 for a first operation in vice one,
09:04
G 55 for another operation in vice two.
09:07
You get the idea.
09:08
So how do we know which work offset to use? Our setup sheet tells us we are using W CS one
09:15
that is work coordinate system one.
09:17
When WC SS one is selected in fusion 360 it will output a G 54
09:23
in the G code program.
09:24
Now, we can also check our G code program and look and see what work
09:28
s that we are using and we will do that. But that's a future lesson.
09:32
We need to let the control know that our G 54 location is right there on our part
09:38
to set this manually. We're gonna use our Hoss
09:41
Heimer 3D sensor. We'll load up our 3D sensor into an empty pocket in our machine
09:46
and jog it down above our part,
09:49
we'll then set each axis one at a time.
09:51
And by the way, this tool gets its name 3D sensor because it can work in any direction.
09:57
Like XY and Z,
09:59
we will slowly jog our sensor against our part moving along the
10:02
X axis until both our indicator needles large and small read zero.
10:08
Now, for more precise adjustments, we can switch our jog increment
10:12
to 0.0001. Once we're close to zero
10:17
from this front view, we can see that our indicator tip is bent
10:21
angled off to one side.
10:22
Now, this tool has been perfectly calibrated so that when it reads zero,
10:27
the center line of our spindle is directly aligned with the edge of our part.
10:32
This will be the G 54 X zero. For our part,
10:37
we can go to our work
10:38
offset page, highlight our G 54 X axis cell
10:43
and press the part zero set button. Part zero set.
10:47
The control will record this X machine position for us.
10:50
Saving it for later to be recalled from inside of our G code program.
10:54
We'll repeat this process for our Y axis
10:58
jogging towards the back edge of our part until our sensor reads zero,
11:04
then highlighting our G 54 Y axis
11:07
and pressing part zero set
11:09
done.
11:11
Now with this simple set up, we wanna make sure that our G 54 Z value is set to zero.
11:16
And this is why
11:17
our work off set Z is actually the distance from where we,
11:21
where we touched off our parts
11:23
to the top of our parts.
11:25
And in this case, we, we touched off our tools
11:28
right on top of our parts. So the distance between those two is zero,
11:34
that's why we kept things simple, set our tools on top of our raw stock.
11:39
That is it. We have told our control where our part is setting our work offset.
11:44
And we've told our hos
11:45
machine how long our tools are by setting our tool offsets.
11:49
Now, for this setup,
11:51
we chose to set our tool and work offsets manually using paper and the heimer,
11:57
that's just the way we did it. But if your machine has a probe on it,
12:01
then be sure to use it. It's much easier and faster.
12:05
You just go to the
12:06
offset pages, follow some instructions, fill in some blanks
12:10
and the control will set
12:12
our,
12:13
our offsets for us.
12:14
Uh But in this case,
12:16
you cannot. And this is the rule to remember.
12:19
You cannot mix and match the way we set tools and work offsets.
12:23
They use completely different systems.
12:24
So if you set
12:26
tool two manually,
12:28
you cannot set tool seven with the probing system,
12:31
you're gonna have problems so never mix and
12:33
match your method for setting tool offsets.
12:36
Keep things simple
12:38
and you might have noticed that we did not
12:39
cover checking our offsets just yet and that's fine
12:43
because we're gonna cover that
12:44
in an upcoming lesson.
After completing this video, you’ll be able to: