Tool and work offsets

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.

Video 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.

After completing this video, you’ll be able to:

  • Assemble tools and tool holders.
  • Properly set up tool offsets.
  • Properly locate G54.

Video quiz

What is the G-code for WCS 1 in the Work Offset page?

(Select one)
Select an answer

1/1 questions left unanswered

Was this information helpful?