& Construction

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

Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
Create 2.5 access tool paths.
00:05
After completing this video, you'll be able to
00:08
create a drilling operation, create a 2.5 axis roughing tool path
00:11
and create 2.5 axis finishing tool baths.
00:16
To get started in fusion, we want to begin with the supply data set. CM two X tool
00:21
pass mm dot F 3D.
00:23
When we open this design up,
00:24
it should automatically be in the manufacture workspace.
00:27
But if not ensure that you do navigate there
00:29
and double check the units are set to metric.
00:32
This design already contains a setup,
00:34
the setup has the stock set and the coordinate system in the correct location.
00:38
The design also contains tools inside of its document.
00:41
You can take a look at the very top in the document for C AM two X tool paths.
00:45
There are tools and if we clear our filters,
00:49
we can see that tools will be available for
00:51
our milling operations as well as our drilling operations.
00:55
So now that we know that we have tools and our set up,
00:58
let's go ahead and get started creating our tool paths.
01:01
There are a couple of main objectives when we're machining apart,
01:04
first,
01:05
we want to remove as much material as possible as
01:08
quickly as possible in what are called roughing operations.
01:11
And then we wanna create finishing operations that will get down to the
01:15
final shape and size of our part and leave a good surface finish.
01:18
Now, there are some general approaches to this for nearly all parts.
01:22
So we're gonna take a look at that with this part here
01:25
to get started. The first operation we want to do is create a facing tool path.
01:29
When we take a look at this thing from the front view,
01:31
we can see that there's stock above the top of our part
01:34
and there's plenty of stock below the bottom of our part.
01:37
For this example, we're not going to be discussing holding it in a vice or a fixture.
01:42
We're just going to assume that we've got plenty of space below the bottom of our part
01:46
and we're holding it inside of some sort of work holding
01:49
that we need to make sure that we don't go all the way to the bottom of our stock.
01:53
We'll talk more about vices and fixtures in some of the three Xs tool paths.
01:58
So from here, we want to face the top of our part
02:01
back in a home view, we're going to go to our two D drop down and select two D face
02:06
from here. We need to select a tool.
02:09
There are only certain types of tools
02:10
that will be applicable for facing operations.
02:13
Our flat end mill as well as a larger face mill would be a good choice
02:17
because we're working on a limited set of tools.
02:19
We're going to be using our 12 millimeter flat end mill or tool. Number one,
02:24
we're gonna be using aluminum finishing for our cutting data.
02:27
This is because a facing tool path does remove raw
02:30
or rough stock from the outside of our part.
02:32
But the surface that it cuts down to will be the final top surface of our part,
02:36
we'll select the tool and that cutting preset.
02:39
Noting that in the feeds and speeds section, those values are now populated
02:43
from here. We're gonna move on to our geometry section
02:46
and with a facing tool path, it automatically gets the outside profile of our stock.
02:51
So we see an orange border on the screen and this tells us that no selection is needed.
02:56
Next in our height section,
02:58
we've got various planes that are gonna dictate what happens with the tool.
03:02
And when
03:03
we have a clearance plane at the very top, followed by a retract plane,
03:07
our feet height plane, the top height and the bottom height.
03:11
By default, with a facing tool path,
03:13
the top height will be the top of our stock
03:15
and the bottom height will be the top of our model
03:18
because of this, we don't need to make any changes or selections.
03:22
But as you begin machining more and more.
03:24
You'll find that reducing the height between things like our clearance plane,
03:28
retract plane and the feed height can drastically speed up the programs.
03:33
What I mean by this is there are different speeds at which the tool is gonna travel,
03:37
the rapid movements and the feed movements
03:39
changing where those happen can really speed up the machining process.
03:43
Reducing the amount of time you're spending, not cutting material.
03:47
Next, we're gonna move over to our passes section
03:50
in the passes section.
03:51
We've got a couple of options, but we're not going to change too much here.
03:54
First note that we've got our pass direction reference.
03:58
This is gonna allow us to change which direction the tool is going by default,
04:02
it'll be going along the X and Y directions.
04:05
Also as we go down, you can see that we've got a pass extension.
04:09
This is gonna be half of our tool or the radius value of our tool.
04:13
This means that the tool is going to extend past
04:15
the end of our stock before it turns around.
04:18
There's also a step over value and in this case, 1.7 millimeters is relatively low.
04:23
I'm gonna set this just shy of the diameter of our tool at 11 millimeters.
04:29
Next, we have a direction reference by default, it's gonna go both ways.
04:33
But if you have a specific machining direction, for example,
04:36
climb or conventional, you can change those.
04:38
Here.
04:39
There is a new option called order for shorter links that can reduce
04:43
the amount of time it takes to machine or face our part.
04:46
However, order for shorter links only works.
04:48
If you change your direction to a specific climb or conventional direction,
04:52
it won't work with the both option.
04:55
There's also a from other side and use chip
04:57
thinning which we're going to omit for right now.
05:00
And in the linking section,
05:01
this is gonna dictate how the tool moves into and out of our cuts.
05:05
And we're gonna leave these as default for now and say, OK,
05:08
once done, we'll get a preview on the screen,
05:10
showing us a green preview of the stock as well as
05:14
the lines that the tool is going to be traveling.
05:16
If we go back to our front view,
05:17
we can now see that the stock is cut down to the top of our part.
05:21
This is done showing us in process stock and
05:24
the visibility can be changed by going down to this
05:26
bottom section in fusion and turning on or off the
05:29
in process stock or by going to our tool,
05:32
visibility
05:32
going on and off for the tool.
05:35
And we can also turn on and off our tool paths.
05:39
This can help especially once we get into more complex
05:41
tool paths that have much more movements on the screen.
05:44
But for right now, we're gonna leave them as is.
05:46
So anytime we click on our facing tool path, we'll get a preview
05:50
now that we face the top of our part,
05:52
we're going to move on to doing some roughing operations
05:55
in the two D tools.
05:56
We've got a two D adaptive clearing,
05:58
which is a wonderful option for nearly all types of parts.
06:02
There are other options such as two D pocket for clearing.
06:05
But the two D adaptive is going to allow us to cut
06:07
a little bit deeper and keep a consistent load on our tool.
06:10
We're going to select two D adaptive clearing.
06:13
We're gonna be using the same tool moving on to our geometry selection
06:17
and we're going to select the bottom outside edge of our part.
06:20
There'll be a blue preview on the screen and this is gonna
06:23
let us know which side of the part is gonna be cut.
06:26
You also note that this goes out to the size of our stock,
06:29
so no other selections are needed.
06:31
Next, we're gonna go to our height section at
06:34
this point.
06:35
All of the heights are going to be ok because
06:37
the bottom height is based on our selected contour.
06:39
However, a two D adaptive tool path is a roughing tool path,
06:44
which means it's intended to leave stock behind.
06:47
And that's gonna not allow us to cut all the way down to the bottom of our part.
06:50
So if we view this from a front view again,
06:52
and we go down to our bottom height and the selected contours
06:55
and we add, say two millimeters
06:58
that's going to allow the tool to go two
06:59
millimeters relative to the bottom of our part.
07:02
However, the positive value is in the positive Z direction.
07:06
Because of the coordinate system, we need to use a negative value.
07:09
If we make this change, all we need to do is edit our tool path,
07:13
go to our height section
07:14
and change the offset value to minus two millimeters and say, OK.
07:19
Now the preview on the screen shows the tool path
07:21
cutting two millimeters below the bottom of our part.
07:24
Let's go ahead and take one quick look at the rest of the settings.
07:27
Before we move on to the next tool path.
07:30
In the passive section,
07:31
we have some values in here such as optimal load that are going to determine
07:35
how much engagement we have between our tool and the material that it's cutting.
07:39
We have a default stock to leave.
07:41
In this case,
07:42
it's half a millimeter in the radial direction and the axial direction.
07:46
This means on the side of the tool and on the bottom of the tool.
07:49
Next, we also have a multiple depths option.
07:52
In this case, our tool can make this cut with a single depth.
07:55
But if we had to cut extremely deep into a part, we may need to toggle that on.
08:00
The next option here is multi
08:02
axis which we're not taking a look at. And the last one is linking
08:05
by default, it'll do a helo
08:07
entry and we're gonna leave all of these values as default and say, OK,
08:12
back in a home view,
08:13
we can now see that we've cleared the material around the outside
08:15
of our part all the way to two millimeters below the part
08:19
minus that extra half a millimeter that it's leaving for a stock to leave.
08:23
Now, we want to remove the material from this phase.
08:26
We can do this in a single operation,
08:28
but it's good practice to go back and do this a couple of different times.
08:31
So we're going to use the same process using a two D adaptive clearing.
08:35
Note that when we're using two D adaptive clearing,
08:38
there is a rest machining option.
08:40
However, with two D tool pass,
08:41
rest machining is really taking a look at a previously
08:45
sized tool and the material that would be left behind
08:48
when we get into 3D tool pass,
08:49
those are model aware and they make better use of
08:52
the material that was left behind from previous operations.
08:55
So for us,
08:56
we're gonna use a closed chain selection and not worry about rest machining
09:01
next.
09:01
In the height section,
09:02
we need to be careful here because we are gonna
09:05
be leaving stock and we can't have a bottom height offset
09:08
because the bottom of the tool is hitting stock,
09:11
we need to make sure that it's stopping at that area.
09:14
And in our passive section, we're leaving a half a millimeter of stock.
09:18
So for this tool path, we're gonna say, OK,
09:21
now that we've got our roughed material,
09:23
we need to go back and finish it and this can
09:25
generally be done with a couple of different tool paths.
09:28
For our part. It's gonna make the most amount of sense to use a two D contour.
09:32
Once again, we're gonna do this in two separate operations.
09:36
We're gonna select our tool.
09:37
We're gonna move to our geometry and select this bottom edge for our contour.
09:41
We're gonna move to our passes, make sure that we're not leaving any stock.
09:45
And we're gonna say, OK,
09:47
because of the size of our tool and the size of material that we need to remove,
09:51
we can do this in a single pass.
09:53
The reason we didn't do the bottom edge at the same time is
09:56
because the bottom edge needs to be cut a little bit lower.
09:59
So we're gonna do a two D contour one more time
10:02
this time selecting our bottom edge.
10:04
But inside of our passes section, we need to make sure that we are not leaving stock.
10:08
And in our height section, we need to make sure that we're using a negative offset.
10:13
When we did our two D adaptive, we had negative two millimeters.
10:16
However, that left half a millimeter of stock behind.
10:20
If we do this, it's going to engage too much stock at the bottom of our cut.
10:24
So we're gonna use minus 1.5 millimeters and say, OK,
10:28
this should get us down to the exact same height as our two D adaptive clearing.
10:33
Now that all of the outside of our part has been machined.
10:36
The last thing that we need to do is take care of the holes,
10:38
the holes are taken care of with drilling operations.
10:42
We're gonna start the drilling operations by using a spot drill.
10:45
This is gonna be tool number two in our tool library.
10:48
And we're gonna select aluminum drilling.
10:51
Then for our geometry, we're gonna select the insides of each of these holes.
10:56
By default. Fusion wants to drill all the way to the bottom of the hole.
10:59
This is a problem because we're using a spot drill and we
11:02
only need to start the hole so that it centers our drill.
11:05
So from our height section,
11:07
the very bottom, we're gonna change the from
11:09
to be the top of our hole.
11:12
And we're going to use the drill tip through bottom and say, OK,
11:15
this is gonna leave a small indent at the center of
11:18
each hole that allows the larger drill bit to be centered.
11:22
Next.
11:22
We're gonna do another drilling operation once again,
11:25
selecting each of these center holes.
11:26
However, this time we're gonna use the final size drill bit.
11:29
It's gonna be tool number three, a six millimeter drill.
11:32
And we'll select aluminum drilling for our preset.
11:35
We're going to go to our geometry selection, select each hole
11:39
and in our height section from our front view,
11:42
we want to make sure that we're drilling through the bottom.
11:45
And in this case, we've got two values,
11:47
we've got an offset value and a breakthrough depth,
11:50
the offset value is going to be based on our Z coordinate orientation.
11:54
This means that we need a negative value to go
11:56
further down and a positive value to go further up.
11:59
However, with the breakthrough depth,
12:01
if we use a positive value of two millimeters,
12:03
this is going to extend beyond the bottom of our part.
12:06
There is one more thing that we need to change and that's gonna be the drilling cycle.
12:11
This is gonna be a canned cycle that gets called inside of our coat.
12:14
Typically, when we're doing a spot drill,
12:17
the drill bit can come down spot the hole relatively quick and retract away.
12:21
However, when we're actually drilling in the material,
12:24
we want to use something like a chip breaking cycle.
12:27
This allows the drill bit to go in a small amount and
12:29
either pause or retract to allow the hole to clear the chips
12:33
and allow coolant to get into that hole.
12:35
This is especially important when we're drilling deep holes to ensure
12:38
that the quality and the diameter of the hole are consistent.
12:42
We're gonna say, OK, and we'll go back to our home view
12:46
at this point, everything looks ok.
12:48
However, the drill bit size is too small for the size of our hole.
12:52
If we use our inspect measure tool and we measure this hole,
12:55
we can see that it's currently at a diameter of eight millimeters.
12:59
We've already created our tool path with a six millimeter drill.
13:03
And if we expand this, you can see that tool number three is a six millimeter drill.
13:07
If we right click, we are able to edit the tool.
13:10
This means that we can go in and modify its parameters.
13:13
You should only do this if you have direct control
13:16
over which tools you have available on your machine.
13:18
In
13:19
this case, I'm gonna just simply change the diameter to eight millimeters
13:22
except
13:23
and now it tells me that this tool path is out of date
13:26
to fix this. All we need to do is go to actions and select generate.
13:31
It's gonna redo the tool path with the updated tool diameter,
13:34
our eight millimeter drill.
13:36
And now we can see the preview on the screen shows
13:38
that the holes are being drilled to the correct size.
13:41
Now, at this point, we've created our facing tool path,
13:44
our two D adaptive tool path to rough the stock
13:47
and our two D contours to finish the outside shape.
13:50
Then we went back with a spot drill to start
13:52
the holes and a drill bit to finish the holes.
13:55
So at this point,
13:56
let's go ahead and make sure that we save everything
13:58
we've done before we move on to the next step.
00:02
Create 2.5 access tool paths.
00:05
After completing this video, you'll be able to
00:08
create a drilling operation, create a 2.5 axis roughing tool path
00:11
and create 2.5 axis finishing tool baths.
00:16
To get started in fusion, we want to begin with the supply data set. CM two X tool
00:21
pass mm dot F 3D.
00:23
When we open this design up,
00:24
it should automatically be in the manufacture workspace.
00:27
But if not ensure that you do navigate there
00:29
and double check the units are set to metric.
00:32
This design already contains a setup,
00:34
the setup has the stock set and the coordinate system in the correct location.
00:38
The design also contains tools inside of its document.
00:41
You can take a look at the very top in the document for C AM two X tool paths.
00:45
There are tools and if we clear our filters,
00:49
we can see that tools will be available for
00:51
our milling operations as well as our drilling operations.
00:55
So now that we know that we have tools and our set up,
00:58
let's go ahead and get started creating our tool paths.
01:01
There are a couple of main objectives when we're machining apart,
01:04
first,
01:05
we want to remove as much material as possible as
01:08
quickly as possible in what are called roughing operations.
01:11
And then we wanna create finishing operations that will get down to the
01:15
final shape and size of our part and leave a good surface finish.
01:18
Now, there are some general approaches to this for nearly all parts.
01:22
So we're gonna take a look at that with this part here
01:25
to get started. The first operation we want to do is create a facing tool path.
01:29
When we take a look at this thing from the front view,
01:31
we can see that there's stock above the top of our part
01:34
and there's plenty of stock below the bottom of our part.
01:37
For this example, we're not going to be discussing holding it in a vice or a fixture.
01:42
We're just going to assume that we've got plenty of space below the bottom of our part
01:46
and we're holding it inside of some sort of work holding
01:49
that we need to make sure that we don't go all the way to the bottom of our stock.
01:53
We'll talk more about vices and fixtures in some of the three Xs tool paths.
01:58
So from here, we want to face the top of our part
02:01
back in a home view, we're going to go to our two D drop down and select two D face
02:06
from here. We need to select a tool.
02:09
There are only certain types of tools
02:10
that will be applicable for facing operations.
02:13
Our flat end mill as well as a larger face mill would be a good choice
02:17
because we're working on a limited set of tools.
02:19
We're going to be using our 12 millimeter flat end mill or tool. Number one,
02:24
we're gonna be using aluminum finishing for our cutting data.
02:27
This is because a facing tool path does remove raw
02:30
or rough stock from the outside of our part.
02:32
But the surface that it cuts down to will be the final top surface of our part,
02:36
we'll select the tool and that cutting preset.
02:39
Noting that in the feeds and speeds section, those values are now populated
02:43
from here. We're gonna move on to our geometry section
02:46
and with a facing tool path, it automatically gets the outside profile of our stock.
02:51
So we see an orange border on the screen and this tells us that no selection is needed.
02:56
Next in our height section,
02:58
we've got various planes that are gonna dictate what happens with the tool.
03:02
And when
03:03
we have a clearance plane at the very top, followed by a retract plane,
03:07
our feet height plane, the top height and the bottom height.
03:11
By default, with a facing tool path,
03:13
the top height will be the top of our stock
03:15
and the bottom height will be the top of our model
03:18
because of this, we don't need to make any changes or selections.
03:22
But as you begin machining more and more.
03:24
You'll find that reducing the height between things like our clearance plane,
03:28
retract plane and the feed height can drastically speed up the programs.
03:33
What I mean by this is there are different speeds at which the tool is gonna travel,
03:37
the rapid movements and the feed movements
03:39
changing where those happen can really speed up the machining process.
03:43
Reducing the amount of time you're spending, not cutting material.
03:47
Next, we're gonna move over to our passes section
03:50
in the passes section.
03:51
We've got a couple of options, but we're not going to change too much here.
03:54
First note that we've got our pass direction reference.
03:58
This is gonna allow us to change which direction the tool is going by default,
04:02
it'll be going along the X and Y directions.
04:05
Also as we go down, you can see that we've got a pass extension.
04:09
This is gonna be half of our tool or the radius value of our tool.
04:13
This means that the tool is going to extend past
04:15
the end of our stock before it turns around.
04:18
There's also a step over value and in this case, 1.7 millimeters is relatively low.
04:23
I'm gonna set this just shy of the diameter of our tool at 11 millimeters.
04:29
Next, we have a direction reference by default, it's gonna go both ways.
04:33
But if you have a specific machining direction, for example,
04:36
climb or conventional, you can change those.
04:38
Here.
04:39
There is a new option called order for shorter links that can reduce
04:43
the amount of time it takes to machine or face our part.
04:46
However, order for shorter links only works.
04:48
If you change your direction to a specific climb or conventional direction,
04:52
it won't work with the both option.
04:55
There's also a from other side and use chip
04:57
thinning which we're going to omit for right now.
05:00
And in the linking section,
05:01
this is gonna dictate how the tool moves into and out of our cuts.
05:05
And we're gonna leave these as default for now and say, OK,
05:08
once done, we'll get a preview on the screen,
05:10
showing us a green preview of the stock as well as
05:14
the lines that the tool is going to be traveling.
05:16
If we go back to our front view,
05:17
we can now see that the stock is cut down to the top of our part.
05:21
This is done showing us in process stock and
05:24
the visibility can be changed by going down to this
05:26
bottom section in fusion and turning on or off the
05:29
in process stock or by going to our tool,
05:32
visibility
05:32
going on and off for the tool.
05:35
And we can also turn on and off our tool paths.
05:39
This can help especially once we get into more complex
05:41
tool paths that have much more movements on the screen.
05:44
But for right now, we're gonna leave them as is.
05:46
So anytime we click on our facing tool path, we'll get a preview
05:50
now that we face the top of our part,
05:52
we're going to move on to doing some roughing operations
05:55
in the two D tools.
05:56
We've got a two D adaptive clearing,
05:58
which is a wonderful option for nearly all types of parts.
06:02
There are other options such as two D pocket for clearing.
06:05
But the two D adaptive is going to allow us to cut
06:07
a little bit deeper and keep a consistent load on our tool.
06:10
We're going to select two D adaptive clearing.
06:13
We're gonna be using the same tool moving on to our geometry selection
06:17
and we're going to select the bottom outside edge of our part.
06:20
There'll be a blue preview on the screen and this is gonna
06:23
let us know which side of the part is gonna be cut.
06:26
You also note that this goes out to the size of our stock,
06:29
so no other selections are needed.
06:31
Next, we're gonna go to our height section at
06:34
this point.
06:35
All of the heights are going to be ok because
06:37
the bottom height is based on our selected contour.
06:39
However, a two D adaptive tool path is a roughing tool path,
06:44
which means it's intended to leave stock behind.
06:47
And that's gonna not allow us to cut all the way down to the bottom of our part.
06:50
So if we view this from a front view again,
06:52
and we go down to our bottom height and the selected contours
06:55
and we add, say two millimeters
06:58
that's going to allow the tool to go two
06:59
millimeters relative to the bottom of our part.
07:02
However, the positive value is in the positive Z direction.
07:06
Because of the coordinate system, we need to use a negative value.
07:09
If we make this change, all we need to do is edit our tool path,
07:13
go to our height section
07:14
and change the offset value to minus two millimeters and say, OK.
07:19
Now the preview on the screen shows the tool path
07:21
cutting two millimeters below the bottom of our part.
07:24
Let's go ahead and take one quick look at the rest of the settings.
07:27
Before we move on to the next tool path.
07:30
In the passive section,
07:31
we have some values in here such as optimal load that are going to determine
07:35
how much engagement we have between our tool and the material that it's cutting.
07:39
We have a default stock to leave.
07:41
In this case,
07:42
it's half a millimeter in the radial direction and the axial direction.
07:46
This means on the side of the tool and on the bottom of the tool.
07:49
Next, we also have a multiple depths option.
07:52
In this case, our tool can make this cut with a single depth.
07:55
But if we had to cut extremely deep into a part, we may need to toggle that on.
08:00
The next option here is multi
08:02
axis which we're not taking a look at. And the last one is linking
08:05
by default, it'll do a helo
08:07
entry and we're gonna leave all of these values as default and say, OK,
08:12
back in a home view,
08:13
we can now see that we've cleared the material around the outside
08:15
of our part all the way to two millimeters below the part
08:19
minus that extra half a millimeter that it's leaving for a stock to leave.
08:23
Now, we want to remove the material from this phase.
08:26
We can do this in a single operation,
08:28
but it's good practice to go back and do this a couple of different times.
08:31
So we're going to use the same process using a two D adaptive clearing.
08:35
Note that when we're using two D adaptive clearing,
08:38
there is a rest machining option.
08:40
However, with two D tool pass,
08:41
rest machining is really taking a look at a previously
08:45
sized tool and the material that would be left behind
08:48
when we get into 3D tool pass,
08:49
those are model aware and they make better use of
08:52
the material that was left behind from previous operations.
08:55
So for us,
08:56
we're gonna use a closed chain selection and not worry about rest machining
09:01
next.
09:01
In the height section,
09:02
we need to be careful here because we are gonna
09:05
be leaving stock and we can't have a bottom height offset
09:08
because the bottom of the tool is hitting stock,
09:11
we need to make sure that it's stopping at that area.
09:14
And in our passive section, we're leaving a half a millimeter of stock.
09:18
So for this tool path, we're gonna say, OK,
09:21
now that we've got our roughed material,
09:23
we need to go back and finish it and this can
09:25
generally be done with a couple of different tool paths.
09:28
For our part. It's gonna make the most amount of sense to use a two D contour.
09:32
Once again, we're gonna do this in two separate operations.
09:36
We're gonna select our tool.
09:37
We're gonna move to our geometry and select this bottom edge for our contour.
09:41
We're gonna move to our passes, make sure that we're not leaving any stock.
09:45
And we're gonna say, OK,
09:47
because of the size of our tool and the size of material that we need to remove,
09:51
we can do this in a single pass.
09:53
The reason we didn't do the bottom edge at the same time is
09:56
because the bottom edge needs to be cut a little bit lower.
09:59
So we're gonna do a two D contour one more time
10:02
this time selecting our bottom edge.
10:04
But inside of our passes section, we need to make sure that we are not leaving stock.
10:08
And in our height section, we need to make sure that we're using a negative offset.
10:13
When we did our two D adaptive, we had negative two millimeters.
10:16
However, that left half a millimeter of stock behind.
10:20
If we do this, it's going to engage too much stock at the bottom of our cut.
10:24
So we're gonna use minus 1.5 millimeters and say, OK,
10:28
this should get us down to the exact same height as our two D adaptive clearing.
10:33
Now that all of the outside of our part has been machined.
10:36
The last thing that we need to do is take care of the holes,
10:38
the holes are taken care of with drilling operations.
10:42
We're gonna start the drilling operations by using a spot drill.
10:45
This is gonna be tool number two in our tool library.
10:48
And we're gonna select aluminum drilling.
10:51
Then for our geometry, we're gonna select the insides of each of these holes.
10:56
By default. Fusion wants to drill all the way to the bottom of the hole.
10:59
This is a problem because we're using a spot drill and we
11:02
only need to start the hole so that it centers our drill.
11:05
So from our height section,
11:07
the very bottom, we're gonna change the from
11:09
to be the top of our hole.
11:12
And we're going to use the drill tip through bottom and say, OK,
11:15
this is gonna leave a small indent at the center of
11:18
each hole that allows the larger drill bit to be centered.
11:22
Next.
11:22
We're gonna do another drilling operation once again,
11:25
selecting each of these center holes.
11:26
However, this time we're gonna use the final size drill bit.
11:29
It's gonna be tool number three, a six millimeter drill.
11:32
And we'll select aluminum drilling for our preset.
11:35
We're going to go to our geometry selection, select each hole
11:39
and in our height section from our front view,
11:42
we want to make sure that we're drilling through the bottom.
11:45
And in this case, we've got two values,
11:47
we've got an offset value and a breakthrough depth,
11:50
the offset value is going to be based on our Z coordinate orientation.
11:54
This means that we need a negative value to go
11:56
further down and a positive value to go further up.
11:59
However, with the breakthrough depth,
12:01
if we use a positive value of two millimeters,
12:03
this is going to extend beyond the bottom of our part.
12:06
There is one more thing that we need to change and that's gonna be the drilling cycle.
12:11
This is gonna be a canned cycle that gets called inside of our coat.
12:14
Typically, when we're doing a spot drill,
12:17
the drill bit can come down spot the hole relatively quick and retract away.
12:21
However, when we're actually drilling in the material,
12:24
we want to use something like a chip breaking cycle.
12:27
This allows the drill bit to go in a small amount and
12:29
either pause or retract to allow the hole to clear the chips
12:33
and allow coolant to get into that hole.
12:35
This is especially important when we're drilling deep holes to ensure
12:38
that the quality and the diameter of the hole are consistent.
12:42
We're gonna say, OK, and we'll go back to our home view
12:46
at this point, everything looks ok.
12:48
However, the drill bit size is too small for the size of our hole.
12:52
If we use our inspect measure tool and we measure this hole,
12:55
we can see that it's currently at a diameter of eight millimeters.
12:59
We've already created our tool path with a six millimeter drill.
13:03
And if we expand this, you can see that tool number three is a six millimeter drill.
13:07
If we right click, we are able to edit the tool.
13:10
This means that we can go in and modify its parameters.
13:13
You should only do this if you have direct control
13:16
over which tools you have available on your machine.
13:18
In
13:19
this case, I'm gonna just simply change the diameter to eight millimeters
13:22
except
13:23
and now it tells me that this tool path is out of date
13:26
to fix this. All we need to do is go to actions and select generate.
13:31
It's gonna redo the tool path with the updated tool diameter,
13:34
our eight millimeter drill.
13:36
And now we can see the preview on the screen shows
13:38
that the holes are being drilled to the correct size.
13:41
Now, at this point, we've created our facing tool path,
13:44
our two D adaptive tool path to rough the stock
13:47
and our two D contours to finish the outside shape.
13:50
Then we went back with a spot drill to start
13:52
the holes and a drill bit to finish the holes.
13:55
So at this point,
13:56
let's go ahead and make sure that we save everything
13:58
we've done before we move on to the next step.
After completing this video, you’ll be able to:
Step-by-step guide