& Construction

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

Professional CAD/CAM tools built on Inventor and AutoCAD
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
Machine Operation one of a part
00:05
in this video.
00:06
We're going to use the face tool path to D contour tool path,
00:09
drill and tap holes and we're going to create a champ for two deeper apart
00:15
To get started in Fusion 360, let's carry on with our engine case are
00:19
ready to program.
00:21
We've already got op one set up and we're
00:23
ready to start machining to begin machining this part.
00:27
We want to start by creating a facing operation on the top to
00:30
take us down to the very top of our part to do this.
00:33
We're going to go to
00:34
and select
00:35
the face.
00:36
We need to begin by selecting the tool that we want to use. So we'll go to intro to C. N.
00:41
C.
00:41
Cloud library and in this case what we're gonna do is
00:44
we're going to use a half inch flat end mill.
00:47
I want to make sure that I select the correct or the appropriate cutting data and in
00:51
this case I'm going to start with aluminum roughing and say okay to select that tool,
00:56
I do want to make some adjustments here.
00:58
I want to make sure that the cutting feed rate is a little bit slower so I'm going to
01:02
reset this to 100 and I'm going to leave my lead in and lead out feed rates at 126.
01:08
It's important to make sure that you're using cutting
01:11
feed rates that are appropriate for your materials,
01:14
the tools that you're using and the way in which you're holding the part,
01:17
you have to be careful not to engage too much
01:20
material if your part is not held extremely rigid.
01:23
Now that we have our tools and our feed rates set,
01:25
we're going to move over to geometry with the
01:28
facing tool path that automatically brings in stock contours.
01:31
So because we set up our stock based off of our solid body,
01:35
the orange profile here represents a slightly larger profile than the actual part.
01:40
So we'll be able to face down the entire top
01:43
for heights,
01:44
it's going to automatically go down to the model
01:46
top and it's going to start at stock top.
01:49
Now we could spend a lot of time adjusting the heights of these planes.
01:53
I'm not going to spend a lot of time doing
01:54
that because these are minor adjustments that we can make,
01:57
they will ultimately make a lot of difference in the final
02:00
program because things like the feed height are going to be,
02:04
where the tool transitions from a rapid movement to a feed movement.
02:07
You need to figure out what's an appropriate clearance height,
02:10
feed height and retract height for your specific machine.
02:14
Often times if a machine moves extremely fast on rapid movements,
02:17
you might want a little bit more space once you
02:20
start your feet height before you begin engaging material.
02:23
So again, I'm going to leave these as default for now on the past this section.
02:28
One thing that we do need to consider is how much material we are engaging.
02:32
So right now the past direction is automatically going to be aligned with the X axis.
02:37
So I'm going to leave that as is the past
02:39
extension goes a little bit past half of the tool,
02:42
which means that it's going to exit the stock completely before it
02:45
turns around and I'm going to leave zero for the stock offset.
02:49
However, for the step over value, I do want to increase this a little bit,
02:53
I can go a little bit further,
02:55
making sure that I take a deeper cut with my half inch end mill.
02:58
So this is going to step over 0.35 or just a little bit more than half of the tool.
03:04
Also notice that we can use multiple depths if we happen to
03:07
take a lot of material off the top of a part.
03:09
We can start by clearing it out using something like an adaptive clearing or we can
03:14
use multiple depths and just make sure that we have a final step for our finish.
03:18
I'm going to allow it to go down a quarter inch at a time and for the finishing step,
03:24
I'm going to allow it to go down 0.5.
03:26
Just take a small cut at the very end.
03:29
I'm going to say, okay, allow it to remove the material from the top
03:33
now that we faced the top of the part. I do want to move on to cutting the outside.
03:38
So the outside is going to be critical and I'm going to use a two D. Contour.
03:42
The two D contour will allow me to use the same half inch flat end mill that
03:46
has an inch and a half long cutting flute and machine the entire outside of our part.
03:51
This is a critical step in the process because we know that we've machined the
03:55
top of the face and we're going to machine the entire outside of the part,
03:59
leaving only the bottom face still needing to be machined on the outside.
04:03
So from here we need to take a look at the feeds and speeds.
04:07
You can see that they have come over from
04:09
our last operation are cutting feed rate is 100.
04:12
Using that custom preset.
04:14
We can also tap into some of the other
04:16
presets such as aluminum slotting roughing or finishing.
04:19
We're going to move over to geometry and we do need to select the lower contour.
04:24
The red arrow on the outside of our
04:26
selected contour means that we're machining the outside.
04:30
The direction of cut is going to be taken care of in the past this section
04:34
we can turn on stock contours and this will help us
04:37
when we're thinking about creating our two D contour cutting,
04:40
it's going to allow us to only make the cuts where material is left behind.
04:46
So for this example,
04:47
turning that on should help us reduce the amount of cutting time that's wasted.
04:53
We don't need to worry about rest machining since the two D.
04:55
Contour is not going to really worry about the top of the stock.
04:58
So we're gonna move on to our heights.
05:01
We're not going to adjust any of the other heights such as the clearance
05:04
or retract but we do need to add some additional offset to the bottom.
05:09
When we're talking about offsetting from a selected contour,
05:12
we need to use a negative value here.
05:14
So negative .05 will allow the tool to go down .05 further than our selected contour.
05:21
This value is negative because Z is negative in that direction.
05:26
In the past this section there are a couple of things that we want to
05:29
think about here first there are a lot of default values for the passes.
05:33
Again, the tolerance value is here.
05:36
This can make a big difference in the amount
05:38
of data that's getting pushed through the controller.
05:40
If we're dealing with a lot of curves are geometry is straight lines and
05:44
arcs so it's really not going to make too much of a final difference.
05:47
We do want to take a look at things like multiple finishing passes,
05:51
repeating the finishing pass and things like finishing pass overlap.
05:56
So I'm going to add a finishing pass overlap of .05.
06:00
And what this means is that the starting and ending point are going to be different.
06:04
Sometimes if you have a lot of depth cuts
06:07
when you're doing roughing passes or multiple depths.
06:09
Having a finishing overlap can reduce any
06:13
deformation that happen on the outside surface.
06:15
I also want to talk about roughing passes as well as multiple depths
06:21
Even though I know there's not much material here.
06:23
I do want to take a small roughing pass.
06:26
I'm going to set this at .03 and that small roughing step over value.
06:31
Notice that it's coming in red. This is because this is a very low value.
06:36
We need to set it a little bit larger in order to have a roughing step over
06:41
Then for multiple depths,
06:43
I want to make sure that I don't go too far down
06:45
because I want to preserve the outside surface quality finish and tolerance.
06:49
So I only want to go down about .475, almost half an inch,
06:55
which is the diameter of my tool.
06:57
I do want to include one finished step down.
07:00
That finished step down at .008 is going to be just fine
07:04
but notice that we can do adjustments to any of these values.
07:09
Also, I'm going to include
07:11
finish only at final depth,
07:13
which means that it will do all of the
07:15
multiple step downs for roughing but it's only going
07:17
to do that final pass at the final depth where we're taking off a very small amount.
07:23
So from here, there's some other things that we do need to think about.
07:27
We need to think about linking parameters right now
07:30
are safe distance is larger than our feed distance.
07:33
So I'm going to reset this 2.2 which matches the
07:36
feed height from our top height inside of our heights
07:41
over here. We also want to think about how we're leading into and out of the cuts.
07:46
So right now we have ramp which will allow it to ramp down as it's making the cut.
07:52
But in this case I want to just exclude a ramp and I'm going to allow it
07:56
to plunge down and I'm going to say okay and just see what happens for my contour.
08:02
So because we have stock contours turned on notice that it is only cutting on
08:07
the outside sections and then it's doing the final cut at the very final depth.
08:12
So these are things that we need to think about because if we go back into our two D.
08:16
Contour and I go back into geometry and turn off stock contours
08:20
it's going to create those cuts all the way down the part.
08:23
Which means that we're likely wasting some time.
08:26
So using options like stock contour and geometry is a good way
08:30
for us to reduce the number of tool paths that get created.
08:33
That might just simply be cutting air
08:36
now that we've cut the top and the outside,
08:38
we need to think about drilling and tapping these
08:41
holes so we're gonna go to our drilling operation,
08:43
we're going to select our appropriate tool.
08:45
In this case, tool number two. Making sure that we're going into intro to C. And C.
08:50
We're going to select the tool.
08:52
We're going to select our geometry by selecting these two holes
08:57
and then for our heights on the bottom, we want to reset this to champ for width.
09:02
This means it's going to take the chance for tool all the way
09:04
down until the champ for width intersects with the diameter of the hole.
09:09
Next I'm going to right click and I want to duplicate this operation.
09:12
When I duplicate it, I've made an exact copy.
09:16
I'm going to edit this and I'm going to select a different tool.
09:19
Again,
09:20
an intro to see and see what we want to do
09:22
is select tool number six which is a number 21 drill.
09:25
That number 21 drill is to pre drill before we tap
09:30
inside of the geometry section. Everything is still selected.
09:33
However the bottom heights we want to set to the bottom of the hole.
09:37
We also want to include drill tip through bottom,
09:40
which will mean that the tapered section of the drill will go down to make
09:44
sure that the full depth of the hole is using the diameter of the drill.
09:48
Lastly we want to use a chip breaking partial retract.
09:52
This means that the drill will go down a small amount
09:54
and then retract a small amount to break the chips.
09:57
This is a great way to go ahead and drill
09:59
deep holes but it also helps when we're dealing with
10:02
small blind holes because they can fill up with chips
10:04
really easily and they can cause problems with whole quality
10:09
Before we do any tapping, let's go ahead and create two d.
10:13
Champ for operations to deeper those holes as well as the outside of our part.
10:17
So under the two D. Menu we're going to select two D champ for two D.
10:21
Champ for only works with an appropriate champ for tool. So an intro to C. N. C.
10:26
We're going to select tool number three using the default presets and will select
10:32
you can see that it populates our feeds and speeds.
10:34
Then we can move on to selecting our geometry.
10:37
We're going to take care of the two holes first.
10:39
We're going to move on to our passes section
10:42
where we're going to dictate the champ for with
10:44
the tip offset as well as the clearance because
10:47
there's no chance for on this model already.
10:50
We need to use some values to represent this.
10:52
So in this case, what we're going to do for our champ for width is set it at .02.
10:58
The champ for offset. We're going to set at 0.3 and the champ for clearance value.
11:04
We're going to reduce this down 2.1.
11:07
We do have to be careful because we have a relatively small hole,
11:11
we're trying to cut a champ for into
11:13
and last but not least.
11:14
We want to make sure that we do an external champ
11:16
for before we tap those holes simply because we already have that
11:20
tool loaded in the machine and we don't want to induce another
11:23
tool change and have to move back to that same tool.
11:26
So the geometry in this case is going to be the outside.
11:29
But remember that we haven't actually machined this pocket yet
11:32
so we're going to hold down the left mouse button
11:35
to open up the edge selection dialog. And we're going to select this edge. Again,
11:40
we want to use an open contour and move our way around.
11:45
Once we select everything we want we can hit Plus to accept
11:48
that another way that we can do this is by holding down the
11:52
key on the keyboard.
11:53
It will let you select a single edge and then
11:56
we can re select that edge to continue chaining it.
11:59
So I'm going to hit the trash can icon to get rid
12:02
of that because I only want to use that single edge selection
12:05
Next. Once again we need to dictate the champ for width.
12:09
The tip offset and the clearance values in this case the width is going to be .01
12:15
The tip offset value. We're going to use .05.
12:20
And for the clearance again we're going to reduce this down 2.1.
12:24
We're going to say okay allow it to de burr that edge
12:27
and then now we want to come back and create a tap cycle
12:31
when we're doing tapping. We want to select the tap from our intro to C and C.
12:35
Library and this is going to be a 10 32 tap tool number four.
12:41
The taps are going to run a little bit slower, generally around 500 rpm.
12:45
And these are automatically going to be synchronized with the mill.
12:49
So when we select the holes that we want to tap and we go to our cycle,
12:53
it's set to tapping,
12:54
which means that it's going to turn the correct direction and amount as it goes into
12:58
the hole and it's going to reverse the direction coming back out of the hole.
13:02
At this point we've now machined everything from that top orientation.
13:07
We faced the top, we've cut the outside with a two D.
13:10
Contour and we can see that it's gone just past the bottom of our part.
13:14
Which means when we flip it over it's going to be
13:16
easy for us to remove the rest of that material.
13:19
We've also created a spot drill, a peck drill cycle or a chip breaking cycle.
13:25
We've champ for the edge of that whole.
13:26
We've champ furred the entire outside of our part.
13:29
And we've also gone back and tap those holes.
13:33
Now we're set to move on to the next operation and orientation for this part.
13:37
But first let's go ahead and save the design and then move on
Video transcript
00:02
Machine Operation one of a part
00:05
in this video.
00:06
We're going to use the face tool path to D contour tool path,
00:09
drill and tap holes and we're going to create a champ for two deeper apart
00:15
To get started in Fusion 360, let's carry on with our engine case are
00:19
ready to program.
00:21
We've already got op one set up and we're
00:23
ready to start machining to begin machining this part.
00:27
We want to start by creating a facing operation on the top to
00:30
take us down to the very top of our part to do this.
00:33
We're going to go to
00:34
and select
00:35
the face.
00:36
We need to begin by selecting the tool that we want to use. So we'll go to intro to C. N.
00:41
C.
00:41
Cloud library and in this case what we're gonna do is
00:44
we're going to use a half inch flat end mill.
00:47
I want to make sure that I select the correct or the appropriate cutting data and in
00:51
this case I'm going to start with aluminum roughing and say okay to select that tool,
00:56
I do want to make some adjustments here.
00:58
I want to make sure that the cutting feed rate is a little bit slower so I'm going to
01:02
reset this to 100 and I'm going to leave my lead in and lead out feed rates at 126.
01:08
It's important to make sure that you're using cutting
01:11
feed rates that are appropriate for your materials,
01:14
the tools that you're using and the way in which you're holding the part,
01:17
you have to be careful not to engage too much
01:20
material if your part is not held extremely rigid.
01:23
Now that we have our tools and our feed rates set,
01:25
we're going to move over to geometry with the
01:28
facing tool path that automatically brings in stock contours.
01:31
So because we set up our stock based off of our solid body,
01:35
the orange profile here represents a slightly larger profile than the actual part.
01:40
So we'll be able to face down the entire top
01:43
for heights,
01:44
it's going to automatically go down to the model
01:46
top and it's going to start at stock top.
01:49
Now we could spend a lot of time adjusting the heights of these planes.
01:53
I'm not going to spend a lot of time doing
01:54
that because these are minor adjustments that we can make,
01:57
they will ultimately make a lot of difference in the final
02:00
program because things like the feed height are going to be,
02:04
where the tool transitions from a rapid movement to a feed movement.
02:07
You need to figure out what's an appropriate clearance height,
02:10
feed height and retract height for your specific machine.
02:14
Often times if a machine moves extremely fast on rapid movements,
02:17
you might want a little bit more space once you
02:20
start your feet height before you begin engaging material.
02:23
So again, I'm going to leave these as default for now on the past this section.
02:28
One thing that we do need to consider is how much material we are engaging.
02:32
So right now the past direction is automatically going to be aligned with the X axis.
02:37
So I'm going to leave that as is the past
02:39
extension goes a little bit past half of the tool,
02:42
which means that it's going to exit the stock completely before it
02:45
turns around and I'm going to leave zero for the stock offset.
02:49
However, for the step over value, I do want to increase this a little bit,
02:53
I can go a little bit further,
02:55
making sure that I take a deeper cut with my half inch end mill.
02:58
So this is going to step over 0.35 or just a little bit more than half of the tool.
03:04
Also notice that we can use multiple depths if we happen to
03:07
take a lot of material off the top of a part.
03:09
We can start by clearing it out using something like an adaptive clearing or we can
03:14
use multiple depths and just make sure that we have a final step for our finish.
03:18
I'm going to allow it to go down a quarter inch at a time and for the finishing step,
03:24
I'm going to allow it to go down 0.5.
03:26
Just take a small cut at the very end.
03:29
I'm going to say, okay, allow it to remove the material from the top
03:33
now that we faced the top of the part. I do want to move on to cutting the outside.
03:38
So the outside is going to be critical and I'm going to use a two D. Contour.
03:42
The two D contour will allow me to use the same half inch flat end mill that
03:46
has an inch and a half long cutting flute and machine the entire outside of our part.
03:51
This is a critical step in the process because we know that we've machined the
03:55
top of the face and we're going to machine the entire outside of the part,
03:59
leaving only the bottom face still needing to be machined on the outside.
04:03
So from here we need to take a look at the feeds and speeds.
04:07
You can see that they have come over from
04:09
our last operation are cutting feed rate is 100.
04:12
Using that custom preset.
04:14
We can also tap into some of the other
04:16
presets such as aluminum slotting roughing or finishing.
04:19
We're going to move over to geometry and we do need to select the lower contour.
04:24
The red arrow on the outside of our
04:26
selected contour means that we're machining the outside.
04:30
The direction of cut is going to be taken care of in the past this section
04:34
we can turn on stock contours and this will help us
04:37
when we're thinking about creating our two D contour cutting,
04:40
it's going to allow us to only make the cuts where material is left behind.
04:46
So for this example,
04:47
turning that on should help us reduce the amount of cutting time that's wasted.
04:53
We don't need to worry about rest machining since the two D.
04:55
Contour is not going to really worry about the top of the stock.
04:58
So we're gonna move on to our heights.
05:01
We're not going to adjust any of the other heights such as the clearance
05:04
or retract but we do need to add some additional offset to the bottom.
05:09
When we're talking about offsetting from a selected contour,
05:12
we need to use a negative value here.
05:14
So negative .05 will allow the tool to go down .05 further than our selected contour.
05:21
This value is negative because Z is negative in that direction.
05:26
In the past this section there are a couple of things that we want to
05:29
think about here first there are a lot of default values for the passes.
05:33
Again, the tolerance value is here.
05:36
This can make a big difference in the amount
05:38
of data that's getting pushed through the controller.
05:40
If we're dealing with a lot of curves are geometry is straight lines and
05:44
arcs so it's really not going to make too much of a final difference.
05:47
We do want to take a look at things like multiple finishing passes,
05:51
repeating the finishing pass and things like finishing pass overlap.
05:56
So I'm going to add a finishing pass overlap of .05.
06:00
And what this means is that the starting and ending point are going to be different.
06:04
Sometimes if you have a lot of depth cuts
06:07
when you're doing roughing passes or multiple depths.
06:09
Having a finishing overlap can reduce any
06:13
deformation that happen on the outside surface.
06:15
I also want to talk about roughing passes as well as multiple depths
06:21
Even though I know there's not much material here.
06:23
I do want to take a small roughing pass.
06:26
I'm going to set this at .03 and that small roughing step over value.
06:31
Notice that it's coming in red. This is because this is a very low value.
06:36
We need to set it a little bit larger in order to have a roughing step over
06:41
Then for multiple depths,
06:43
I want to make sure that I don't go too far down
06:45
because I want to preserve the outside surface quality finish and tolerance.
06:49
So I only want to go down about .475, almost half an inch,
06:55
which is the diameter of my tool.
06:57
I do want to include one finished step down.
07:00
That finished step down at .008 is going to be just fine
07:04
but notice that we can do adjustments to any of these values.
07:09
Also, I'm going to include
07:11
finish only at final depth,
07:13
which means that it will do all of the
07:15
multiple step downs for roughing but it's only going
07:17
to do that final pass at the final depth where we're taking off a very small amount.
07:23
So from here, there's some other things that we do need to think about.
07:27
We need to think about linking parameters right now
07:30
are safe distance is larger than our feed distance.
07:33
So I'm going to reset this 2.2 which matches the
07:36
feed height from our top height inside of our heights
07:41
over here. We also want to think about how we're leading into and out of the cuts.
07:46
So right now we have ramp which will allow it to ramp down as it's making the cut.
07:52
But in this case I want to just exclude a ramp and I'm going to allow it
07:56
to plunge down and I'm going to say okay and just see what happens for my contour.
08:02
So because we have stock contours turned on notice that it is only cutting on
08:07
the outside sections and then it's doing the final cut at the very final depth.
08:12
So these are things that we need to think about because if we go back into our two D.
08:16
Contour and I go back into geometry and turn off stock contours
08:20
it's going to create those cuts all the way down the part.
08:23
Which means that we're likely wasting some time.
08:26
So using options like stock contour and geometry is a good way
08:30
for us to reduce the number of tool paths that get created.
08:33
That might just simply be cutting air
08:36
now that we've cut the top and the outside,
08:38
we need to think about drilling and tapping these
08:41
holes so we're gonna go to our drilling operation,
08:43
we're going to select our appropriate tool.
08:45
In this case, tool number two. Making sure that we're going into intro to C. And C.
08:50
We're going to select the tool.
08:52
We're going to select our geometry by selecting these two holes
08:57
and then for our heights on the bottom, we want to reset this to champ for width.
09:02
This means it's going to take the chance for tool all the way
09:04
down until the champ for width intersects with the diameter of the hole.
09:09
Next I'm going to right click and I want to duplicate this operation.
09:12
When I duplicate it, I've made an exact copy.
09:16
I'm going to edit this and I'm going to select a different tool.
09:19
Again,
09:20
an intro to see and see what we want to do
09:22
is select tool number six which is a number 21 drill.
09:25
That number 21 drill is to pre drill before we tap
09:30
inside of the geometry section. Everything is still selected.
09:33
However the bottom heights we want to set to the bottom of the hole.
09:37
We also want to include drill tip through bottom,
09:40
which will mean that the tapered section of the drill will go down to make
09:44
sure that the full depth of the hole is using the diameter of the drill.
09:48
Lastly we want to use a chip breaking partial retract.
09:52
This means that the drill will go down a small amount
09:54
and then retract a small amount to break the chips.
09:57
This is a great way to go ahead and drill
09:59
deep holes but it also helps when we're dealing with
10:02
small blind holes because they can fill up with chips
10:04
really easily and they can cause problems with whole quality
10:09
Before we do any tapping, let's go ahead and create two d.
10:13
Champ for operations to deeper those holes as well as the outside of our part.
10:17
So under the two D. Menu we're going to select two D champ for two D.
10:21
Champ for only works with an appropriate champ for tool. So an intro to C. N. C.
10:26
We're going to select tool number three using the default presets and will select
10:32
you can see that it populates our feeds and speeds.
10:34
Then we can move on to selecting our geometry.
10:37
We're going to take care of the two holes first.
10:39
We're going to move on to our passes section
10:42
where we're going to dictate the champ for with
10:44
the tip offset as well as the clearance because
10:47
there's no chance for on this model already.
10:50
We need to use some values to represent this.
10:52
So in this case, what we're going to do for our champ for width is set it at .02.
10:58
The champ for offset. We're going to set at 0.3 and the champ for clearance value.
11:04
We're going to reduce this down 2.1.
11:07
We do have to be careful because we have a relatively small hole,
11:11
we're trying to cut a champ for into
11:13
and last but not least.
11:14
We want to make sure that we do an external champ
11:16
for before we tap those holes simply because we already have that
11:20
tool loaded in the machine and we don't want to induce another
11:23
tool change and have to move back to that same tool.
11:26
So the geometry in this case is going to be the outside.
11:29
But remember that we haven't actually machined this pocket yet
11:32
so we're going to hold down the left mouse button
11:35
to open up the edge selection dialog. And we're going to select this edge. Again,
11:40
we want to use an open contour and move our way around.
11:45
Once we select everything we want we can hit Plus to accept
11:48
that another way that we can do this is by holding down the
11:52
key on the keyboard.
11:53
It will let you select a single edge and then
11:56
we can re select that edge to continue chaining it.
11:59
So I'm going to hit the trash can icon to get rid
12:02
of that because I only want to use that single edge selection
12:05
Next. Once again we need to dictate the champ for width.
12:09
The tip offset and the clearance values in this case the width is going to be .01
12:15
The tip offset value. We're going to use .05.
12:20
And for the clearance again we're going to reduce this down 2.1.
12:24
We're going to say okay allow it to de burr that edge
12:27
and then now we want to come back and create a tap cycle
12:31
when we're doing tapping. We want to select the tap from our intro to C and C.
12:35
Library and this is going to be a 10 32 tap tool number four.
12:41
The taps are going to run a little bit slower, generally around 500 rpm.
12:45
And these are automatically going to be synchronized with the mill.
12:49
So when we select the holes that we want to tap and we go to our cycle,
12:53
it's set to tapping,
12:54
which means that it's going to turn the correct direction and amount as it goes into
12:58
the hole and it's going to reverse the direction coming back out of the hole.
13:02
At this point we've now machined everything from that top orientation.
13:07
We faced the top, we've cut the outside with a two D.
13:10
Contour and we can see that it's gone just past the bottom of our part.
13:14
Which means when we flip it over it's going to be
13:16
easy for us to remove the rest of that material.
13:19
We've also created a spot drill, a peck drill cycle or a chip breaking cycle.
13:25
We've champ for the edge of that whole.
13:26
We've champ furred the entire outside of our part.
13:29
And we've also gone back and tap those holes.
13:33
Now we're set to move on to the next operation and orientation for this part.
13:37
But first let's go ahead and save the design and then move on
Step-by-step guide
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in to start learning
Sign in for unlimited free access to all learning content.Save your progress
Take assessments
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement.May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.