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In this practice, you’ll draw and extrude geometry that is intended for machining.
Learning objectives:
Exercise
Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
00:01
This is the practice exercise video solution
00:04
for this practice.
00:05
We're going to start with a new untitled
00:07
document and practice some sketching and modeling.
00:10
We want to begin by checking our document units and in this case,
00:13
we're gonna set our document units to inch
00:16
from here. We want to start a new sketch.
00:20
We can pick any sketch plan we want. But in this case, I'm gonna select the top plane.
00:25
I wanna begin by using a rectangle.
00:27
I'm gonna set this as a center rectangle so I can use the origin
00:32
whenever modeling,
00:33
it's important that we use the origin and the
00:34
standard planes to maintain symmetry of a part.
00:38
This will simplify the number of dimensions and constraints that are needed and
00:41
also make sure that the design is easy to update later on.
00:45
We're gonna set this at a width of six inches,
00:47
hit tab and move over and set this at a height of two inches and hit enter.
00:53
Now that we have the base of our design created,
00:55
I'm gonna finish the sketch and extrude this into 3D
00:59
using the extra tool. I'm gonna pull this up a distance of half inch.
01:04
We'll select. OK. And now we've begun creating our design.
01:08
I'm gonna make some modifications to this by using the fillet command.
01:12
And I wanna make sure that I get all four corners,
01:15
begin using the manipulator and set the corner radius at half inch
01:21
from here. I'm going to explore another tool, modify and shell.
01:25
We'll select the top phase and begin using
01:27
the onscreen manipulator to drag this inward.
01:30
I want to set this at a wall thickness of 0.25 inches and hit. Enter
01:35
the shell tool will maintain a quarter inch wall thickness
01:38
and a quarter inch bottom thickness based on that value.
01:42
Next, I'm gonna select this inside face right click and create a new sketch.
01:48
This will automatically project the selected face as a profile.
01:52
We can use this for things like offset or to measure from the edges.
01:56
What we want to do is create a new center point circle
02:01
with a diameter value of 0.75.
02:05
Now that we have this created,
02:07
I'm going to select the circle and I want to use the offset command
02:12
as we drag this out.
02:13
The offset command or tool will allow us
02:15
to create an offset of our selected geometry.
02:19
I'm gonna bring this out until it's offset a distance of one inch and hit. Enter,
02:23
notice that this creates a couple of different closed profile regions.
02:27
These outside profile regions are not going to be used
02:30
but we can leave them inside of the sketch.
02:33
If you go to trim the outside of the sketch,
02:36
likely you'll get issues with constraints and dimensions being broken.
02:40
So in some cases, it's easier for us to leave that information.
02:44
Next,
02:45
I'm going to use the two point rectangle and I'm going to select
02:48
the upper edge of this profile and the lower edge of this profile,
02:52
then we'll come back and add a dimension.
02:55
I want to make sure that the side of this is a distance of 0.5 inches in we'll hit enter
03:01
and then the overall width of this is gonna be a distance of 0.25.
03:06
Now that we have this object on the left hand side,
03:09
I also want to make a vertical construction line from the origin.
03:13
We'll hit escape to get off of our line tool.
03:15
And this vertical construction line needs to be changed to construction
03:19
in the sketch palette or by using X on the keyboard,
03:22
this line is going to be here so that we can use it for mirroring geometry.
03:26
Next, we're gonna select create mir
03:29
and in this instance, we don't need to grab all four edges of our rectangle.
03:33
We only need the left and the right.
03:35
We're gonna select the vertical construction line to mirror and select OK.
03:39
The main reason we only needed the left and the right lines
03:42
is because the profile is already brought in from our sketch creation.
03:46
So even though there's no short line between these two ends,
03:49
we still have a valid sketch profile.
03:52
Next, let's go ahead and finish the sketch.
03:55
Select extrude,
03:57
select these outside regions as well as this inside region and pull it upward.
04:02
We're not gonna go all the way to the top. We'll go a distance of 0.2 and select. OK.
04:07
This is now joined with the rest of the model.
04:10
If this model was created for injection molding,
04:13
we could leave these square corners.
04:14
However, they're going to be problematic if we decide to mill this part.
04:18
So we're going to go to modify select file
04:21
and note that with the file tool,
04:22
we can select these vertical edges through solid geometry.
04:26
We also need to make sure that we fill at these corners of this rectangle as well.
04:32
Some of this could be done at the sketch level.
04:35
But oftentimes it's easier for us to modify
04:37
these parameters later at the feature level,
04:40
we're going to increase this to a value that's slightly
04:42
larger than a tool that we want to use.
04:44
So this radius value of 0.15 should be large enough for us to use a quarter inch NM.
04:50
If we hit enter, we can always go back and use the inspect tool and measure the radius.
04:55
Here. We can see the radius of 0.15 that we entered, gives us a diameter value of 0.3.
05:01
This means a quarter inch tool can come in and finish these pockets
05:04
without fear of chattering in those
05:05
corners because the radius values are different
05:08
at this point. This is all we're going to do with this design.
05:11
But it's a good idea to continue to play around with sketching.
05:14
And oftentimes grab a model inside of your work area and try to replicate it in 3D.
05:20
Once you're done, feel free to save your design before moving on.
Video transcript
00:01
This is the practice exercise video solution
00:04
for this practice.
00:05
We're going to start with a new untitled
00:07
document and practice some sketching and modeling.
00:10
We want to begin by checking our document units and in this case,
00:13
we're gonna set our document units to inch
00:16
from here. We want to start a new sketch.
00:20
We can pick any sketch plan we want. But in this case, I'm gonna select the top plane.
00:25
I wanna begin by using a rectangle.
00:27
I'm gonna set this as a center rectangle so I can use the origin
00:32
whenever modeling,
00:33
it's important that we use the origin and the
00:34
standard planes to maintain symmetry of a part.
00:38
This will simplify the number of dimensions and constraints that are needed and
00:41
also make sure that the design is easy to update later on.
00:45
We're gonna set this at a width of six inches,
00:47
hit tab and move over and set this at a height of two inches and hit enter.
00:53
Now that we have the base of our design created,
00:55
I'm gonna finish the sketch and extrude this into 3D
00:59
using the extra tool. I'm gonna pull this up a distance of half inch.
01:04
We'll select. OK. And now we've begun creating our design.
01:08
I'm gonna make some modifications to this by using the fillet command.
01:12
And I wanna make sure that I get all four corners,
01:15
begin using the manipulator and set the corner radius at half inch
01:21
from here. I'm going to explore another tool, modify and shell.
01:25
We'll select the top phase and begin using
01:27
the onscreen manipulator to drag this inward.
01:30
I want to set this at a wall thickness of 0.25 inches and hit. Enter
01:35
the shell tool will maintain a quarter inch wall thickness
01:38
and a quarter inch bottom thickness based on that value.
01:42
Next, I'm gonna select this inside face right click and create a new sketch.
01:48
This will automatically project the selected face as a profile.
01:52
We can use this for things like offset or to measure from the edges.
01:56
What we want to do is create a new center point circle
02:01
with a diameter value of 0.75.
02:05
Now that we have this created,
02:07
I'm going to select the circle and I want to use the offset command
02:12
as we drag this out.
02:13
The offset command or tool will allow us
02:15
to create an offset of our selected geometry.
02:19
I'm gonna bring this out until it's offset a distance of one inch and hit. Enter,
02:23
notice that this creates a couple of different closed profile regions.
02:27
These outside profile regions are not going to be used
02:30
but we can leave them inside of the sketch.
02:33
If you go to trim the outside of the sketch,
02:36
likely you'll get issues with constraints and dimensions being broken.
02:40
So in some cases, it's easier for us to leave that information.
02:44
Next,
02:45
I'm going to use the two point rectangle and I'm going to select
02:48
the upper edge of this profile and the lower edge of this profile,
02:52
then we'll come back and add a dimension.
02:55
I want to make sure that the side of this is a distance of 0.5 inches in we'll hit enter
03:01
and then the overall width of this is gonna be a distance of 0.25.
03:06
Now that we have this object on the left hand side,
03:09
I also want to make a vertical construction line from the origin.
03:13
We'll hit escape to get off of our line tool.
03:15
And this vertical construction line needs to be changed to construction
03:19
in the sketch palette or by using X on the keyboard,
03:22
this line is going to be here so that we can use it for mirroring geometry.
03:26
Next, we're gonna select create mir
03:29
and in this instance, we don't need to grab all four edges of our rectangle.
03:33
We only need the left and the right.
03:35
We're gonna select the vertical construction line to mirror and select OK.
03:39
The main reason we only needed the left and the right lines
03:42
is because the profile is already brought in from our sketch creation.
03:46
So even though there's no short line between these two ends,
03:49
we still have a valid sketch profile.
03:52
Next, let's go ahead and finish the sketch.
03:55
Select extrude,
03:57
select these outside regions as well as this inside region and pull it upward.
04:02
We're not gonna go all the way to the top. We'll go a distance of 0.2 and select. OK.
04:07
This is now joined with the rest of the model.
04:10
If this model was created for injection molding,
04:13
we could leave these square corners.
04:14
However, they're going to be problematic if we decide to mill this part.
04:18
So we're going to go to modify select file
04:21
and note that with the file tool,
04:22
we can select these vertical edges through solid geometry.
04:26
We also need to make sure that we fill at these corners of this rectangle as well.
04:32
Some of this could be done at the sketch level.
04:35
But oftentimes it's easier for us to modify
04:37
these parameters later at the feature level,
04:40
we're going to increase this to a value that's slightly
04:42
larger than a tool that we want to use.
04:44
So this radius value of 0.15 should be large enough for us to use a quarter inch NM.
04:50
If we hit enter, we can always go back and use the inspect tool and measure the radius.
04:55
Here. We can see the radius of 0.15 that we entered, gives us a diameter value of 0.3.
05:01
This means a quarter inch tool can come in and finish these pockets
05:04
without fear of chattering in those
05:05
corners because the radius values are different
05:08
at this point. This is all we're going to do with this design.
05:11
But it's a good idea to continue to play around with sketching.
05:14
And oftentimes grab a model inside of your work area and try to replicate it in 3D.
05:20
Once you're done, feel free to save your design before moving on.
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