& Construction
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& Manufacturing
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Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
Create a three d. mechanical link.
00:05
After completing this video, you'll be able to
00:08
disable, capture design history,
00:09
create a fully defined sketch and use extrude and fill it.
00:14
Infusion 3 60. Let's get started with the supply data set D.
00:17
Feature link dot F three D.
00:20
In most cases when you upload an F three D.
00:22
To fusion 3 60 it contains history of how the part was created. In some cases in F.
00:27
Three D. Can be created but not contain any history now.
00:31
This imported model doesn't contain any sketch
00:33
or feature history that can be manipulated.
00:35
We want to create a full featured parametric model of this link
00:39
and there are a couple ways that we can do this first.
00:42
Let's talk about capturing design history and what that actually means.
00:46
Infusion 3 60 anytime we create a sketch of feature or
00:49
any of the other tools used in fusion 3 60 history is
00:53
maintained meaning that there is an order of operations to create that
00:56
part and something that we can go back to to manipulate.
00:60
In a case like this, we have an F. Three D file that doesn't contain that history
01:04
in order to create it.
01:05
We can use this as a reference but we need
01:06
to be careful not to project references from this design.
01:10
Otherwise we will contain links between the two and really
01:14
what we want is a fully featured dimension model.
01:16
So to get started,
01:18
I want to talk about capturing design history and how we can turn that on and off.
01:22
First. Let's take a look at the create menu and notice at the very bottom.
01:26
The last two options are creating a PCB and creating a base feature.
01:30
Next let's go to the gear icon in the bottom right of fusion 360 and turn on.
01:35
Do not capture design history.
01:37
We're going to select continue and if you
01:39
have a design that contains sketches and features,
01:42
all history will be removed.
01:44
Now the reason that this is important is because there are some tools that
01:47
are enabled once history has been turned off for example under the create menu.
01:52
Now we can see find features and fluid volume.
01:55
These tools are available in other areas of fusion 3 60 such
01:59
as when you're simplifying a geometric design for use with things like
02:03
generative design or simulation.
02:05
But for right now if we select find features
02:08
we expand our crank arm component
02:10
and we select the body.
02:12
We can have it look for things like patterns, mirrors revolves extrude and champers
02:17
we say okay
02:19
it creates a history in the browser.
02:21
It lets us know how it thinks this part was created.
02:24
Notice that there are a lot of extrude revolves.
02:27
There's a mirror of certain geometry.
02:29
You can see here that these occurrences are the text on the other side of the link.
02:33
Also note that there are a lot of filets.
02:35
These filets are contained on a lot of the text
02:38
as well as in certain areas of the model.
02:41
Now even though we have this history in the browser not everything can be changed.
02:46
Some things can be edited. Things like filets.
02:48
However, if we select an extrude and right click there's no edit option.
02:53
So another thing that we can do when history is
02:55
turned off is we can manually de feature this part.
02:58
If it helps us reverse engineer it.
03:00
For example if we want to get rid of the recesses and
03:03
the text we can select these inside faces holding down the shift key
03:08
and then we can go to modify and delete
03:11
Fusion 3 60 is able to patch and reconcile the
03:14
geometry around this area by simply removing those faces.
03:18
You can also use delete on the keyboard to make that happen.
03:22
Other areas of the design such as these filets can be removed as well. If we wish
03:27
for example we can select the filets on this end and hit delete
03:32
once we're done removing features from apart to
03:35
help us reverse engineer it we can always
03:37
go back to the top level of our browser right click and capture design history.
03:42
This will create a new component and base feature for the crank arm but
03:46
any of the history that was used to remove certain features has been erased.
03:51
So at this point in time it's important to note that this crank arm
03:54
is a component and when starting new designs in fusion 3 60 in general,
03:59
it's a good idea to create a new
04:00
component components are required for mechanical motion.
04:04
They ease when you're creating exploded views and animations
04:07
and they also help downstream when creating detailed drawings.
04:10
They also will aid an organization of your timeline and your browser.
04:15
So for this example let's get started by going to assemble and new component,
04:20
we're going to be creating a new component called link
04:24
and will simply hit enter
04:26
the new component is created which contains its own coordinate system.
04:30
If we take a look at this,
04:31
you can see that the coordinate system is placed well above the current link.
04:35
And if we view this from the front we can actually see that the crank arm is at an angle.
04:40
Remember that we don't want to project any references
04:43
from the crank arm into our new link.
04:45
So we're just going to be using it for measurement values.
04:48
I'm going to rotate this around and just make quick note of inspection values.
04:53
We have 10.2 millim diameter on the big end and we have a distance of 49.637.
05:01
Notice that this is a straight line distance. If we want to get an accurate distance.
05:05
It's a good idea to select the boars and we can get a distance between this.
05:10
We can also add comments to the design.
05:12
For example, 10.2 millimeter diameter big end
05:19
diameter small end.
05:22
I'm going to select post and now the comment is saved in my design.
05:26
It's a good time for you to practice using inspect and measure.
05:29
So go ahead and measure a couple other areas of the design.
05:32
For example, the distance between the top and the bottom face is 6.51 mm.
05:38
You can measure the distance between two faces here to figure
05:42
out what the distances between the opening and the closing sections.
05:46
And we can also figure out what the bore diameter is and distances for filets.
05:52
Once you've measured all those values, let's get started by creating a new sketch.
05:56
We're going to rotate this around and we're going to select the
05:59
front plane and we're going to base our design about the origin.
06:02
So using a center diameter circle,
06:05
we'll start there creating an inside and an outside diameter
06:08
and we'll do the same thing on the back.
06:11
We want to make sure that there is a horizontal vertical
06:13
constraint between the centers of each side of the link.
06:17
And then we can use our dimension tool to place
06:19
a dimension of 10.2 mm on the big end and 10
06:24
on the small end.
06:26
The outside diameter value isn't as critical, but I'm going to place this at 19 mm,
06:30
making both of these the same.
06:34
The distance between the two center points is going to
06:36
be important for the overall motion of the reciprocating saw.
06:40
In this case, I'm going to be using a value of 49.5.
06:44
Next we need to create the rectangular portion in the center
06:48
for this. I'm going to use a line from center to center.
06:51
I'm going to hit escape to get off my line tool.
06:54
I'm going to convert this to construction using my sketch palette
06:57
With it still selected. I'll use offset and I'll offset a distance of 5 mm
07:02
with the offset line. We can then use mirror
07:05
to create a mirror of that line,
07:07
selecting our horizontal construction line.
07:11
Then we want to create the flat spots on the back side of the link
07:14
for this.
07:15
I'm going to use my line tool making sure that I snapped to the outside diameter
07:19
and then use my dimension tool for the angle.
07:22
This is going to be 45 degrees overall.
07:25
So I need to make it 22 a half degrees on the one side.
07:30
Then I'll use the horizontal vertical constraint
07:32
and once more will mirror that geometry across to the other side.
07:36
Using mirror means if we make any changes to the overall design.
07:40
For example, if we decide that this angle needs to be steeper,
07:43
we can adjust it to 25° and both sides will change for this example,
07:47
we are going to stick with 22.5°.
07:51
There is one more element that we need to know and that's
07:53
going to be the diameter of the cut on the inside.
07:56
You can see that this contains a flat here.
07:59
Now we want to figure out exactly where that flat is,
08:01
it doesn't look like there's a lot of space here,
08:04
but we need to make sure that we do account for that for this.
08:07
I'm going to create another extrude. I'm going to use a small circle
08:13
and I just want to give it roughly the right size
08:18
Looking like we're gonna be at about 13 mm. This is going to be a reference for me.
08:22
So I'm going to select that and convert it to construction.
08:26
Then I want to create a vertical line that goes from the outside to outside.
08:30
And I'm going to apply a tangent constraint between it and the circle.
08:35
So this gives me the flat spot that I need.
08:37
And I can modify this dimension value,
08:39
say down to 12 or up to 14 and have
08:43
that line adjust its position figuring out these references.
08:47
It's going to be an important aspect of building a parametric design,
08:50
understanding how you want to dimension something so that it can update properly.
08:55
Next we're going to finish the sketch and we'll
08:56
be using this to create the solid body.
08:59
Well, first begin by extruding the smaller section,
09:02
I'm going to use the direction set to symmetric,
09:06
set the measurement value so that it's the full length
09:09
And this section is going to be a distance of 7.45 mm.
09:14
We'll need to expand the sketches and bring the sketch back.
09:17
We're going to exclude the other side,
09:19
making sure to include everything with the exception of these small sections.
09:23
Once again using symmetric setting it to the full length and
09:28
this side is going to be a distance of 13 mm.
09:32
We're going to right click and repeat the extrude
09:34
this time. We're going to extrude the center section.
09:37
This is going to be symmetric again the whole length and 6.5 mm.
09:43
Now we need to remove the section from the center.
09:46
Once again we can right click and repeat the
09:48
extrude and we can select the center section.
09:52
We need to hold down control or command to select multiple profiles.
09:56
Use the symmetric option the whole length one more
09:59
time and the distance between these is 4.65 mm.
10:04
Now that we've removed all of that information.
10:06
We can hide the sketch, we can hide our crank arm and we can apply some filets.
10:11
So from modify fill it.
10:13
I'm going to select the two vertical edges on the big
10:16
side and the two vertical edges on the smaller side.
10:19
And I'm going to apply a five millimeter Philip.
10:22
I'm going to right click and repeat this and apply it to the top and bottom.
10:26
This time I'm going to use the on screen manipulator and drag this out
10:30
and in this case 5.5 millimeters. And hit enter too. Okay,
10:35
so now we've recreated the link using a single sketch and
10:39
all the dimensions required as well as a handful of features.
10:42
Now we have a fully featured parametric version of this link.
10:46
We don't have the recesses or the text that was included on the original.
10:50
But all the critical features, including the hole diameters,
10:53
thicknesses and required geometry are there at this point.
10:57
Let's make sure that we do save our new link.
10:59
And instead of doing a save, I'm going to do a save as
11:03
notice that I have another folder in this case,
11:06
I want to go back and go into my parametric
11:08
modeling folder and I'm going to call this one parametric link
11:13
from here.
11:13
Continue to make any adjustments or modifications that you see fit
11:16
and then make sure that you save it before moving on.
00:02
Create a three d. mechanical link.
00:05
After completing this video, you'll be able to
00:08
disable, capture design history,
00:09
create a fully defined sketch and use extrude and fill it.
00:14
Infusion 3 60. Let's get started with the supply data set D.
00:17
Feature link dot F three D.
00:20
In most cases when you upload an F three D.
00:22
To fusion 3 60 it contains history of how the part was created. In some cases in F.
00:27
Three D. Can be created but not contain any history now.
00:31
This imported model doesn't contain any sketch
00:33
or feature history that can be manipulated.
00:35
We want to create a full featured parametric model of this link
00:39
and there are a couple ways that we can do this first.
00:42
Let's talk about capturing design history and what that actually means.
00:46
Infusion 3 60 anytime we create a sketch of feature or
00:49
any of the other tools used in fusion 3 60 history is
00:53
maintained meaning that there is an order of operations to create that
00:56
part and something that we can go back to to manipulate.
00:60
In a case like this, we have an F. Three D file that doesn't contain that history
01:04
in order to create it.
01:05
We can use this as a reference but we need
01:06
to be careful not to project references from this design.
01:10
Otherwise we will contain links between the two and really
01:14
what we want is a fully featured dimension model.
01:16
So to get started,
01:18
I want to talk about capturing design history and how we can turn that on and off.
01:22
First. Let's take a look at the create menu and notice at the very bottom.
01:26
The last two options are creating a PCB and creating a base feature.
01:30
Next let's go to the gear icon in the bottom right of fusion 360 and turn on.
01:35
Do not capture design history.
01:37
We're going to select continue and if you
01:39
have a design that contains sketches and features,
01:42
all history will be removed.
01:44
Now the reason that this is important is because there are some tools that
01:47
are enabled once history has been turned off for example under the create menu.
01:52
Now we can see find features and fluid volume.
01:55
These tools are available in other areas of fusion 3 60 such
01:59
as when you're simplifying a geometric design for use with things like
02:03
generative design or simulation.
02:05
But for right now if we select find features
02:08
we expand our crank arm component
02:10
and we select the body.
02:12
We can have it look for things like patterns, mirrors revolves extrude and champers
02:17
we say okay
02:19
it creates a history in the browser.
02:21
It lets us know how it thinks this part was created.
02:24
Notice that there are a lot of extrude revolves.
02:27
There's a mirror of certain geometry.
02:29
You can see here that these occurrences are the text on the other side of the link.
02:33
Also note that there are a lot of filets.
02:35
These filets are contained on a lot of the text
02:38
as well as in certain areas of the model.
02:41
Now even though we have this history in the browser not everything can be changed.
02:46
Some things can be edited. Things like filets.
02:48
However, if we select an extrude and right click there's no edit option.
02:53
So another thing that we can do when history is
02:55
turned off is we can manually de feature this part.
02:58
If it helps us reverse engineer it.
03:00
For example if we want to get rid of the recesses and
03:03
the text we can select these inside faces holding down the shift key
03:08
and then we can go to modify and delete
03:11
Fusion 3 60 is able to patch and reconcile the
03:14
geometry around this area by simply removing those faces.
03:18
You can also use delete on the keyboard to make that happen.
03:22
Other areas of the design such as these filets can be removed as well. If we wish
03:27
for example we can select the filets on this end and hit delete
03:32
once we're done removing features from apart to
03:35
help us reverse engineer it we can always
03:37
go back to the top level of our browser right click and capture design history.
03:42
This will create a new component and base feature for the crank arm but
03:46
any of the history that was used to remove certain features has been erased.
03:51
So at this point in time it's important to note that this crank arm
03:54
is a component and when starting new designs in fusion 3 60 in general,
03:59
it's a good idea to create a new
04:00
component components are required for mechanical motion.
04:04
They ease when you're creating exploded views and animations
04:07
and they also help downstream when creating detailed drawings.
04:10
They also will aid an organization of your timeline and your browser.
04:15
So for this example let's get started by going to assemble and new component,
04:20
we're going to be creating a new component called link
04:24
and will simply hit enter
04:26
the new component is created which contains its own coordinate system.
04:30
If we take a look at this,
04:31
you can see that the coordinate system is placed well above the current link.
04:35
And if we view this from the front we can actually see that the crank arm is at an angle.
04:40
Remember that we don't want to project any references
04:43
from the crank arm into our new link.
04:45
So we're just going to be using it for measurement values.
04:48
I'm going to rotate this around and just make quick note of inspection values.
04:53
We have 10.2 millim diameter on the big end and we have a distance of 49.637.
05:01
Notice that this is a straight line distance. If we want to get an accurate distance.
05:05
It's a good idea to select the boars and we can get a distance between this.
05:10
We can also add comments to the design.
05:12
For example, 10.2 millimeter diameter big end
05:19
diameter small end.
05:22
I'm going to select post and now the comment is saved in my design.
05:26
It's a good time for you to practice using inspect and measure.
05:29
So go ahead and measure a couple other areas of the design.
05:32
For example, the distance between the top and the bottom face is 6.51 mm.
05:38
You can measure the distance between two faces here to figure
05:42
out what the distances between the opening and the closing sections.
05:46
And we can also figure out what the bore diameter is and distances for filets.
05:52
Once you've measured all those values, let's get started by creating a new sketch.
05:56
We're going to rotate this around and we're going to select the
05:59
front plane and we're going to base our design about the origin.
06:02
So using a center diameter circle,
06:05
we'll start there creating an inside and an outside diameter
06:08
and we'll do the same thing on the back.
06:11
We want to make sure that there is a horizontal vertical
06:13
constraint between the centers of each side of the link.
06:17
And then we can use our dimension tool to place
06:19
a dimension of 10.2 mm on the big end and 10
06:24
on the small end.
06:26
The outside diameter value isn't as critical, but I'm going to place this at 19 mm,
06:30
making both of these the same.
06:34
The distance between the two center points is going to
06:36
be important for the overall motion of the reciprocating saw.
06:40
In this case, I'm going to be using a value of 49.5.
06:44
Next we need to create the rectangular portion in the center
06:48
for this. I'm going to use a line from center to center.
06:51
I'm going to hit escape to get off my line tool.
06:54
I'm going to convert this to construction using my sketch palette
06:57
With it still selected. I'll use offset and I'll offset a distance of 5 mm
07:02
with the offset line. We can then use mirror
07:05
to create a mirror of that line,
07:07
selecting our horizontal construction line.
07:11
Then we want to create the flat spots on the back side of the link
07:14
for this.
07:15
I'm going to use my line tool making sure that I snapped to the outside diameter
07:19
and then use my dimension tool for the angle.
07:22
This is going to be 45 degrees overall.
07:25
So I need to make it 22 a half degrees on the one side.
07:30
Then I'll use the horizontal vertical constraint
07:32
and once more will mirror that geometry across to the other side.
07:36
Using mirror means if we make any changes to the overall design.
07:40
For example, if we decide that this angle needs to be steeper,
07:43
we can adjust it to 25° and both sides will change for this example,
07:47
we are going to stick with 22.5°.
07:51
There is one more element that we need to know and that's
07:53
going to be the diameter of the cut on the inside.
07:56
You can see that this contains a flat here.
07:59
Now we want to figure out exactly where that flat is,
08:01
it doesn't look like there's a lot of space here,
08:04
but we need to make sure that we do account for that for this.
08:07
I'm going to create another extrude. I'm going to use a small circle
08:13
and I just want to give it roughly the right size
08:18
Looking like we're gonna be at about 13 mm. This is going to be a reference for me.
08:22
So I'm going to select that and convert it to construction.
08:26
Then I want to create a vertical line that goes from the outside to outside.
08:30
And I'm going to apply a tangent constraint between it and the circle.
08:35
So this gives me the flat spot that I need.
08:37
And I can modify this dimension value,
08:39
say down to 12 or up to 14 and have
08:43
that line adjust its position figuring out these references.
08:47
It's going to be an important aspect of building a parametric design,
08:50
understanding how you want to dimension something so that it can update properly.
08:55
Next we're going to finish the sketch and we'll
08:56
be using this to create the solid body.
08:59
Well, first begin by extruding the smaller section,
09:02
I'm going to use the direction set to symmetric,
09:06
set the measurement value so that it's the full length
09:09
And this section is going to be a distance of 7.45 mm.
09:14
We'll need to expand the sketches and bring the sketch back.
09:17
We're going to exclude the other side,
09:19
making sure to include everything with the exception of these small sections.
09:23
Once again using symmetric setting it to the full length and
09:28
this side is going to be a distance of 13 mm.
09:32
We're going to right click and repeat the extrude
09:34
this time. We're going to extrude the center section.
09:37
This is going to be symmetric again the whole length and 6.5 mm.
09:43
Now we need to remove the section from the center.
09:46
Once again we can right click and repeat the
09:48
extrude and we can select the center section.
09:52
We need to hold down control or command to select multiple profiles.
09:56
Use the symmetric option the whole length one more
09:59
time and the distance between these is 4.65 mm.
10:04
Now that we've removed all of that information.
10:06
We can hide the sketch, we can hide our crank arm and we can apply some filets.
10:11
So from modify fill it.
10:13
I'm going to select the two vertical edges on the big
10:16
side and the two vertical edges on the smaller side.
10:19
And I'm going to apply a five millimeter Philip.
10:22
I'm going to right click and repeat this and apply it to the top and bottom.
10:26
This time I'm going to use the on screen manipulator and drag this out
10:30
and in this case 5.5 millimeters. And hit enter too. Okay,
10:35
so now we've recreated the link using a single sketch and
10:39
all the dimensions required as well as a handful of features.
10:42
Now we have a fully featured parametric version of this link.
10:46
We don't have the recesses or the text that was included on the original.
10:50
But all the critical features, including the hole diameters,
10:53
thicknesses and required geometry are there at this point.
10:57
Let's make sure that we do save our new link.
10:59
And instead of doing a save, I'm going to do a save as
11:03
notice that I have another folder in this case,
11:06
I want to go back and go into my parametric
11:08
modeling folder and I'm going to call this one parametric link
11:13
from here.
11:13
Continue to make any adjustments or modifications that you see fit
11:16
and then make sure that you save it before moving on.
Step-by-step