Transcript
00:02
Mirrors and patterns.
00:05
In this video, we’ll create a body mirror, a feature mirror, a face pattern and a component pattern.
00:12
In Fusion 360, we want to get started with the supplied dataset pipe pattern.
00:18
With pipe pattern, you'll notice that there are several components as well as bodies in this design.
00:23
We have a pipe cap, we have a pipe extension, we have a couple McMaster-Carr hardware in this case, a bolt and a nut.
00:31
And then we have a manifold.
00:33
We're going to be taking a look at various ways to mirror and pattern bodies, components and faces using this as our example.
00:40
To get started, I first want to take a look at the pipe extension.
00:44
So I'm going to activate this component, expand it and note that this has a single body.
00:50
What we want to do first is we want to take a look at creating a mirror of a body.
00:55
When we go to the Create menu, we want to navigate down to Mirror and note that it's set to bodies
01:02
but we can use this for faces, bodies, features or components.
01:07
We're going to be mirroring this entire body and the mirror plane that we're going to be using is the back face.
01:13
When we do this, we have the option to join or create a new body.
01:18
We're going to be joining these together, creating a single solid body of the pipe.
01:23
This pipe component now is still a single body but it has the extension that goes on the other side of it,
01:29
and because we used a mirror, we were able to join it.
01:33
We could also take this and we could create a pattern of it, putting it in each of the following positions.
01:40
So in order to do that, we would want to go to the rectangular pattern.
01:45
Instead of using faces, we can select bodies which will create multiple bodies inside of this component.
01:52
Or we can create individual components.
01:54
In this case, I want to pattern the component.
01:57
The component will be the pipe extension.
02:00
For our direction we're going to be using the default X direction and then we can simply begin dragging this out.
02:07
In this case, we're going to be going a total distance of minus 1000 mm.
02:12
We can define this as the entire extent or we can do it as the distance between each.
02:19
When we do it as the distance between each, that'll be minus 500 mm.
02:23
Once we say, OK, note that we now have pipe extension with the colon two and three after it.
02:30
That's because these are identical copies.
02:32
Any change that's made to the original will also modify each of these copies.
02:38
Let's activate the top level and let's take a look at some other options we have when creating mirrors and patterns.
02:44
Next, I want to focus on this pipe cap.
02:46
This is currently a body.
02:48
And what I want to do first is I want to hide my pipe extension as well as the hardware that's on this body.
02:54
I want to focus my attention on creating a pattern of this specific geometry so I can add hardware around the entire part.
03:04
We're going to start by taking a look at Create, Pattern and we want to use a circular pattern.
03:10
Because we don't necessarily know the feature that was used to create this, we can use the faces option.
03:17
By using faces we can select the fillet, the circular section, the chamfer and the inside.
03:23
When we do this, we then need to select the axis of revolution.
03:27
And I'm going to grab the outside of the part and I'm going to increase the number of instances to 10 and say OK.
03:34
When I do this, all 10 instances have been created.
03:37
However, if we view this from a back view, you'll note that the holes didn't go all the way through.
03:43
There are a couple ways that we can deal with this.
03:45
We can create a sketch to extrude all the way through.
03:48
We can go back and we can find the feature that was used to remove that hole and we can pattern that feature.
03:54
We can do this by simply selecting it and finding it inside of the timeline.
03:59
We can also create a pattern of faces.
04:02
Or we can use things like direct modeling tools such as Delete.
04:06
If I take that original feature and I go to create, patterns and circular pattern,
04:13
now the type is automatically set to features because it was pre-selected.
04:17
If I select the same axis of revolution and the same number 10 and I say OK, now we were able to remove all of those holes quickly and easily.
04:26
Sometimes if you don't have that feature available to you, you might need to use other tools like direct modeling tools.
04:33
But in this instance we had it available and we could easily add it.
04:37
Now let's bring back the hardware and the pipe extension.
04:41
The hardware is comprised of two components, a bolt and a nut.
04:45
I'm going to pre select both of those and I'm going to select the option to create a circular pattern.
04:52
The component type is automatically pre-selected as are both of the objects.
04:57
We simply need to select the axis of revolution and the number of instances.
05:02
Once we've created those instances,
05:03
you'll notice that in the browser we have a colon after each one and the number 2, 3, 4, 5, 6 all the way up through 10.
05:12
That means that any changes made to the original are going to propagate to all of these other instances since they’re exact copies.
05:21
When we use functionality like mirror, we need to be careful because that doesn't necessarily have the same option.
05:29
So let's take a look at how we can create a mirror of these components.
05:33
The first thing we need is a plane in the middle so that way we can mirror to the other position.
05:39
I'm going to go to Construct and select Midplane.
05:42
I'm simply going to select the inside faces of my pipe flange because that will give me a midplane directly in the center.
05:50
I'm going to say OK.
05:51
And I want to take a look at just creating a mirror of the original bolt and nut.
05:56
When I go to create and I select mirror, it's automatically set to components,
06:02
and can select my plane and noting that it's putting it on the opposite side.
06:07
Once we say, OK, note that inside of the browser, we now have restarted that count after the colon.
06:14
They also have mirror in the name.
06:17
That's because these mirrored components are not going to be the same as the original components.
06:23
Downstream this is problematic if you're keeping track of these items and say a bill of materials.
06:29
That parts list or bill of materials is not going to include the correct number of these items because this mirror no longer follows that same suit.
06:38
What you would want to do instead is create a copy of these and not a mirror or opposite version.
06:44
I'm going to take the mirror in the timeline, I'm going to select Delete on the keyboard to get rid of it.
06:49
And then we could take an option such as Move/Copy.
06:52
We could set the Move/Copy to components.
06:55
We could select our hardware, in this case, we want just the bolt and the nut.
07:00
We want to select Create Copy and then we can drag it to its new position.
07:06
Once we say, OK, note that inside of the browser we have 11.
07:11
So that's an important distinction to keep track of whenever you're creating assemblies of components,
07:16
especially when things like hardware are involved or exact copies of specific components like this pipe.
07:24
If we wanted to create a linear pattern of these,
07:27
we could take each of these and we could create a linear pattern just like we did with the original pipe.
07:33
That would create another instance of this that would fall in line with the same part number.
07:39
So keeping those nuances in check is important downstream, especially when we start to create detailed drawings.
07:46
Now let's take a look at the end of this manifold.
07:49
It's open on the right side but we have a cap on the left side.
07:52
Let's go back to a home view and let's focus just on the manifold.
07:57
I'm going to right click on it and isolate it.
07:60
I'm also going to activate it so that way I'm working just on the manifold.
08:04
From here I want to take a look at creating a mirror of some geometry.
08:09
Because the mirror in this case is going to apply to the same body,
08:13
I don't have to worry about the issue of creating another instance or a copy of component.
08:18
In this case, we simply want to select the inside and outside faces of that cylinder and then we want to select our mirror plane,
08:26
and then we'll say, OK.
08:29
Notice when we do this, the geometry fails.
08:32
It wasn't able to create that mirror.
08:35
This is because in this case, it's still missing some geometry.
08:40
We tried to mirror it as a face and in some cases that works fine, in other cases, it won't.
08:46
In this case however, we could take the feature, the revolve and we could create a mirror of that feature.
08:53
Once again, we'll select the mirror plane.
08:55
The compute option in this case will allow it to adjust based on its surrounding geometry.
09:00
And then it should be able to create the mirror and combine it with the rest of the geometry.
09:06
Let's do a quick check by going to Inspect and creating a section analysis,
09:11
and simply dragging a plane back through to make sure that the manifold does look correct.
09:17
We expand this, we should note that we still have a single solid body.
09:21
So this means that the mirror of that future is exactly what worked in this case.
09:27
I'm going to hide the analysis.
09:28
I'm gonna right click at the top level and unisolate all,
09:32
navigate back to the home position, activate the top level and then make sure that I save this design before moving on.
00:02
Mirrors and patterns.
00:05
In this video, we’ll create a body mirror, a feature mirror, a face pattern and a component pattern.
00:12
In Fusion 360, we want to get started with the supplied dataset pipe pattern.
00:18
With pipe pattern, you'll notice that there are several components as well as bodies in this design.
00:23
We have a pipe cap, we have a pipe extension, we have a couple McMaster-Carr hardware in this case, a bolt and a nut.
00:31
And then we have a manifold.
00:33
We're going to be taking a look at various ways to mirror and pattern bodies, components and faces using this as our example.
00:40
To get started, I first want to take a look at the pipe extension.
00:44
So I'm going to activate this component, expand it and note that this has a single body.
00:50
What we want to do first is we want to take a look at creating a mirror of a body.
00:55
When we go to the Create menu, we want to navigate down to Mirror and note that it's set to bodies
01:02
but we can use this for faces, bodies, features or components.
01:07
We're going to be mirroring this entire body and the mirror plane that we're going to be using is the back face.
01:13
When we do this, we have the option to join or create a new body.
01:18
We're going to be joining these together, creating a single solid body of the pipe.
01:23
This pipe component now is still a single body but it has the extension that goes on the other side of it,
01:29
and because we used a mirror, we were able to join it.
01:33
We could also take this and we could create a pattern of it, putting it in each of the following positions.
01:40
So in order to do that, we would want to go to the rectangular pattern.
01:45
Instead of using faces, we can select bodies which will create multiple bodies inside of this component.
01:52
Or we can create individual components.
01:54
In this case, I want to pattern the component.
01:57
The component will be the pipe extension.
02:00
For our direction we're going to be using the default X direction and then we can simply begin dragging this out.
02:07
In this case, we're going to be going a total distance of minus 1000 mm.
02:12
We can define this as the entire extent or we can do it as the distance between each.
02:19
When we do it as the distance between each, that'll be minus 500 mm.
02:23
Once we say, OK, note that we now have pipe extension with the colon two and three after it.
02:30
That's because these are identical copies.
02:32
Any change that's made to the original will also modify each of these copies.
02:38
Let's activate the top level and let's take a look at some other options we have when creating mirrors and patterns.
02:44
Next, I want to focus on this pipe cap.
02:46
This is currently a body.
02:48
And what I want to do first is I want to hide my pipe extension as well as the hardware that's on this body.
02:54
I want to focus my attention on creating a pattern of this specific geometry so I can add hardware around the entire part.
03:04
We're going to start by taking a look at Create, Pattern and we want to use a circular pattern.
03:10
Because we don't necessarily know the feature that was used to create this, we can use the faces option.
03:17
By using faces we can select the fillet, the circular section, the chamfer and the inside.
03:23
When we do this, we then need to select the axis of revolution.
03:27
And I'm going to grab the outside of the part and I'm going to increase the number of instances to 10 and say OK.
03:34
When I do this, all 10 instances have been created.
03:37
However, if we view this from a back view, you'll note that the holes didn't go all the way through.
03:43
There are a couple ways that we can deal with this.
03:45
We can create a sketch to extrude all the way through.
03:48
We can go back and we can find the feature that was used to remove that hole and we can pattern that feature.
03:54
We can do this by simply selecting it and finding it inside of the timeline.
03:59
We can also create a pattern of faces.
04:02
Or we can use things like direct modeling tools such as Delete.
04:06
If I take that original feature and I go to create, patterns and circular pattern,
04:13
now the type is automatically set to features because it was pre-selected.
04:17
If I select the same axis of revolution and the same number 10 and I say OK, now we were able to remove all of those holes quickly and easily.
04:26
Sometimes if you don't have that feature available to you, you might need to use other tools like direct modeling tools.
04:33
But in this instance we had it available and we could easily add it.
04:37
Now let's bring back the hardware and the pipe extension.
04:41
The hardware is comprised of two components, a bolt and a nut.
04:45
I'm going to pre select both of those and I'm going to select the option to create a circular pattern.
04:52
The component type is automatically pre-selected as are both of the objects.
04:57
We simply need to select the axis of revolution and the number of instances.
05:02
Once we've created those instances,
05:03
you'll notice that in the browser we have a colon after each one and the number 2, 3, 4, 5, 6 all the way up through 10.
05:12
That means that any changes made to the original are going to propagate to all of these other instances since they’re exact copies.
05:21
When we use functionality like mirror, we need to be careful because that doesn't necessarily have the same option.
05:29
So let's take a look at how we can create a mirror of these components.
05:33
The first thing we need is a plane in the middle so that way we can mirror to the other position.
05:39
I'm going to go to Construct and select Midplane.
05:42
I'm simply going to select the inside faces of my pipe flange because that will give me a midplane directly in the center.
05:50
I'm going to say OK.
05:51
And I want to take a look at just creating a mirror of the original bolt and nut.
05:56
When I go to create and I select mirror, it's automatically set to components,
06:02
and can select my plane and noting that it's putting it on the opposite side.
06:07
Once we say, OK, note that inside of the browser, we now have restarted that count after the colon.
06:14
They also have mirror in the name.
06:17
That's because these mirrored components are not going to be the same as the original components.
06:23
Downstream this is problematic if you're keeping track of these items and say a bill of materials.
06:29
That parts list or bill of materials is not going to include the correct number of these items because this mirror no longer follows that same suit.
06:38
What you would want to do instead is create a copy of these and not a mirror or opposite version.
06:44
I'm going to take the mirror in the timeline, I'm going to select Delete on the keyboard to get rid of it.
06:49
And then we could take an option such as Move/Copy.
06:52
We could set the Move/Copy to components.
06:55
We could select our hardware, in this case, we want just the bolt and the nut.
07:00
We want to select Create Copy and then we can drag it to its new position.
07:06
Once we say, OK, note that inside of the browser we have 11.
07:11
So that's an important distinction to keep track of whenever you're creating assemblies of components,
07:16
especially when things like hardware are involved or exact copies of specific components like this pipe.
07:24
If we wanted to create a linear pattern of these,
07:27
we could take each of these and we could create a linear pattern just like we did with the original pipe.
07:33
That would create another instance of this that would fall in line with the same part number.
07:39
So keeping those nuances in check is important downstream, especially when we start to create detailed drawings.
07:46
Now let's take a look at the end of this manifold.
07:49
It's open on the right side but we have a cap on the left side.
07:52
Let's go back to a home view and let's focus just on the manifold.
07:57
I'm going to right click on it and isolate it.
07:60
I'm also going to activate it so that way I'm working just on the manifold.
08:04
From here I want to take a look at creating a mirror of some geometry.
08:09
Because the mirror in this case is going to apply to the same body,
08:13
I don't have to worry about the issue of creating another instance or a copy of component.
08:18
In this case, we simply want to select the inside and outside faces of that cylinder and then we want to select our mirror plane,
08:26
and then we'll say, OK.
08:29
Notice when we do this, the geometry fails.
08:32
It wasn't able to create that mirror.
08:35
This is because in this case, it's still missing some geometry.
08:40
We tried to mirror it as a face and in some cases that works fine, in other cases, it won't.
08:46
In this case however, we could take the feature, the revolve and we could create a mirror of that feature.
08:53
Once again, we'll select the mirror plane.
08:55
The compute option in this case will allow it to adjust based on its surrounding geometry.
09:00
And then it should be able to create the mirror and combine it with the rest of the geometry.
09:06
Let's do a quick check by going to Inspect and creating a section analysis,
09:11
and simply dragging a plane back through to make sure that the manifold does look correct.
09:17
We expand this, we should note that we still have a single solid body.
09:21
So this means that the mirror of that future is exactly what worked in this case.
09:27
I'm going to hide the analysis.
09:28
I'm gonna right click at the top level and unisolate all,
09:32
navigate back to the home position, activate the top level and then make sure that I save this design before moving on.
Step-by-step guide
