Create holes and threads

00:02

Create holes and threads.

00:05

In this video, we'll use hole, we’ll use hole with a sketch reference and we'll use thread.

00:12

In Fusion 360, we want to get started with the supplied data set, gear reduction housing assembly detail.

00:18

We want to start by selecting gear housing assembly, right clicking and isolating.

00:24

We want to isolate it because we want to show the holes in the design,

00:27

and we want to make sure that we understand whether or not they're the correct sizes.

00:32

The first thing that we want to do is we want to identify the threaded areas in the housing.

00:38

We view this from the front.

00:40

You can see that we have a smaller area in here and we have the appearance of a thread.

00:46

Let's go ahead and take a look at Inspect to make sure that these are the correct size.

00:51

You'll note that the diameter of the upper portion is 6 mm.

00:55

And if we select in the canvas area and we select the diameter of the threaded portion, we can see that it's 5.035 mm.

01:04

We can check a thread chart to make sure that this is the correct size for tapping an M6 hole.

01:11

You'll also note that this hole is blind.

01:13

It's going into the housing and not out the back side.

01:16

But let's take a look at some of the other areas.

01:19

Note that we don't see any cosmetic threads here but let's inspect the hole to make sure that it is the right size.

01:25

This one's exactly 5 mm and the upper portion is exactly 6 mm.

01:31

That's slightly different from the areas that have the cosmetic thread appearance.

01:36

So let's take a look at the gear housing and see how we can add this.

01:40

I'm going to hide the front housing as well as the front cover and I want to activate the back housing.

01:45

I’m going to focus my attention just on these holes.

01:49

I'm going to start by creating a sketch.

01:52

The sketch creation is not strictly required but it does help speed things up a little bit.

01:57

We're going to use the create point option and place a point at the center of all the holes that are of interest.

02:06

Once we do that, we can finish the sketch and we want to go to Create and Hole.

02:13

Inside of here the placement option can be single or it can be from sketch.

02:18

We're going to use these From Sketch option and select all of our sketch points.

02:23

Don't worry about the preview on the screen as we're going to adjust the size and type of the hole.

02:28

Now that we have all of them selected, we're going to change the hole type.

02:32

We're going to set it to Tapped and then we need to select the size.

02:36

This will be an isometric profile and we want to go until we find 6 millimeter.

02:43

We're going to be using an M6x1 and note that we only have a single option for the thread class set to 6H.

02:50

When we do this, it's going to adjust the hole size for us.

02:54

Note that we can set it to Modeled which will put a physical thread in the hole or we can have it be cosmetic.

03:02

When we do this, we should also pay attention to the objects to cut.

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Right now we only have the back housing visible so it's only going to cut through it.

03:09

But if we had other bodies visible, we'd want to make sure that we're only applying this to the back housing.

03:15

We can modify other parameters such as the extent if we wanted to go to the back of the housing for example.

03:23

And we want the bottom to be flat instead of tapered.

03:27

We can set all of those different options.

03:29

So that way we are dealing with a completely threaded hole.

03:33

We're going to say OK.

03:35

And now if we use Inspect and we measure the diameter of one of these holes, we'll see that now instead of 5 mm, it's 5.035 mm.

03:45

Let's go back to a home view and let's right click at the very top level of the assembly and unisolate all.

03:51

This will bring everything back with the exception of the front housing and front cover.

03:57

We still have the back housing active so the opacity of everything else changes.

04:01

So let's go ahead and activate the top level.

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The next thing that we want to focus on is this gear on the inside.

04:08

This is our spur gear 16 teeth, so I'm going to right click and isolate that.

04:13

We want to add a physical thread to this section of the shaft.

04:17

So the first thing that I want to do is I want to make sure that I activate this gear and focus my attention solely on it.

04:24

Next from Create instead of using hole, we're now going to use a tool called Thread.

04:29

When we look through here, you'll notice that thread and hole are in the same section.

04:34

Thread can be used on holes that are already created,

04:37

or we could use hole at the same time to create not only the hole in the object but also the physical threads.

04:44

For creating external threads, however, we want to use the Thread tool.

04:48

We're going to select the faces and we're going to use the modeled option.

04:52

So select modeled and for the faces, let's select this external section.

04:57

Going to navigate to a right view and zoom in so I can see the physical threads.

05:02

We also have some options to modify things like its size, its profile and the designation.

05:09

Also note that there is a remember size option if you plan to create multiples.

05:15

One thing that you will note is that we are seeing a very sharp edge that's being created on the front side.

05:22

If we turn off the full length option, we can actually change where this is starting.

05:29

But because we are actually starting on a face that has a taper on the front side, it's not going to allow us to go further than that front edge.

05:38

So keep in mind that there are some limitations when we're using this full length option.

05:43

And if we want to have the thread go all the way to the end, we might need to modify some of these parameters.

05:50

Note that we have a length and an offset value.

05:53

If we offset it 1 millimeter, note that it's offsetting it from the back side.

05:58

And the length of this, if we set it to 10.5 mm, note that it's not able to create it for the full distance.

06:08

So for this example I'm going to select full length, say OK, and I want to take a look at the chamfer that's created on the end of this.

06:16

I'm going to right click on the chamfer and edit the feature.

06:19

Holding down the control or command key, I'm going to deselect that front edge and say OK.

06:25

When I do this, it's going to modify that face selection.

06:28

Now you can see that the thread does come all the way out and if we need to create a chamfer on the front of it,

06:33

we can do so with a revolve cut or we could add the chamfer back if needed.

06:38

For this example however, you might not want a physical thread, you might want just a cosmetic appearance.

06:44

If that's the case, we can always go back in and modify that tool.

06:48

Or we can go into our top level settings and modify the document settings for the thread type.

06:54

Overall we can have modeled or cosmetic.

06:58

If we set everything to cosmetic at the top level, it will override those settings in each of those individual features.

07:05

We can always go back to those individual features and we can modify them.

07:09

But this is a great way for us to also go back and include the chamfer on that front edge,

07:14

without having to worry about the remnant that's left behind from the model thread.

07:19

This can still be manufactured and in most cases, you aren't going to want the physical threads on the part when you manufacture it.

07:26

At this point, let's activate the top level, right click and unisolate all.

07:32

Go back to a home view and then let's make sure that we save this design before moving on.