Drill and tap

00:02

In this video, we're going to drill and tap.

00:06

After completing this step, you'll be able to create a spot drill operation, create a peck drill operation and create a tapping operation.

00:15

In Fusion 360, we want to carry on with our CAD/CAM Milling dataset.

00:19

At this point, we've gone all the way through the model, to rough and finish the major geometry and we've roughed and finish the slots.

00:27

Now we need to drill and tap all the holes in the design.

00:30

To do this, we're going to start by going to drilling and select the drill operation.

00:35

We need to select the proper tool so we'll go into our introduction library.

00:39

A note that we have a drill, a spot drill and then we have a tap.

00:43

For this operation, we're going to select the 5 mm spot drill.

00:47

One thing to note is none of the tools so far have had tool numbers which means that Fusion 360 is automatically going to increment them for us.

00:56

If you're starting fresh and don't have predefined tools inside of your machine, this can work.

01:01

However, it's always a good idea to define those tool numbers.

01:05

So once we're done programming the part we're going to go back and make some adjustments to these tool numbers.

01:10

Now that we have our tool selected, we need to move on to our geometry.

01:14

There are a few different ways that we can select holes in Fusion 360. We can manually select them based on faces.

01:21

We can use some other options such as selected points which allows us to select an edge

01:26

and it will automatically grab the center point or we can use the option to give it a diameter range.

01:33

We know that we're drilling a hole for an M5.

01:36

So if we set the lower end at 4 mm, noticed that it automatically grabbed all the holes for us and it knows exactly what the depth is.

01:45

We're going to move on to the heights section but note that we're using a spot drill.

01:49

So instead of using the whole bottom, I'm going to use the whole top and check the drill tip through bottom,

01:56

which allows the end of the spot drill to go through all the way up to the end of its taper.

02:01

This works for a smaller spot drill but if you have a larger spot drill, you want to be careful that you're not exceeding the diameter of the hole.

02:09

And lastly we needed to find the cycle. For us, drilling rapid out is going to work fine because we're barely taking the drill tip into the material.

02:17

So we're going to say, okay.

02:19

Now it starts at the red arrow and it moves its way all the way around until it gets to the green arrow.

02:26

Now we want to drill the holes so I'm going to right click on this drilling operation and duplicate it.

02:33

I'm going to select the duplicate right click and edit.

02:37

Now we're going to change our tool instead of using the spot drill, we want to use our 4.2 mm drill.

02:44

Once again, the drill bit doesn't have a tool number so it's automatically incremental.

02:50

The whole geometry is going to be the same.

02:52

However, I'm going to use the reverse order option

02:54

which means it's going to start at the hole that it finished the spot drilling and work its way backwards.

02:60

On this specific part, it's not going to make much of a difference because it could simply jump to the next location.

03:07

But depending on the specific hole pattern, this can save a lot of time.

03:11

Next, we want to make sure that we take a look at the heights and we use whole bottom.

03:17

It's also important to note that the whole bottom is going to be based on the entire depth of the hole.

03:24

And we need to keep in mind that these are tapped holes.

03:27

If we're drilling exactly to the whole bottom,

03:29

we don't want to tap to the whole bottom because we're going to be bottoming out the tap on solid geometry.

03:36

So we need to be real careful on the detailed drawing to see if we need the exact depth of threads or if we need the exact depth of the hole.

03:45

Depending on geometry on the other side of the part, one of them might be more important than the other.

03:51

We're going to be using the whole death as the bottom.

03:54

So we're going to move on to our cycle and we're going to change this to a different type of cycle

03:58

because we don't want to feed all the way through the hole.

04:01

We want to allow it to extract some chips.

04:03

There are two options that we have chip breaking partial were tracked and deep drilling.

04:09

The chip breaking partial retract will allow it to go down a set amount, come back slightly and then proceed to go down again.

04:16

When we use full retract, it'll use that same packing depth however, will retract completely out of the hole.

04:24

This helps evacuate chips from the hole and in some cases this is going to be more important.

04:29

However, for our case we're going to use the partial attract as this will work fine for our geometry.

04:34

Using the default settings for packing depth and amount we're going to say, okay.

04:40

Now that we've created our spot drill and our drilling operation, it's time to create our tapping operation.

04:46

I'm gonna right click and I'm gonna duplicate this one more time.

04:51

Then we're going to right click and edit the duplicate.

04:54

Now, instead of drilling we're going to use our 5 mm tap and we're going to select that tool.

05:01

In the geometry section we'll deselect reverse. So now we're starting at the original point working our way around.

05:08

In the heights section, we want to be careful of the whole bottom because again we don't want to bottom out the tap.

05:14

So I'm going to add a positive value of .5 mm. So that way the tap doesn't go all the way to the bottom.

05:22

This generally needs to be figured out based on your specific geometry.

05:26

If you have a certain amount of threads that are going to be tapered and you need a full depth thread,

05:32

you need to calculate how deep your hole needs to go relative to the tap you're using.

05:37

And lastly the cycle needs to be changed to a tapping cycle.

05:41

This is extremely important as it slows down the spindle speed and also it synchronizes the spindle speed with the Z depth.

05:50

So this allows us to go to the bottom of the hole at the specific thread pitch

05:54

and then it will reverse the spindle as it's retracting out of the hole.

05:58

We're going to say okay. And now we've created our spot drilling, our drilling and our tapping operations.

06:05

At this point, we want to validate our tool numbers.

06:08

So we have tool one which is our large end mill tool to which was our 4 mm end mill.

06:13

And we have to all 3, 4 and 5 for spot drilling, drilling and tapping.

06:18

If we go back into our tool library, we have our library that we're using but we also have our CAD/CAM Milling dataset.

06:25

If we're going to carry on using these tools and we want to restructure the tool numbers.

06:30

We can modify them here by right clicking and re-numbering specific tools

06:35

or we can edit the tool and we can go to its post processor section to change the tool number.

06:41

Either option is going to be fine.

06:43

But when we're in the tool library and we're inside of our document, renumbering the tools,

06:49

in this case, using the re-number tool option allows us to pick the first tool and then we can change its offset value.

06:57

So it's important to note the options that we have.

07:01

But in our specific instance, we're going to carry on using these predefined tool numbers.

07:05

And that means that when we set up the machine, we need to make sure that the tool numbers match the specific cycles that are using them.

07:13

This helps us keep our tools in order inside of the tool changer.

07:17

And depending on the speed of your tool changer, this could save you a little bit of programming time.

07:23

We're going to save this design before moving on.