Create a tool library

00:02

In this video, will create a tool library.

00:05

After completing this step,

00:07

you'll be able to modify user preferences to enable cloud libraries, create a new cloud library and modify tool parameters.

00:16

In fusion 360, we're going to get started with a new untitled document.

00:20

First, we want to go up to our user preferences and make sure that we have cloud libraries enabled.

00:26

You can find this in the general manufacturer section as a check box.

00:30

Once we ensure that those are enabled, we're going to navigate to the manufacturer workspace, I'm going to change my default units.

00:38

I'm going to set this 2 inch for this design and then I want to go to manage and tool library.

00:45

Inside of here, if we've enabled cloud libraries, we should now see cloud and local.

00:50

Inside of a cloud, we're going to right click and create a new tool library.

00:55

I'm going to call this one cam DFM or cam designed for manufacturer.

01:01

Notice that there is no data in here.

01:03

Now in side of the tool library we can either create new tools or we can copy them from the fusion 360 library.

01:10

To do that, we're going to get started by left clicking on the fusion library.

01:14

Going up to the right, first, we're going to filter by hole making.

01:20

When we take a look at whole making we want to look for a spot drill. And then we want to identify an

01:28

We're going to select the 8th inch spot drill and notice at the bottom we have a lot of different cutting data.

01:33

This doesn't matter at the moment for us really. We need to right click and copy the tool.

01:38

Then navigate back to our cam DFM library and paste the tool.

01:43

We're going to select it right click and edit.

01:47

We're going to change the post processor data because we want this to be tool number one.

01:51

It changes both the length and the diameter offsets as well.

01:56

In the general section, the description eight inch spot drill is still fine,

01:59

in the culture section, we can modify any parameters that we need.

02:03

Inside of here, this has the number of flutes, the diameter of the tool and how far it's sticking out from the holder.

02:09

You'll notice that this is a relatively small tool and a large standard cap 40 holder.

02:15

That's okay for this example. But note that we do want to make sure that we replicate the holder based on what's actually holding our tool.

02:23

There's information about the holder and we can select another one, such as a drill chuck if needed.

02:27

And then there's cutting data which determines how fast the rpm's are and how fast the tool is going to be moving.

02:34

In this case, I'm going to reduce the spindle rpm which is a rather large number. And I'm going to set this to 5000 rpm.

02:42

When I do that, notice that it modifies some of the other values.

02:46

Right now, it's set to feet per minute.

02:48

You also notice that there are vertical feed rates since this is a spot drill,

02:52

it's not going to be moving in the X and y, it's simply going to be moving vertically.

02:57

Right now the plunge feed rate is set to 21 and the feed per revolution is set to a relatively small number.

03:04

We're going to set the feed rate to a smaller number.

03:08

So this plunge value instead is going to be 4 inches per minute. And they're attract rate will leave at

03:15

Notice that when we change the plunge feed rate,

03:17

it automatically changes the feed per revolution because this is linked based on the back end parameters.

03:23

From here, we can accept the change and now we need to continue to populate our tool library.

03:29

When we go back to the fusion library, you'll notice that everything is still a spot drill and that's because our filter is still active.

03:36

We can clear the tool category and the filters,

03:38

and now we can take a look at milling or whole making and notice that it changes what we see in the library.

03:45

We need to add some drills and taps before we get into our end mills. So let's go ahead and look for a number seven drill.

03:52

We can do this by scrolling through the library or we can use diameter ranges.

03:57

If we want to use a number seven, we can say that it's equal to .201.

04:02

And this brings up a number 7 drill.

04:05

Once again, we'll copy and paste it into our cam DFM library, again, we'll have to clear the filters to see everything that's in here.

04:14

Our number seven drill, we're not going to make too many modifications, but we do want to adjust the number two tool 2.

04:21

We can also modify cutting parameters and give it to flutes.

04:26

We're going to accept this change and then go back into our fusion 360 library.

04:30

Now we want to look for a tap when we take a look at this and we go to whole making, you can see that we have tap, left hand and tap right hand.

04:39

We're going to select the right hand tap and we want to find a quarter 20.

04:43

Well scroll down a little bit until we see a quarter

04:46

We will copy the tool and then we'll go back into our key M V F M and paste it.

04:52

We're going to edit this tool in its post processor number and this is going to be tool number 3 in our library.

04:58

Will accept the change.

05:00

Again, we'll clear those filters and make sure that we have tools 1, 2 and 3.

05:04

Then we'll go back to our fusion 360 library.

05:07

Now we want to find a flat end mill which will be in the milling section and we'll filter by flat end mill.

05:13

In the sample tools inch section, we're going to be looking for an eighth inch flat end mill.

05:19

We're also going to do this for a quarter inch and a half inch. But we're going to do these one at a time.

05:25

I'm going to copy of the tool and paste it into my library and then I'm going to go back,

05:30

grab the quarter inch and we'll do the same thing for the half inch.

05:41

Now I can modify their parameters and set their tool numbers, in the post processor section are eighth inch is going to be tool number 4.

05:51

A quarter inch is going to be tool number 5.

05:60

And then our half inch is going to be tool number

06:09

Then we'll go into our filters and let's go ahead and clear all the filters to see what tools we have.

06:14

Right now, we have tools one through six, a spot drill a number seven, drill a quarter, 20 tap an eighth, a quarter and a half inch flat end mill.

06:22

Now that we have these in here, we can go ahead and modify some of their parameters.

06:26

We're going to right click and edit the tool and go to cutting data.

06:30

Inside of here on the left hand side, notice that there are various parameters based on what you're doing with the tool.

06:37

If we go down to a low carbon steel or brass, you can see that it changes the feed rates.

06:43

We're going to be using the quarter inch an eighth inch for finishing operations.

06:47

So we want to make sure that we take a look at the aluminum finishing.

06:51

Right now, it's spinning at about 12,000 rpm and we're actually going to reduce this to 10,000 rpm.

06:58

When I do that, it automatically changes some of the other values. And we're going to go down until we find the feed per tooth.

07:04

We're going to change this 2.002.

07:08

When we do that, it changes the cutting feed, right. Because it's based on those parameters.

07:13

We're going to accept those changes and we'll take a look at the quarter inch next.

07:18

We're going to go to cutting data and once again, we want to take a look at aluminum finishing.

07:23

Inside of here, we're also going to change this to

07:27

We're going to take a look at some of the other parameters.

07:31

In this case we were looking at a feed per tooth of values for lead in and lead out.

07:41

You notice that these values are rounded right now, I'm going to set them to 120.

07:48

And for the ramp feed rate, I'll do that at 120 as well.

07:52

We can also modify values for things like the plunge feed rate.

07:56

In this case, plunge, we're going to set to 30 and then we've got passes and links and these other values that we're using here,

08:04

we can also modify various parameters for the tool itself.

08:08

For example, if we want to increase it to four flutes and change how far it's sticking out of the holder.

08:14

We can always come back and modify these later on as we're using them.

08:18

Last, let's make some adjustments to the half inch in milk.

08:21

Under the cutting data, we're going to go into aluminum roughing, since this is going to be a roughing tool.

08:27

We're going to modify to make sure that we're using

08:32

And we want to take a look at the FPT or feed per tooth.

08:36

Right now it's set 2.005 and we're going to adjust this 2.008.

08:42

Everything else I'm going to leave as is but I do want to modify the cutter and note that it is a four flute and accept the changes.

08:52

There are a few more tools that we need. So we'll go back into our filters for milling.

08:56

We're gonna look for a ball end mill and this is going to be a quarter inch ball in mill.

09:02

Once again, we'll copy the tool. Go into our cam library and we'll paste it.

09:08

We'll modify its parameters after we find the rest of our tools.

09:11

Now we're going to be looking for a face mill.

09:14

We're gonna take the 2 inch face male sample.

09:17

We're going to copy this tool and we're going to paste it into our cam DFM library.

09:22

Last thing that we need is a chance for mill and this is something that we're going to have to make custom.

09:27

So inside of here let's first modify our tools.

09:31

The ball in mill that I grabbed. I actually want to be a bull nose mill.

09:35

So if I edit the tool I can go into the cutter section and I can actually change its profile and make it a bull nose milk.

09:42

I then need to make sure that I modify its parameters.

09:45

This is going to be four flute,

09:47

it's going to be quarter inch diameter but the radius value for the corner is actually going to be quite a bit smaller.

09:54

We're going to get rid of all the decimals that are in here and we're going to set up the corner at

09:59

This will allow us to create a small, fill it on the bottom of any of the features that we machine with this tool.

10:06

This is also going to be tool number seven.

10:10

We do want to go into the general and we want to change the description since we did change it to a bull nose.

10:17

So I'm going to change it to a bull nose end mill and I'm going to put a note about the corner radius

10:24

That way when we're looking at this in our tool library, we know exactly what value it is.

10:29

At any time, it's showing up in our tool library like this, it's missing some required data.

10:36

When we take a look, we go through everything looks okay in here.

10:42

But in the cutting data sometimes you'll note that it might be missing some information.

10:46

You'll note here that an aluminum roughing and finishing, it's missing some of the data. It's not specified.

10:53

I'm going to turn these options off,

10:55

which means that I'm going to be using the values that are inside of my tool path and not using the ones from the tool library itself.

11:04

It still says that it's missing some data but that's okay, because we're only going to be using it for some of the cutting data, not all of it.

11:11

We're going to be focusing on the aluminum values for roughing and finishing.

11:16

Lastly we're going to change the tool number for our face mill before we get in and we start creating our champ for mill.

11:23

The face Smell is going to be tool number eight and we're going to accept that change.

11:28

In order to create a new tool, we need to hit the plus icon and determine what tool we want to create.

11:35

In this case, we're going to be looking at creating a champ for mill which is under engrave slash chamfer.

11:41

We're going to go to our cutter section and we want to define this as 45°.

11:47

I'm going to change the number of flutes to we're going to be using the inches and high speed steel for material.

11:54

And then down in the diameter, we're going to set this at a .25 diameter.

12:01

The shaft diameter is also going to be .25.

12:04

Then we need to define the other values in our case, the inclusive angle is 90. The taper angle is 45.

12:12

All that will be fine and we need to make the tip diameter a little bit larger.

12:17

Right now it's set to zero, which means it can be used as an engraved tool.

12:21

But we're going to set it at .125 When we do that, it gives us a flat section at the bottom and it gives us the chance for on the side.

12:30

Everything else is going to be fine in here.

12:32

I'm going to reset this to tool number nine.

12:35

Then we're going to accept it noting that we can come back and make adjustments to these at any point in time.

12:42

Everything looks pretty good. And since this is a cloud library, I don't need to make any saves.

12:47

The document is unsaved because we change the units but that doesn't really have any effect on a tool library.

12:54

We can always come back in, go to our tool library and make any additional adjustments needed.

12:59

From here, make sure that you have played around with all the different various parameters and settings and search this tool library,

13:05

and then we can move on to the next step.