Tool library setup

00:02

In this lesson, we'll go through the process to set up our tool library.

00:07

After completing this lesson, you'll be able to Import a tool library, modify tool parameters and use Form Mill.

00:16

In Fusion 360, we want to carry on with our spline coupler.

00:19

If you had any issues, you can upload the supply dataset spline coupler dovetail.

00:25

That data set won't include the UMC-750 table, but it will have all the information you need to follow this lesson and create a dovetail cutter.

00:33

We're going to start by expanding our bodies folder showing our stock in hiding our part.

00:39

We want to create a new sketch, and this is going to be on the YZ plane.

00:44

And we're going to use Create, Project Include and Intersect.

00:50

For our selection, we're going to use selected entities, and we want to select the faces of interest.

00:55

In this case, it's going to be this taper, and this short section here.

01:01

We'll say 'okay', and navigate back to a right hand view.

01:04

Using our line tool, we will begin designing our cutter.

01:08

We're going to come out to the left, come up.

01:12

We're going to come over to this point,

01:15

and then we use our constraints to make sure that this edge is vertical.

01:20

Using our sketch dimension tool, we will start by selecting the axis of revolution and then the endpoint that will be inside of that dovetail.

01:28

We'll right click and turn this into a diameter dimension.

01:32

We're going to make this a half inch diameter tool, and we're going to give it an overall length of 2".

01:40

Once we've got this profile, we can finish the sketch.

01:43

We want to expand our sketches folder, and we're going to rename sketch8 to be our dovetail.

01:49

I also want to note that inside of the user preferences, you want to make sure that you have cloud libraries enabled.

01:55

This will be in the general manufacturer section, and you can enable cloud libraries here.

02:01

Now we're going to navigate to the manufacturer workspace, and we want to begin by going into our tool library.

02:10

If there are any tools in the current document,

02:13

inside of here, you'll notice that there are some tools we can right click and we can remove unused tools.

02:20

This will clear out any tools that were saved in the design.

02:24

Now in the case of using distributed design,

02:26

if you brought in additional functionalities such as a fixture or a table that were part of another design, they might contain data.

02:35

So this is why it's always important that you check some of these before you get to programming,

02:39

to make sure that you don't have extra tools in here that don't match the specific library.

02:44

Now in the cloud section, I'm going to right click, and I'm going to import.

02:49

I want to navigate to the location of my multi-access tools and select open.

02:54

Now we've brought in 11 tools including spot drill and drill bits, taps, flat end mills, ball end mills, a taper mill as well as a chamfer mill.

03:04

The one thing we're missing is a dovetail cutter, and we're going to do this by going to manage and selecting form mill.

03:13

We'll begin by noting the coordinate system here.

03:16

Z is pointing up and when we select our profile and we select our tool axis, you'll notice that we get a red arrow on the screen.

03:26

The red arrow on the screen is pointing up toward the machine.

03:29

However, we need to flip our tool over.

03:32

For the compensation point, I want to select the point on the outside edge of my dovetail.

03:37

I'm going to say 'okay', and then I want to go into my tool library and check on that form mill.

03:43

You'll notice here that the form mill is created upside down.

03:47

It's created based on the coordinate system of our design, and the orientation when we created it.

03:54

Let's go ahead and try creating it one more time.

03:57

We will select form mill, will select our axis of evolution and instead of flipping the axis, we're going to leave the arrow pointing up,

04:06

and we're going to say 'okay' and check the tool library.

04:10

So now we have two different form mills in two different orientations.

04:14

This is going to be important because again it's referenced based on the Z up coordinate system.

04:21

So if we have to flip it over, you just need to make sure that you use that flip option.

04:27

I'm going to delete the upside down tool.

04:32

And then for my form mill tool, I'm going to double click to edit.

04:35

I'm going to start by going to the post processor, and we'll make this tool number 12.

04:40

Then you'll note in the cutting data section that all of the information is empty.

04:44

In this course, we're not actually going to be using this to cut our geometry,

04:49

but it's important to understand the process any time you need to make a custom tool.

04:54

So if we want to add specific information, for example, if this tool is going to be at 5000 rpm, the ramp spindle speed will also be at 5000 rpm.

05:05

We will just simply need to go down the line and enter all the data that we want to use for this cutter.

05:10

I'm going to run it at 20 inches per minute and notice that it populates most of the other values. For my ramp,

05:17

I'm going to run that a little bit slower, and then I have this data in here for plunge feed rates.

05:23

I'm not going to be plunging with this tool but it is still asking for this data, so I'm going to go ahead and enter it,

05:29

and I'll allow flood coolant to be turned on any time this tool is used.

05:34

So again, we can double check all the information we have.

05:38

We can enter data such as the number of flutes we have, the material if it's specified.

05:43

And then any additional information that we might want to change.

05:47

For example, the diameter, at this time it's .5 based on our sketch.

05:52

If we try to increase this, notice that nothing changes in the preview.

05:57

So in general, you want to make sure that you leave this data based on your sketch profile, but it does allow you to come in and make modifications.

06:07

It's also important that we add a description.

06:11

I'm simply going to call this a dovetail cutter but in reality, you would necessarily have a vendor or a product ID.

06:17

And if you're getting a custom tool made, then you would want to put that information in there as well.

06:23

Now that we have our dovetail cutter, I'm going to right click and copy the tool, then I'm going to go to my multi-axis tools, cloud library.

06:31

I'm going to right click and paste it there.

06:33

So that way it's included in that library.

06:35

Even if I use it in another design.

06:38

From here, I want to make sure that I select 'closed'.

06:41

I'm going to expand my models, and I'm going to hide that sketch because it's no longer needed.

06:47

I also want to show my part as well as my table and all the fixed during that I created and go back to a Home view.

06:55

At this point, let's make sure that we save the design before moving onto the next step.