Managing tool libraries

00:09

To access the Tool Library, on the Toolbar, from the Workspace Picker, select Manufacture.

00:17

On the Milling tab, in the Manage panel, expand the Manage drop-down and click Tool Library.

00:25

The Tool Library dialog appears.

00:28

From here, you can view the list of libraries available.

00:33

The Tool Library comes preloaded with the Fusion 360 Library that includes sample tools.

00:40

You can also access any local tool libraries created for your specific machine.

00:47

Fusion also offers Cloud libraries for custom libraries available from the cloud, for use on any device.

00:56

This is useful for teams or for individuals who need to access tools on the go.

01:03

To set up a Cloud library, close the Tool Library dialog.

01:08

Then, from the Application Bar, expand the Profile drop-down.

01:14

Select Preferences.

01:16

The Preferences dialog displays.

01:20

From the list, under General, select Manufacture.

01:25

Then, enable the checkbox next to Enable Cloud Libraries.

01:31

Next, click Apply, and then OK.

01:35

Now, from the Toolbar, in the Manage panel, select Tool Library.

01:42

The Tool Library dialog displays.

01:45

Notice that now, the Cloud library displays in the list of available libraries.

01:52

Click Cloud, and the dialog updates to list the available tools associated with the Cloud account.

01:59

To create a new Cloud library, back in the library list, right-click Cloud, and from the shortcut menu, select New Library.

02:11

A text field displays.

02:14

Enter a name for the library, such as, “Turning”.

02:19

On your keyboard, press ENTER to confirm.

02:23

Now, you can create a tool for the Cloud library.

02:28

From the Toolbar, select New tool.

02:31

The New tool dialog displays, listing available tools for creation.

02:37

Under Turning, select Turning general.

02:42

Back in the Tool Library dialog, the details for the new tool display.

02:48

In the General tab, in the Description field, enter, “CNMT Right Hand”.

02:58

From here, you can also update the tool’s vendor, product ID, and product link.

03:06

Next, open the Insert tab.

03:10

Expand the Unit drop-down and select Millimeters.

03:16

From this tab, you can also specify several other options for the insert tool.

03:22

Notice that the ISO code is currently blank.

03:27

Review the shape, relief angle, tolerance, and cross-section.

03:34

Expand the Insert Size drop-down and select 09.

03:40

Next, expand the Thickness drop-down and select T3.

03:47

Finally, expand the Corner radius drop-down and select 08.

03:54

Once configured, notice that the ISO code updates.

03:59

If you already have an ISO code, you can type it in this field, and the settings change accordingly.

04:06

Now, open the Holder tab.

04:10

Here, you can change the settings for the unit, style, hand, and clamping.

04:18

In the Geometry group, in the Cutting width field, enter, “25”.

04:25

The tool preview updates based on the data entered.

04:30

Next, in the Head length field, enter, “32”.

04:36

In the Overall length field, enter, “125”.

04:41

For both Shank width and Shank height, enter, “20”.

04:48

Open the Setup tab.

04:51

Under Orientation in Turret, use the arrows to set the orientation of the tool, or the angle of the tool with respect to the cutting direction.

05:01

In this example, it is set to 0 degrees.

05:06

Under Compensation, you can specify the toolpath compensation position.

05:13

This should be set based on how you reference your tools at the machine.

05:18

Leave this set to Tip Tangent, which measures from each cutting edge, square to the axes.

05:26

Finally, under Spindle Rotation, you can specify the direction of spindle rotation.

05:33

Ensure Clockwise spindle rotation is enabled.

05:38

Open the Cutting data tab.

05:41

Here, you can set default speeds and feeds for the tool.

05:46

Under Feedrates, you can adjust various feedrates.

05:51

Under Speed, you can determine to use a constant surface speed,

05:56

which speeds the spindle up as it gets closer to the center of the stock.

06:01

Finally, open the Post processor tab.

06:05

In the Number field, enter the number you wish to associate with the tool, such as, “4”.

06:13

Then, click within the Compensation offset field.

06:18

The field updates with the tool number and uses a formula to determine the tool length offset

06:25

and tool diameter offset in the NC program.

06:29

Once the tool is configured, click Accept.

06:33

In the Cloud Turning library, tool 4 displays along with a preview and parameters.

06:42

Managing and creating tools and tool libraries is a highly customizable process.