Overview#
Every operation needs a tool. In Fusion, a tool is a data record that carries geometry (diameter, flute length, shaft, holder), identity (number, description, vendor, product ID) and cutting data (spindle speed, feed rates) so the toolpath and simulation can be generated correctly. Tools live in tool libraries, which you can think of as files that can be stored locally, in the cloud, or on a network share.
Getting tools right pays off three ways:
- Accurate toolpaths: strategies use flute length, shank diameter and corner radius to avoid gouges and to decide stepdown limits.
- Safe simulation: the holder and shaft shapes let Simulate detect collisions that a bare cutter model would miss.
- Faster programming: a tuned tool with saved presets means you pick it, and speeds and feeds fill in.
Fusion tools also carry a tool number that becomes the T-number in G-code, and offsets (length/diameter) that connect to the controller's tool table. Mismatch between Fusion's tool numbers and the machine's physical tool changer is a common source of crashes.
Where to find it#
- Manage > Tool Library on the Manufacture toolbar (available on any tab).
- Inside an operation, the Tool tab has a Select button that opens the same library browser.
- In the Tool Library, right-click a tool and choose Edit tool.
The Tool Library dialog has a left panel of libraries and a panel of tools; import and export are on the library right-click menu.
Library locations#
| Location | What it is | Notes |
|---|---|---|
| Documents | Tools saved in the active document | A default library is created automatically; tools you select from other libraries are copied here and can be modified |
| Hub Libraries | Tools stored in the cloud, available to members of your Fusion hub | Replacing the Cloud library; Autodesk notes it is rolling out to a portion of customers |
| Cloud | Tools stored in the cloud, accessible from any device | If not visible, enable Preferences > General > Manufacture > Enable Cloud Libraries |
| Local | Tools stored on your device | Editable; not shared |
| Fusion Library | Read-only tools from Autodesk, organised by process and by units (for example Holders (Inch), Holders (Metric)) | Selecting a tool copies it to the document |
| Vendor | Read-only tools from online tooling manufacturers | Rolling out gradually; otherwise use Download Vendor Libraries and import |
Selecting a tool from any library copies it into the active document. The key habit is the same: keep your master tools in a library you control (Local or Cloud), and copy them into the document by using them.
Tip: Selecting a library tool copies it into the document's Documents library, so editing the library tool does not change tools already used in a document. To change a document tool, edit it in the Documents library or select it again from the source library.
Tool types#
The New Tool dialog starts with a type. Typical choices:
- Milling: ball end mill, bull nose end mill, flat end mill, face mill, tapered mill, radius mill, engrave/chamfer mill, dovetail mill, lollipop mill, slot mill, thread mill, and circle segment barrel, lens, oval and taper mills (form mills are covered in their own help topic).
- Hole making: boring bar, counter bore, drill, center drill, spot drill, reamer, counter sink, tap left hand, tap right hand.
- Turning: turning general, turning boring, turning grooving, turning threading.
- Cutting: waterjet, laser cutter, plasma cutter.
- Probes: probe.
- Holders: holder.
- Depositing: electric arc wire, laser powder, laser wire.
Choose the closest type; geometry fields and available strategies follow from it. A flat end mill can run adaptive, offset roughing and contour passes; a bull nose does the same with a corner radius; a face mill is intended for Face operations.
Tool dialog tabs#
For a milling or hole-making tool the editor has these tabs: General, Cutter, Shaft, Holder, Cutting data and Post processor.
General#
- Description: a human-readable name ("12 mm 3FL carbide endmill").
- Vendor, Product id, Product Link: identify where to buy the tool; the link appears on the library Info tab.
The tool number, offsets, turret, comment, manual tool change, live tool and break control live on the Post processor tab (below); Unit and Material are on the Cutter tab; Coolant is on the Cutting data tab.
Cutter#
Geometry that defines the cutting end:
| Parameter | Meaning |
|---|---|
| Type | Changes the form of the tool (ball, flat, bullnose, tapered and so on) |
| Unit | Millimeters or Inches |
| Clockwise spindle rotation | On for right-handed tools; off for left-handed tools (CCW) |
| Number of flutes | Cutting edges ("teeth") |
| Material | Unspecified, HSS, Ti Coated, Carbide or Ceramic |
| Diameter | Cutting diameter |
| Shaft diameter | Diameter of the clamping surface |
| Overall length | Length of the entire tool |
| Length below holder | Length protruding from the holder |
| Shoulder length | Length above the cutting edge |
| Flute length | Length of the cutting edge |
| Corner radius | Radius on the cutter corner |
| Tip angle, tip diameter, tip length | Chamfer, spot drill, engrave and center drill tools |
| Taper angle, included angle | Included angle is twice the taper angle |
| Thread pitch, number of teeth, thread profile angle | Taps and thread mills |
Real dimensions matter. If you enter a flute length longer than the real one, a stepdown can exceed what the tool can do. If you enter length below holder shorter than reality, Simulate understates reach and misses collisions, and might choose too short a tool reach.
Holder#
Holders are not required, but give a visual reference and are used for collision detection. Pick one from the holder list on the left of the Holder tab (use Search to filter). A Shaft tab lets you add segments (height, upper and lower diameter) between the tool and the holder.
Post Process#
Parameters passed to the post processor:
- Number: the tool number in the NC program.
- Length offset and Diameter offset (the latter for cutter radius compensation).
- Turret position, Comment (typically output to the NC program), Manual tool change, Live Tool (spinning tool on a lathe) and Break control (machine-dependent breakage check).
Cutting data (Feed & Speed)#
This tab contains:
- Speed group: Spindle speed (rpm), Surface speed (ft/min for inch tools, m/min for metric) and Ramp spindle speed.
- Feedrates group: Cutting feedrate, Feed per tooth, Lead-in feedrate, Lead-out feedrate, Ramp feedrate.
- Vertical feedrates group: Plunge feedrate and Feed per revolution.
- Passes and linking group: Use stepdown, Use stepover, Coolant.
A single tool can hold multiple presets (Add preset on the Cutting data tab; presets can be renamed, sorted, and copied to other tools of the same type) (for example: "Aluminum roughing", "Steel finishing") so one physical tool covers several materials. Each operation can choose which preset to use. Details are on the feeds-and-speeds page.
Step by step: create a tool#
- Open Manage > Tool Library.
- In the left panel, select your destination library (Local or Cloud, or Documents).
- Create a new tool and pick Flat end mill (use the library's new-tool command; the exact button is not described in the topics checked).
- On General: Description "10 mm 3FL carbide flat". On Post processor: Number 1, offsets 1.
- On Cutter: Diameter 10, Number of flutes 3, Overall length 72, Length below holder 35, Flute length 22, Shaft diameter 10 (example values).
- On Holder: select a holder that matches your machine.
- On Cutting data: add a preset for Aluminum. Enter surface speed or spindle speed, and fz. Fusion fills in the dependent fields.
- Click Accept.
- Close the library. In an operation, click Select on the Tool tab and choose the new tool.
Using tools in operations#
On an operation's Tool tab, Select opens the library. After selecting, the operation shows Preset (if the tool has any), Spindle speed, Cutting feedrate and related fields. You can override these on the operation without altering the library tool. Overrides are saved only in that operation.
Note: not confirmed in Autodesk's documentation: how Fusion treats operations that share a tool number but have edited tool copies. Keep tool numbers unique per distinct tool.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Library location | Documents, Hub, Cloud, Local, Fusion Library, Vendor | Hub/Cloud for sharing; Local for your device |
| Tool type | Selects geometry model | Flat, ball, bull nose, drill, tap, etc. |
| Number (T) | Tool number in the NC program (Post processor tab) | Keep unique per distinct tool |
| Diameter / Length offset | Offset numbers in the NC program | Often set to the tool number (general practice) |
| Diameter | Cutting diameter | Used for toolpath calculation |
| Number of flutes | Flute count | Needed for feed per tooth |
| Flute length | Max cutting depth reach | Strategies limit stepdown to this |
| Length below holder | Stick-out | Affects collision and reach |
| Holder | Holder profile or library holder | Needed for realistic simulation |
| Preset | Saved speed/feed set | Select per operation |
| Coolant | Tool coolant type | Not all options exist for all machines |
| Unit | Inch or mm | Cutter tab |
Tool management practices#
- One library per machine or per tool crib. If your machine has a 20-pocket changer, build a library that mirrors it, with tool numbers equal to pocket numbers. Operations then post T-numbers matching reality.
- Name consistently: size, type, flutes, material, coating. "6 mm 3FL ALU polished" beats "tool 4".
- Duplicate for variants: a roughing preset and a finishing preset on the same tool is better than two near-identical tools, unless they are physically different tools with different stick-out.
- Back up: right-click a library and choose Export library. Export formats are Fusion Tool Library (.tools, .json), HSM Tool Library (.hsmlib) and CSV (expressions are not exported to CSV).
- Import: right-click a Local or Cloud library and choose Import Tools or Import Libraries. Accepted: .tools/.json, .hsmlib, .csv, Generic Tool Catalog (GTC) packages (.zip) and P21 files (.p21).
- Vendor tools: use the Vendor libraries if available, or Download Vendor Libraries to fetch read-only tool data from the Tools for Autodesk Fusion website and import it.
Tips and pitfalls#
Tip: Model the holder and stick-out honestly. A common "crash in simulation" that is really a "crash in reality" is a holder body hitting a vertical wall because you used a short stick-out in the tool but a long one on the machine.
Tip: Keep tool numbers unique per distinct tool in a document and check them before posting.
Warning: Editing a library tool does not update copies already stored in existing documents.
Warning: Unit mismatch. Values you type into a metric tool as "0.25" mean 0.25 mm. Always check the tool Unit on the Cutter tab.
Warning: Do not trust vendor-supplied speeds blindly. Presets are starting points. Machine rigidity, spindle power, and workholding determine what is practical.
Practice exercise#
Create a Local library named "Shop Basics" (or use Documents if Local is unavailable) with these tools: a 10 mm 3-flute flat end mill (T1), a 6 mm ball end mill (T2), a 6 mm drill (T3) and a 90 degree 12 mm chamfer mill (T4). Give each a holder, flute length and stick-out. Add an "Aluminum" preset on T1 with surface speed 250 m/min and fz 0.06 mm.
Then, in a Setup, create a 2D Offset Roughing operation that uses T1 and confirm that the operation's spindle speed and feedrate reflect the preset (spindle speed approximately 7,958 rpm from 250 m/min on a 10 mm tool, with feedrate approximately 1,432 mm/min for 3 flutes at 0.06 mm/tooth).
Related#
- Feeds and speeds: tuning the cutting data tab
- Drilling: drill and tap tool types in use
- Turning: lathe tool and holder specifics
- Setups and stock: choosing tools after defining the Setup