CAM Assist faces the stock, roughs out the bulk of the material with constant-engagement (adaptive) roughing, then finishes each face with the operation type that suits it: wall, flat, freeform, chamfer or T-slot. Holemaking and deburring complete the program. This article explains each stage and the settings that change it.
The stages at a glance
| Stage | What it does | Program stage section |
|---|---|---|
| Facing | Machines the top of the stock flat, usually with a face mill. | Facing |
| Roughing | Removes the bulk of the material, leaving stock for finishing. | Roughing |
| Finishing | Cuts each face to size and surface finish. | Wall, Flat, Freeform, Chamfer |
| Holemaking | Spot drills, drills, bores, reams, taps and thread mills holes. | Holemaking |
| Deburring | Breaks sharp edges. | Deburring |
You choose which of these CAM Assist generates in the Setups stage, under Toolpath Types. See Set up your setups. To see how each one appears in your CAM package, see Which operations and setups does CAM Assist create in my CAM package?
Facing
Facing operations machine the top faces of the part flat, usually with a face mill. In the Program stage they appear as Facing. CAM Assist leaves out face mills whose cutting force would be too high for the setup's Workholding security. See What is workholding security in CAM Assist?
Roughing
What is adaptive roughing?
Adaptive roughing (also called adaptive clearing, constant-engagement roughing, high-efficiency roughing or dynamic milling) keeps the load on the cutter roughly constant. Instead of plunging into corners at full width, the toolpath uses smooth, often trochoidal moves that limit how much of the tool is engaged.
Why CAM Assist uses it:
- Deeper cuts at higher feeds: with a light, steady width of cut, the tool can usually take most of its flute length in one step down.
- Longer tool life: no sudden spikes in load when the tool enters a corner.
- Less chatter and heat, which helps in tough materials.
In the Program stage these operations are called Adaptive roughing. In your CAM package they become that package's adaptive or dynamic roughing toolpath, such as Adaptive Clearing in Autodesk Fusion or Dynamic OptiRough in Mastercam.
What is pocket roughing?
Where a tool has to cut full width, for example in a narrow slot, CAM Assist uses a slotting or pocketing strategy instead. These operations appear in the Program stage as Pocket roughing.
How does CAM Assist choose roughing tools?
CAM Assist can use more than one roughing tool. It weighs the suitable tools in your libraries and picks the combination it expects to machine the part fastest, allowing for both cutting time and tool changes. Often a larger tool clears most of the material before smaller tools reach into tighter areas, but the sequence adapts to each part. It won't use a tool and approach whose estimated sideways cutting force is above the setup's Workholding security limit.
To stop an operation roughing an area, use Change volume boundaries. See Change roughing boundaries.
Why does roughing leave stock?
Roughing leaves a layer of material for finishing to remove: Axial stock to leave on floors and Radial stock to leave on walls. Both must be greater than zero.
| Stock left | Effect |
|---|---|
| Too little | Finishing may not clean up the surface, because roughing tools deflect and leave an uneven surface. |
| Too much | The finishing tool takes a heavy cut, which can cause deflection, a poor finish and an out-of-tolerance size. It also adds finishing time. |
Set them on the Roughing tab of the part's configuration: click Configuration in the header of the Setups, Feature planning or Tools stage. See Configuration settings.
Finishing
CAM Assist assigns each face of the part to a finishing operation. The operation type depends on the face's shape:
| Finishing type | Used for | Typical tool |
|---|---|---|
| Wall | Vertical and steep side walls. | End mill, or a ball mill allowed Wall finishing |
| Flat | Horizontal floors and flat faces. | End mill or ball mill |
| Freeform (Contour, Scallop, Blend, Generic) | Curved 3D surfaces. | Ball mill or end mill |
| Chamfer | Modeled chamfers on edges. | Chamfer mill |
| T-Slot | Undercut walls and slots that can't be reached from above. Needs Undercuts ticked under Toolpath Types in the Setups stage, and undercut tools in your libraries. | T-slot cutter |
You can change a finishing operation's type, tool, setup, tool axis and faces after the run. See Edit an operation.
Freeform finishing
CAM Assist doesn't use a single pattern for every 3D surface. For each group of freeform faces it chooses one of these operation types:
| Freeform type | What it does |
|---|---|
| Contour freeform | Constant-Z passes. Suits steep surfaces. |
| Scallop freeform | Passes at a constant stepover across the surface. Suits shallow surfaces. |
| Blend freeform | Passes that blend between the edges of a surface. Used for fillets and similar features. |
| Generic freeform | Uses the freeform finishing type set for your CAM package (below). |
CAM package finishing options
Some CAM packages add their own settings to the part's configuration, at the bottom of its Finishing tab (roughing options on the Roughing tab). They choose which of the CAM package's toolpaths CAM Assist uses.
Autodesk Fusion: Extra Finishing options > Freeform operations sets the toolpath for generic freeform operations.
| Option | What it does |
|---|---|
| Contour3D (default) | Always uses Contour toolpaths. |
| Contour3D/Scallop | Contour on steep areas, Scallop on shallow areas. |
| Contour3D/Parallel | Contour on steep areas, Parallel on shallow areas. |
| Steep and Shallow | Always uses Steep and Shallow toolpaths. Needs Fusion's Machining Extension. |
Mastercam:
| Setting | Option | What it does |
|---|---|---|
| Flat operations | 2D Area mill (default) | Uses a 2D Area Mill toolpath where it can, otherwise Horizontal. |
| Horizontal | Uses the 3D Horizontal Area toolpath. | |
| Freeform operations | Waterline (default) | Finishes freeform surfaces with Waterline toolpaths. |
| Hybrid | Finishes freeform surfaces with Hybrid toolpaths, which combine waterline passes on steep areas with scallop passes on shallow areas. |
Siemens NX: Flat operations > Cut pattern sets Follow Periphery (default) or Follow Part. See What does CAM Assist add to my Siemens NX part?
GibbsCAM: the Process preference group sets the Freeform process (Contour, Adv3D or Surface) and flat options, and Roughing Type chooses Volumill or Standard Roughing. See GibbsCAM process preference settings.
Internal corners
Two settings on the configuration's Finishing tab control how CAM Assist finishes internal corners:
- Maximum internal corner radius: the largest internal corner radius CAM Assist tries to finish with a ball-end or corner-radius tool.
- Allow equal tool and feature radii in vertical corners (Enabled or Disabled): lets CAM Assist finish an internal corner with a tool whose radius matches the corner. With it off, CAM Assist uses a tool smaller than the corner, which can mean an extra tool and a longer cycle time. With it on, the tool choices you see when you edit a wall operation can also be wider.
Finishing operation order
Finishing operation order on the configuration's Finishing tab sets the order of the finishing operations:
| Option | What it does | Choose it when |
|---|---|---|
| Group by operation type | Groups operations of the same type together, for example all wall finishing, then all flat finishing. | You want a program that's easy to read and edit. |
| Minimize tool changes | Keeps each tool's operations together. | Tool changes are slow on your machine, or you want to avoid the witness marks a tool can leave when it comes back to a face. |
When one tool can't finish a face
CAM Assist adds a - Partial operation and a - Rest operation that cleans up what the first tool left. See What are Rest and Partial finishing operations?
Holemaking
CAM Assist matches each hole to the tools in your libraries and builds the sequence: spot drilling, drilling, boring (including helical boring with an end mill), reaming, and tapping or thread milling for threaded holes. See Hole element settings: bottom, bore, thread, pilot and spot drilling and CAM Assist didn't drill, tap or ream a hole.
Deburring
Deburring breaks the part's sharp edges. Deburring tool on the configuration's Finishing tab chooses a Ball mill (rounded edge break) or a Chamfering tool (angled chamfer). See Configuration settings.
What this means for you
- You don't pick toolpath patterns face by face: CAM Assist chooses them. Change the result afterwards with Edit an operation, or in your CAM package.
- Settings that change the result: stock to leave, corner settings, finishing operation order, deburring tool and your CAM package's finishing options.
- Faces CAM Assist can't finish are left for you. See Why didn't CAM Assist finish some faces?