CAM Assist plans the program in its own terms (facing, roughing, wall finishing, drilling and so on). When you click Send to CAM package, each operation becomes one of your CAM package's own toolpaths, in your own setups. This article lists what each CAM Assist operation and setup item becomes in Autodesk Fusion, Mastercam, Siemens NX and GibbsCAM, and how SolidCAM differs.
How the mapping works
- CAM Assist reads your setups, part, stock and workholding from your CAM package.
- It plans an abstract strategy: which tool removes which volume, finishes which faces, or makes which hole.
- When you send the program, your CAM package creates a standard toolpath for each operation, with CAM Assist's tool, faces or boundaries, and cutting parameters filled in.
The result is ordinary operations you can edit, simulate and post like any others. CAM Assist only uses some of each CAM package's toolpath types. If you'd rather use a different one, change the operation's type in your CAM package after sending.
Some choices are yours: your CAM package's finishing options on the Finishing tab of the part's configuration, and the operation type when you edit an operation. See How does CAM Assist rough and finish a part?
Setups, part, stock and workholding
| CAM Assist | Autodesk Fusion | Mastercam | Siemens NX | GibbsCAM |
|---|---|---|---|---|
| Setup | Setup | Machine group | WORKPIECE geometry group under an MCS | Coordinate system with bodies on it |
| Part | The setup's Model | Master Model (Job Setup) | Part (Specify Part) | Part body |
| Stock | The setup's Stock | Stock (stock setup) | Blank | Stock body, or the stock box in Document Control |
| Workholding | The setup's Fixture | Fixture (Job Setup) | Check geometry | Fixture body |
| Avoidance geometry | Chosen in CAM Assist | Chosen in CAM Assist | Chosen in CAM Assist | Chosen in CAM Assist |
For how each CAM package sets these up, and what to do when CAM Assist doesn't find them:
- Autodesk Fusion: What does CAM Assist change in my Autodesk Fusion document?
- Mastercam: CAM Assist won't start in Mastercam: machine group, stock or Master Model errors
- Siemens NX: CAM Assist doesn't find my setups or stock in Siemens NX
- GibbsCAM: Prepare a GibbsCAM part for CAM Assist
- SolidCAM: How do I get CAM Assist in SolidCAM?
To choose bodies in CAM Assist, see Select avoidance geometry and workholding.
Operations
The names below are each CAM package's toolpath types.
| CAM Assist operation | Autodesk Fusion | Mastercam | Siemens NX | GibbsCAM |
|---|---|---|---|---|
| Facing | Face | Facing | Floor Facing | Pocket (facing) |
| Adaptive roughing | Adaptive Clearing | Dynamic OptiRough | 3D Adaptive Roughing | Volumill, or Standard Roughing (Roughing Type setting) |
| Pocket roughing (slots) | Pocket Clearing | Dynamic OptiRough | Cavity Mill | Contour or standard pocket roughing |
| Flat finishing | Flat | 2D Area Mill or Horizontal Area (Flat operations setting) | Floor Facing | |
| Wall finishing | 2D Contour; Contour for 3D walls | Contour | Planar Profiling; Wall Profiling for 3D walls | Contour |
| Freeform finishing | Contour, Scallop, Parallel, Steep and Shallow or Blend | Waterline or Hybrid (Freeform operations setting), or Scallop | Area Mill; Streamline for blend surfaces | Contour, Adv3D or Surface (Freeform setting) |
| Chamfer finishing | 2D Chamfer | Model Chamfer | Planar Profiling | Contour |
| Undercuts (T-slot) | 2D Contour | Contour | Planar Mill | Contour |
| Deburring | 2D Chamfer (chamfer mill) or 2D Contour (ball mill) | Model Chamfer (chamfer mill) or Contour (ball mill) | 3 Axis Deburring | Contour |
| Spot drilling, drilling, reaming, tapping | Drill | Drill | Spot Drilling or Drilling | Drill |
| Helical boring | Bore | Helix Bore | Hole Milling | Drill (helix bore) |
| Thread milling | Thread | Thread Mill | Thread Milling | Thread mill |
Notes by CAM package:
- Autodesk Fusion: Freeform operations on the configuration's Finishing tab chooses the toolpath for generic freeform operations: Contour3D (default), Contour3D/Scallop, Contour3D/Parallel or Steep and Shallow. Steep and Shallow needs Fusion's Machining Extension. Operations are grouped in folders such as Facing, Roughing, Holemaking and Chamfering inside each setup.
- Mastercam: Flat operations chooses 2D Area mill (default) or Horizontal. If CAM Assist can't build the 2D Area Mill regions for a face, it uses Horizontal instead. Freeform operations chooses Waterline (default) or Hybrid. Toolpath Generation on the configuration's General tab decides whether Mastercam calculates the toolpaths straight away. See The "CloudNC CAM Assist Completed" message in Mastercam.
- Siemens NX: operations go in a CAM_ASSIST program folder with one folder per setup. Deburring uses a chamfer tool on NX 2306 and later, and a ball mill on NX 2212. The operations need the matching NX CAM licenses. See What does CAM Assist add to my Siemens NX part? and Which Siemens NX licenses does CAM Assist need?
- GibbsCAM: the Roughing Type and Process preference settings choose the roughing and freeform processes. See GibbsCAM process preference settings.
- SolidCAM: each SolidCAM setup becomes a CAM Assist setup. The part is the CAM part's target, and the first setup uses the CAM part's stock; later setups carry on from the setup before. Each setup's fixture is used as workholding. Operations are created from the templates in SolidCAM's
CamAssistfolder and added at the end of each setup, not in folders. One CAM Assist operation can become several SolidCAM operations, for example drilling at different depths. CAM Assist doesn't create reaming or thread milling operations in SolidCAM. See No toolpaths appear in SolidCAM after running CAM Assist.
What this means for you
- You post CAM Assist's operations with your usual post processor. See Does CAM Assist work with my CNC machine and post processor?
- You can change any operation's toolpath type, parameters or tool in your CAM package after sending, as you would for your own operations.
- To change which CAM package toolpath CAM Assist uses for flat or freeform finishing, click Configuration at the top of the Setups stage and use your CAM package's options on the Finishing tab before you run. See Configuration settings.
- To change an operation's type before sending, see Edit an operation.