These settings control how CAM Assist machines a hole group and each feature in it. Open them from a hole group card in the Feature planning stage. See Review and edit hole groups in Feature planning.
Where to find them
- Open details on the card: the hole's dimensions and every setting in one window. Choose Overview on the left for the group settings, or a feature or Hole bottom for its own settings. Click Done to keep your changes or Cancel to discard them. Done is unavailable while a feature has an error ("Fix the hole element errors to save.").
- Group settings on the card: the group settings, edited on the card.
- A bore, chamfer, thread or the bottom in the card's callout or diagram: that feature's settings, edited on the card. Changes on the card save automatically once they're valid.
A dot next to a feature's title means you've changed it from every CAM Assist suggestion. Depth comes from the model and can't be changed (padlock, "From the model").
Group settings
| Setting | What it does | Default |
|---|---|---|
| Restrict to setups | Select one or more setups to machine the group's holes only in those setups. Shown only when the part has setups. See Choose which setups machine a group. | None selected: any setup may be used |
| Pilot drilling | Shown with a padlock ("This feature is coming soon") and can't be changed. CAM Assist plans pilot drilling itself. | Automatic |
| Spot drilling | Automatic, Required or Disallowed. Spotting improves hole position. If no spot drill is available, the holes are still machined, but Required reports an error and Automatic may report a warning. | Automatic |
Feature settings
| Feature | Settings |
|---|---|
| Hole bottom | Shape: Drill point or Flat. A through hole has no bottom to choose. Point angle is locked: the drill's own point angle is used. |
| Bore | Diameter, and Finish > Ream to size to ream it. |
| Chamfer | Start ⌀ and End ⌀. Included angle is calculated from the diameters and the element depth. |
| Thread | The thread (see Choose a thread for a hole), Thread depth and Threading process: Automatic, Cut tap or Thread mill. |
| Fillet | Shown for reference only. CAM Assist can't machine a hole that contains a fillet, so it plans no hole-making for it. |
| Unsupported section | CAM Assist found a section it can't machine. There's nothing to set. |
When CAM Assist read a feature more than one way, choose the feature Type (Bore, Chamfer or Thread) and step through the readings with the Suggestion arrows. For a thread, likely threads are listed under Suggested for this bore.
Some labels on the card differ slightly from the Open details window, for example Diameter ⌀, Threadmill and Recommended. They're the same settings.
Thread depth
Choose Full depth to thread the whole bore, or Custom to enter a depth. The hint below shows the most you can enter. With a custom depth, turn on From far end to thread from the other end of the hole.
| Message | Fix |
|---|---|
| Enter a valid threaded depth greater than zero. | Enter a positive depth. |
| Threaded depth must be at least one pitch for the selected thread. | Increase the depth, or choose Full depth. |
| Threaded depth cannot exceed the selected cylinder depth. | Reduce the depth to at most the value in the hint. |
Reaming and thread milling availability
If Ream to size or Threading process shows a padlock with "Your CAM add-in doesn't support reaming yet" or "Your CAM add-in doesn't support thread milling yet", your CAM package's add-in can't create that operation. Autodesk Fusion, Mastercam, GibbsCAM and Siemens NX all support both at the time of writing.