CamCraft

Getting started

Common workflows

Short how-to recipes, one per task. They are not a reference: each links the page that explains the screen in depth. Every recipe ends the same way: Simulate, Deviate, then Post, which refuses by name if something is unsafe (see Reading a refusal). A passing post is not a guarantee; read the program and dry-run it (Posting).

The recipes use one sample part: testdata/models/Milling-test.step in the repository, a small STEP model. Any STEP part of your own works the same.

All recipes start the same way: Model to import the part, Stock to describe the block, Origin to place the work offset, Tools > New tool… to make the cutters (First run).

Face the stock top

  1. On the Stock page pick Box, and use Fit to Models so the block covers the part. Each face of the box has its own allowance: give the top the extra material you want faced off.
  2. Make a flat or face mill under Tools > New tool…, larger than the pass width you want.
  3. Add Face (Milling 2D). On Heights, set the top at the stock top and the bottom at the depth to remove. On Passes, set Stepover and Stepdown.
  4. Click Generate, then Simulate: the tool must clear the whole top of the stock. Deviate shows any material left.

More: Operations.

Square up a block in two setups

  1. Set up the first side as above: Face, then Contour around the outside, leaving the stock you want to keep for the final pass.
  2. Setup > Setups > New setup, with Carry stock and WCS over ticked. The new setup starts from a copy of the first one's stock and work offset.
  3. Re-place the stock and work offset to describe the flipped block (the setup's Settings page has the alignment, including flips such as Flip over X).
  4. On the new setup's Settings page, set the stock source to what the first setup leaves behind, so verification sees the faced and profiled block.
  5. Add Face to the final thickness. Generate, Simulate.
  6. Post writes the program for each setup. CamCraft refuses a carried stock it cannot verify, such as between setups on different machines.

More: Setups.

Pocket and contour a 2D part

  1. Import the STEP model and set the stock as above.
  2. Add Pocket (Milling 2D). On Geometry, pick the pocket's floor face or its loop in the viewport (a click picks the whole face).
  3. On Heights set the bottom at the pocket floor. On Passes set Stepover, Stepdown and Stock to leave so the roughing leaves material for a finish pass.
  4. Click Generate. Add a second Pocket or a Contour on the same geometry with Stock to leave at zero for the finish pass, and Contour around the outside the same way.
  5. Simulate and Deviate; the Frame gouge and Frame rest buttons take the view to the worst spots.

Drill and tap a hole pattern

  1. Add Drill (Drilling). Click Detect holes to find the holes in the model, or pick the hole edges yourself.
  2. Choose the cycle (Cycle): spot, drill, peck, deep or tap. For peck, set Peck depth.
  3. Add one operation per tool: a spot drill first, then the drill, then a tap (or a Thread operation under Milling 2D to thread-mill).
  4. Generate each, Simulate, and Post. Rigid tapping needs a machine that states support for it; a machine without it is refused by name.

Chamfer and deburr edges

  1. Add Chamfer (Milling 2D) for edges you pick, or Deburr (Milling 3D) to break every edge.
  2. Use a chamfer tool or a small ball mill; set its size under Tools.
  3. Generate, then Deviate to check the edge break against the model.

3D rough and finish a surface

  1. Add Adaptive (Milling 2D) or a 3D roughing strategy under 3D Pocket, with Stock to leave on Passes for the finish.
  2. Add 3D Finish and choose a strategy (parallel, scallop, waterline, pencil and others). Use a ball mill.
  3. For rest machining, use the Rest roughing setting on the rougher so it works on what the earlier operation left.
  4. Generate each, Simulate, Deviate: look for gouge first, rest second.

Turn a simple part on a lathe

  1. Click the machine button on the Setup group and pick Turning. The ribbon now shows the Turning group.
  2. Set the stock as a cylinder and the work offset at the chuck or the face.
  3. Add Facing, Profile Rough, Profile Finish, Groove Rough, Threading and Part, in that order, each with its own tool.
  4. Generate each in order, Simulate, then Post with the Fanuc Lathe post.

Cut a sheet part

On a router: follow the full walkthrough in Your first router part (Sienci AltMill 4x4, grblHAL, corner G54, Drill, 2D Pocket, and 2D Contour with holding tabs — Tab count, Tab width and Tab height under Lead in / Lead out — plus RichAuto DSP A11 shop-router notes).

On a plasma table: click the machine button and pick Plasma cutting, add a Plasma Profile, and set Compensation and Direction on its page. Make the torch tool with Kerf width; Pierce height is on the operation's page.

Simulate and Post as usual.

Re-post a job for a different machine

  1. Open the setup's Machine page and Load machine (.mch), or pick another machine, then pick its post on the Post page.
  2. Regenerate the stale operations (Regenerate all stale, or Generate on each).
  3. Post. Read what is refused: a machine-limit refusal names the axis or setting and the limit. Fix the setup, not the limit.

Use the tool library

Tools can export a library (Export library…) and Import library… reads one back, so tools are reused across jobs.

Not yet

Importing a tool library from another system, and a router machine mode (tabs work today on a mill Contour), are not described here because they are not on main yet.