Preparing machining operations

Geometry describes the part. An operation specifies how to machine it. Inspect every operation before calculation and export.

How do I create an operation for selected objects?

Select the required contours in Drawing, then choose an available operation from Operations. Select the new operation in the left list to edit its parameters. Name operations meaningfully, for example Holes, Outside cut or Marking.

The available kinds depend on the selected post-processor. Cut is used for vector cutting, Engrave for marking along contours, Hatch for filling an area with engraving lines, Profile for milling along a contour and Pocket for removing material from an area. Select the process first, then set its appropriate values; changing the name alone does not change the machining kind.

How can a DXF arrive with Cut already assigned?

In Settings choose the default DXF operation, for example Cut when supported by your post. Opening the next DXF can then create operations immediately. Choose None when you want to assign every operation yourself. This preference is for new imports; it does not rewrite the machining decisions in an existing saved project.

Generated shapes also offer Create operations. Check that option to insert the geometry together with the selected default operation. Clear it when you only need drawing objects or intend to assign different processes to separate contours.

Why can the same text or contour be machined twice?

The same geometry can belong to two operations, for example an automatically created Engrave followed by a manually added Cut. Simulation then shows both, and their ordering rules may differ. This is different from intentional depth passes within one operation.

When adding an operation to already assigned objects, leave Replace existing operations enabled if the new process should replace the old one. Clear it only when you intentionally want both processes. Review the left list, remove an unwanted operation and calculate again. Keep the drawing objects when you only want to remove their machining assignment.

How do Center, Inside and Outside affect the result?

Center follows the drawn contour. Inside and Outside move the toolpath to the chosen side using the cutting width or tool diameter. For a finished outside edge you usually place the tool outside; for a hole you usually place it inside. Check the displayed path rather than relying only on the label.

Offset compensation needs a valid closed contour. Tiny gaps, overlaps and self-intersections can prevent a valid result. Do not compensate the same width twice, once in the geometry and again in the operation. Common cut pipe layouts use Center because a shared boundary cannot independently offset for both neighboring parts.

Which values should I set for cutting or engraving?

Check the feed, power where supported, cutting width, number of passes and any process-specific delay. Use settings established for your machine and material. The application cannot infer a suitable power or speed merely from a DXF outline.

For milling, also check tool diameter, safe height, final depth and stepdown. Final depth below the work surface is negative; stepdown is a positive amount per pass. For Pocket, use a positive stepover no greater than the tool diameter. Recalculate after changing these values and inspect the pass count and clearance moves in simulation.

Can I edit several operations together?

Use the operation selection controls on the left, including Select all operations when appropriate. Inspect which operations are selected. In Common parameters check only the fields you want to change, enter their values and press Apply to selected operations; editing a value alone does not apply it. If the operations use different processes, some fields may not apply to every selected item.

For a change that should affect only one contour, select its own operation and verify the highlighted geometry. After a bulk change, inspect representative operations and calculate again. Saving a copy of the project before a major strategy change makes it easier to compare the previous result.

How do I choose where a contour starts and its direction?

Select the relevant operation or drawing contour and open its path settings. Choose the start point and cutting direction, then inspect the calculated path. When more than one contour is involved, identify the intended contour before applying its settings.

Entry and exit paths can move the start of machining away from the finished edge. Leave sufficient space for them around nearby parts and sheet borders. A lead that fits one contour may collide with an adjacent part after nesting. Common cut layouts restrict offset, entry/exit leads and loop features; start and direction choices remain available.

What is the difference between User priority / inner first and Manual operation order?

User priority / inner first uses your operation priorities while keeping inner cutting contours before the enclosing outside contour. It is useful when you want influence over the order without losing the hole-before-outline rule.

Manual operation order follows the operation order you set and does not automatically impose that nesting rule. Use it when you need a specific sequence and have checked the consequences yourself. Use Up and Down to order operations, calculate and watch the sequence. This orders operations, not every individual contour within a multi-contour operation. A part cut free too early may move before its remaining features are machined.

When should I choose By nesting level or One family at a time?

By nesting level groups work by how deeply contours sit inside other contours. It is useful for completing a similar depth of internal features across a job before proceeding outward. One family at a time keeps a part and its contained features together before moving to another family.

These choices organize the machining order; they do not change the drawing geometry or automatically solve every production constraint. Inspect a representative part with holes and a neighboring part in simulation. For intentional exact sequencing between unlike operations, use Manual operation order and verify the resulting order explicitly.

Can I alternate cuts in distant areas to spread heat?

First choose By nesting level or One family at a time, then choose distant-cut alternation in the spatial ordering settings. It is unavailable in User priority / inner first and Manual operation order. It favors work away from the recently cut area while respecting the applicable cutting-order rules. This can help distribute cutting activity across the sheet.

It is an ordering aid, not a thermal calculation or a guarantee against distortion. Heat also depends on material, thickness, power, speed and how much material remains connected. Review the longer rapid moves and the inner/outer sequence. Exact Manual operation order takes precedence over automatic spatial reordering.

Where is Punch and when can I use it?

Punch is a machining operation, not a separate ready-made shape. It is available when the selected post supports that process. Select the relevant geometry, choose Punch from Operations and set the fields presented for the operation.

If Punch does not appear, check the selected post instead of looking for it in Complex shapes. A laser or router post may not support the same commands as a punching machine. Inspect the calculated result and ensure the selected post describes the machine process you actually intend to use.