To change the machining order of features and operations

When you create features, FeatureCAM splits them into operations for manufacturing. For example, from a Hole feature, FeatureCAM creates spotdrill, drill, and countersink operations. FeatureCAM uses logic to ensure that operations created from a feature are manufactured in the correct order. For example, a Hole is spot-drilled before it is drilled and a Pocket is roughed before it is finished.

By default, a part is manufactured in the order it is created. You can change the order of manufacture manually, or you can set automatic ordering optimizations.

To order operations manually

1. Select View tab > Reports panel > Operation List.
2. Select Manual Ordering in the Op List tab of the Results window.
3. Drag items in the operation list to change the order.

If you create a new operation with Manual Ordering selected, the new operation is inserted at the end of the list.

To order operations automatically

1. Select Automatic Ordering at the top of the Op List tab.
2. Click Ordering to display the Automatic ordering options dialog.
3. Select or deselect the following ordering options:
   • Minimize tool changes — Groups operations together that use the same tool. This saves time for you by eliminating or reducing needless tool changes. You must select this check box if you want to generate hole macros in the NC code.
   • Do finish cuts last — Moves the finish milling operations to the end of the Setup without altering the order of the finishing operations. If you want to perform all rough milling operations before finish milling operations, select the Do finish cuts last attribute.
   • Cut higher operations first — Affects only milling Setups. Select this option to mill the features from the top of the stock first and work toward the bottom. If you deselect this option, you should graphically verify the toolpath before cutting your part.
   • Minimize rapid distance — Affects only milling Setups and is the only ordering option that changes the order of features specified in the part view. Minimize rapid distance moves to the next closest feature that uses the same tool as the last operation. You must deselected this option if you want to generate hole macros in the NC code.

   As you select ordering options, the operations are re-sorted.

4. For turning documents:
   • To automatically optimize the operation order, select Use rules.
   • To order the operations by feature type, select Use template, click Edit template, and set the order of the operations in the Feature Order dialog. This template is remembered for all your parts.
5. Click OK.

If you create a new operation with Automatic Ordering selected, the new operation is automatically sequenced using the selected ordering options.

Note: If Never is selected on the Options > Manufacturing > Toolpaths page, click Update Now on the Op List tab to update the Operation List.