Tool Mapping

To open the Tool Mapping dialog, Click NC Code in the Steps panel, then click Re-map the tools to new tool slots in the NC Code dialog.

The Tool Mapping dialog is where you change the tool slot assigned to the selected tool. You can change the Cutter comp. offset register for any tool here too.

The dialog has a table at the top. Each row of the table represents a tool. Select a tool to edit its values in the fields below the table.

Double-click on a tool name, or click the + to the left of the tool name to see the list of operations that use that tool.

Click the Add tool slots button at the top left of the table to open the Number of tool slots dialog. It enables you to increase the number of tool slots listed; you cannot reduce this number.

Tool number — This corresponds to the first (gray) column in the table and is the current tool slot number for that tool. To move a tool to a different slot tool slot, enter a new Tool number and click the Set button, or drag-and-drop the name of the tool in the table onto the tool slot number in the left column. More than one turning tool can occupy the same tool slot.

Diameter offset register — Specifies the diameter cutter compensation offset register number for the tool. This value is passed to XBUILD as <COMP-NUM>. It corresponds to the Diameter column in the Tool Mapping table. Enter up to 8 digits.

Length offset register — Specifies the tool length offset register number. Most lathe controllers have a single register that contains the length and diameter offset values. In this case, the Length offset register is the important field to set in FeatureCAM. This value is passed to XBUILD as <OFFSET#>. It corresponds to the Length column in the Tool Mapping table. Enter up to 8 digits.

2nd Length (for grooves) — The second length offset register for groove tools. The default second offset register number is the Tool number plus the 2nd offset reg. increment in the Turn default attributes.

Note: To set the offset registers by operation, select the operation in the table. You may need to expand the tool name to view the operation.

Note: Most lathe controllers have a single register that contains the length and diameter offset values. In this case, the Length offset register number is the important field to set in FeatureCAM.

Block offset register — Enter the tool block offset register number. This value is passed to XBUILD as <TOOL-BLOCK-OFFSET-NUM>. This option corresponds to the Block Offset column in the Tool Mapping table.

Tool ID — This corresponds to the ID column in the table and is the tool ID register for the tool. This is a seldom-used field that is used by Bridgeport lathes and occasionally for Cincinnati machines.

The Tool Mapping dialog has these buttons:

Same — This sets the cutter comp. offset registers for all tools to the value of their tool slot number.

Set — Select a tool in the table, enter a Tool number and click the Set button to assign this tool a number specific for this part.

Note: This assignment is for the current part only. If you want to assign a tool to a default tool slot for all parts, use the Overrides tab of the Tool Properties dialog.

Save in Crib — This permanently assigns the tool number with the tool in the database. The tool is then locked in this position for all parts that use the tool.

Clear in Crib — The tool number slot for the selected crib is erased. This means you want FeatureCAM to assign a tool number automatically.

Note: See Tool Manager for more information on tooling databases.

Set All — All tools numbers are set to their current values and are not changed.

Reset All — This returns all tool slot numbers and cutter comp offset registers to their initial values.

Select Block — Click this button to display the Tool Block Selection dialog, which you can use to specify which tool block is used to hold the selected tool.

Tool Life — Tool life management enables you to limit the use of a tool and automatically switch to another tool when that limit is reached. It is useful when cutting hard material that may wear out a tool during a single program run. The table in the Tool Mapping dialog displays the number of Holes that are cut by each drilling tool and the Time (number of minutes) that each milling tool is used during a single run of the NC program. Select a tool in the table and click the Tool Life button to open the Tool Life dialog.

Note: This button is not available until after you have run a simulation.

Show Machine — In Swiss Turning documents, click this button to show a preview of the active MD file on the right of the dialog with the tool slot numbers displayed. To control the view of the machine preview, right-click the image and select Pan and Zoom or Rotate, then click and drag the image. Click Hide Machine to hide the machine preview.