Probe geometry for tool wear

00:03

In the Manufacturing Extension, the Probe Geometry strategy enables you to use probe cycles on your CNC machine

00:11

to measure and verify the geometry of critical features.

00:14

If there is deviation due to tool wear,

00:17

subsequent machining operations can be adjusted to compensate for the wear and to help ensure continued accuracy.

00:25

In this example of a part with toolpaths already set, the semi-finishing and finishing passes are split into 2 operations,

00:33

and a tool wear update will be applied between the operations.

00:37

In the 2D Contour dialog for the semi-finishing operation, the cutter Compensation Type is set to In control,

00:44

and for added accuracy, the finishing Stepover is set to the same value as the Stock to Leave.

00:50

This helps to ensure that the deflection is representative of the finishing cuts.

00:56

To generate a Probe Geometry operation, on the Manufacture workspace toolbar, click Inspection > Probing > Probe Geometry.

01:06

In the Probe Geometry dialog, on the Tool tab, click Select to open the Select Tool library.

01:13

Select a probe—here, Cube OP 20—then click Select.

01:19

Back in the Probe Geometry dialog, click the Geometry tab and verify that Select is active for Probe Surfaces.

01:27

Then, on the canvas, select the geometry you wish to inspect.

01:32

Back in the dialog, under Feature Tolerances, update the Position and Size—in this case, to 0.1 mm for both.

01:42

For this example, click the Actions tab, and then select Out of Position and Wrong Size.

01:49

This instructs the machine to stop machining and show a warning when the position or angle of the geometric feature is out of tolerance.

01:57

To improve the accuracy of future machining operations,

02:00

select Update Tool Wear to update the tool-wear compensation stored in the controller of the CNC machine.

02:07

Then, click Select and select a reference operation in the Browser.

02:12

This is typically the last operation that machined the feature, and provides important information, such as the tool number and stock to leave.

02:21

Next, set the Minimum Update Threshold—here, to .02 mm.

02:27

This function stops the tool wear from updating the controller for every micro-deviation found.

02:33

In this case, a value of .02 mm means that the tool wear updates only when the deviation of the tool is .02 mm or more.

02:43

A general rule is that up to 10% deviation is acceptable.

02:48

Finally, select Print Results to import the results back into Fusion for graphical representation.

02:54

Click OK, and the operation is generated.

02:59

In the Browser, rename your operation appropriately.

03:03

Then, click and drag it to the desired place in your machining workflow—in this case, just after the semi-finish pass.

03:11

In this example, the steps are repeated to create another Probe Geometry operation—this time, to probe for length.

03:19

Notice that the probe point can be dynamically dragged on the canvas.

03:25

After making selections and clicking OK, the operation is added to the Browser.

03:32

Again, the operation is renamed and reordered in the workflow.

03:38

In this example, it is optimal to do a final check of the bore as well.

03:43

The steps are repeated to create another Probe Geometry.

03:47

However, this time Update Tool Wear is not selected.

03:51

Now, you are ready to begin using the Probe Geometry feature to create probing operations.

03:58

Using these probing cycles on your CNC machine can help to ensure that your machining operations are accurate

04:05

by detecting and compensating for potential tool wear.