Probing tool wear with stock to leave

[ELAFING]

I have a bore that is machined -.020. 

How do I probe the bore and adjust tool wear using this -.020 as the calculation?

i.e. the probe returns -.025 from nominal dia. I want the tool wear to adjust the -.005 only, not the -.025.

Thanks in advance. 

[Richard.stubley]

Hi @ELAFING,

Its exactly for days like this we put update tool wear into the probe geometry toolpath.

You need your toolpath before the probing operation with the stock to leave applied. 
In my case its a 50mm hole with 0.2 radial stock to leave applied.
I then make a probe geometry item and in the actions tab under the update tool wear check box I select the previous machining op as my reference toolpath.
then posting out the NC code shows a diameter value of 49.6mm is output (50mm -0.2 twice as it radial stock to leave)

I hope this answers your question if not give me a shout. We even go as far as checking you had cutter comp on in the reference operation as its no point updating the wear table if the feature you are probing did not use cutter comp in the first place.

[ELAFING]

So whats the next move? If I duplicate the tool path and move it after the probe move it will over cut if I remove stock to leave, correct? Do I keep stock to leave the same and let if use comp to bring it to size? 

Thank you for jumping in on this.  

[Richard.stubley]

Hi @ELAFING,

Yes if you duplicate the semi finish toolpath, move this to after the probing operation. Remove the stock to leave this should then do what you are after.

I see this being implemented in 2 scenarios.

            1: A one off part.
In this case I would semi finish the feature, add a stock to leave on the feature but make sure the finishing stepover on the feature is the same as the stock to leave.

I am doing this to give representative forces on this semi finishing cut that will then be on the finishing cut. We know that tool wear is as much about deflection as wear itself.

I then do the probe geometry toolpath and select this previous milling operation as the reference operation.

Now I do the final milling operation.

Optionally I could probe the feature again to ensure it is prefect, tick the out of size action in Fusion and set the correct tolerances. (You can also tick print results to get this output)

2: Repeat production.

Similar to the one off part, but here I am improving the quality of the next part while still checking the part I have just machines is correct to tolerance.

I machine the feature fully.

Then add a probe geometry feature with tool wear update and out of size action.
This will check that the part I have just made is correct to drawing, but with the added benefit of improving the quality of the next part by updating the tool wear.

[ELAFING]

Fantastic!!! I cant wait to give this a try. Did some probing along axis yesterday to set rotational values. I love this stuff. 👍

Thank you very much Richard.

[Richard.stubley]

No Problem, Here are some other tutorial videos I have done that may be of use.

Probe WCS https://www.youtube.com/watch?v=vZnPwe3ZqwE&t=32s&ab_channel=AutodeskFusion360

Part alignment https://www.youtube.com/watch?v=y2D1Ct8nMEM&ab_channel=AutodeskFusion360

Manual measure https://www.youtube.com/watch?v=1uhETSR-ALY&t=433s&ab_channel=AutodeskFusion360