In process probe inspection

[Eric_Evans_a_GiroDisc_com]

We are adding a Haas DS30 to our shop and want to make use of the new in process inspection tools.  I have two questions about this function:

1) Is there a way to automatically recognize and recut out of tolerance features?

Ideally a probe cycle would be run at the end of a program, recognize X, Y and Z features are OOT, comp the tools, and recut.  What I would like to avoid would be running a probe cycle on one feature, comping that specific tool, recutting the feature, reloading the probe, probing the next feature, comping that next tool, recutting, reloading the probe, probing the next feature, comping, recutting, reloading, probing, etc..., etc...  Lots of potential time wasted with redundant tool changes

2) Is there a way to perform inspections on every N-th part?

We would inspect the first part, and then every 5th part.  We usually do runs on 10-50 parts before swapping to a different program, so this counter would need to reset every time we load a new program.

I'm sure this can be done with macros but I'm curious if these can be programmed directly within Fusion?  We do not have the probing extension yet so I haven't been able to click around and try for myself.

[Richard.stubley]

Hi @Eric_Evans_a_GiroDisc_com,

First of all the good bits...
We currently have a toolpath called Probe Geometry, this allows the use of the macro that can probe a feature and then update cutter compensation. 
We don't do an automatic recut detection this has lots of issues associated with it. I hope we will have an elegant solution to this at some point. 
The solution we normally use is to think about "improving the quality of the next part" but still "validate this part".
So if you use the "update tool wear" function to update the tool wear in addition to the "out of size" action you will ensure this part meets the specification but update the tool wear for the next part. 
See this video here: Tool Wear Update https://www.youtube.com/watch?v=PpY5Ddhx4B0&ab_channel=AutodeskFusion360

About Probing the Nth part. You can easily set up a counter and run a sub program at a Nth number that's not too difficult to set up.


Now onto the bad news......
We don't natively support lathe programming. However that doesn't mean it cant be done. 
As you have a Y axis you basically have a 3 axis mill, that can also spin 🙂 so you can use the milling probing IF THE MACROS ON THE DS ARE THE SAME as the mills. 
There would need to be some post work involved too. 

Do you have any information on the probing macros loaded onto the DS? 
Shamefully I've never actually first hand done lathe probing on a HAAS.

[Eric_Evans_a_GiroDisc_com]

Unfortunately this machine does not have a Y axis.  Can we still do the surface inspect routine and limit the axis to X, Z and C?

Sounds like we will be doing a bit of macro hand coding, hopefully there are plans to expand probing in Fusion to lathes...

[Richard.stubley · Accepted solution]

Hi @Eric_Evans_a_GiroDisc_com,

Sorry I thought it had a Y axis. 

On the inspect surface side of things you would need a very hefty re write of the post processor to get it to work correctly on the lathe. Unless you are happy to do this yourself or pay a reseller I'd stick with the macros in this case as I think they are more what you are after. 

I think the macro probing is the way forward on this. How its implemented in your case is going to be the question.
The 2 solutions I can think of. 

Use manual nc (Pass through) to send through all the code needed to execute the Macro. 
Store this in a template and then just apply it when needed. Downside of this is you will need to hand edit the diameter and Z positions for each feature. The template will insert the bilk of the code but you will need to do some editing. 

The next option is to use the probing functions in Fusion but write the post in a way that will work with your macros. 
This might be the better option as its got less room for error regarding the manual editing. However what you see on the screen and for the simulation will more than likely be wrong, the output code should be correct though when we prove it out.

If you can get a copy of the manual for the Macros I'll be happy to take a look and see what I can do. 

[Eric_Evans_a_GiroDisc_com]

Having a manual NC pass through would not be too bad.  I will probably need that anyways to setup the probe cycles for every Nth part.

I have an NC template set up for this family of parts to "automate" the programming, updating diameters and depths in the manual NC would be quick.

Here are the lathe probe manuals and a sample program I was provided from the local Haas dealers.  Unfortunately it does not contain a variable list, and the machine is not here to check the control...