Probe WCS: Will it update my WCS or does it just a reference?

[CuttingEdgeManufacturing]

I am using probe WCS to check a tight tolerance bore after cutting. and somehow the parts are off center. They thought the vice might have moved. but it didn't. now they are questioning if the probe is slowly moving my WCS around after each part when it checks the bore. I don't believe it does. but I figured id see what you guys know.

[DarthBane55]

Could you post the code line of the actual probing cycle here please?

The probe can do all of it, it can measure bore, it can set work offsets too, and it can do both at the same time as well.  It depends what's on your particular line of code.

[CuttingEdgeManufacturing]

Sure here it is.

(Probe WCS1)
/ N3900 G28 G91 Z0.
N3905 G90
N3910 M1
N3915 T1 M6
N3920 G54
N3925 G28 G91 Z0.
N3930 G90
N3935 G0 X0. Y0.
N3940 G43 Z2.2 H1
N3945 T2
N3950 G65 P9832
N3955 G65 P9810 Z0.2 F80.
N3960 G65 P9810 Z-0.8381
N3965 G65 P9814 D1.25 Q0.4 S1.
N3970 G65 P9810 Z0.2
N3975 G0 Z2.2
N3980 G65 P9833

N3985 M5
N3990 G28 G91 Z0.

[programming2C78B]

Yes. S1 is offset 1, or g54. You want to probe it as any other work offset and use I assume it's being milled to 1.25 at x0. y0. so not sure why your positional would be off every time! 

[DarthBane55 · Accepted solution]

EDIT: sorry @programming2C78B I was writing as you posted the answer already.

S1 does indeed update your work offset.  Did you get a Renishaw manual?  Here are the parameters you can play with, when using macro 9814 (bore/boss):  (there are more pages explaining how it works, I suggest you find a manual and read it, it will make you understand all of it pretty clearly.  You just have to read the chapter on the cycle you are interested in really).

  

[CuttingEdgeManufacturing]

so what if i dont want it to update my WCS? i simply want to measure a bore size. do i just give it a bogus WCS like G59 so it doesnt actually update the one im using?

[DarthBane55]

You simply don't write S1, this is optional.  Just delete it from your line.

You can also add tolerances to the bore measured, as you'll see in the pages i posted.  So if your bore is very tight tolerance, you can put that tolerance on this line, and the machine will alarm out and stop when the bore is out of tolerance.  You can also see the actual measurement in your machine, it is stored under variable #138 I believe.

[CuttingEdgeManufacturing]

oh ok. i gotcha. yea I know i can set a tolerance. almost did that, but wrote a macro instead to take the measurement and compare to my tolerance, then adjust cutter comp and recut.

#100 = #188 (store bore measurement in non volitile variable)
IF #100 LT 1.2497 GOTO5000 (check bore measurement to tolerance)
IF #100 GT 1.2500 GOTO6000 (check bore measurement to tolerance)

(in tolerance bore continues)
N3995 G90
N4000 G0 X0.
N4005 G53 G0 Y0.
N4010 M30

(update tool wear based on bore measurement)
N5000
#101 = 1.2498 - #100
#2615 = #2615 - #101
GOTO3360


(bore oversized - retract and alarm out)
N6000
N3985 M5
N3990 G28 G91 Z0.
N3995 G90
N4000 G0 X0.
N4005 G53 G0 Y0.
#3000 = 100 (Bore Oversized - Scrapped Part)

[DarthBane55]

Excellent!  This is great work...  however... hehe...  you can do this automatically by adding T at the end of the line.

Say it is T10 that cuts the bore, if you add T10 at the end of the line, it will update wear offset on T10 automatically to make the bore nominal.

What you did is great though, because it will recut automatically.  I did very similar, just a bit different.  So I rough the bore leaving for example 0.020" radial allowance.  Then I semi-finish with the finishing tool, and leave 0.010" allowance.  Then I probe, and it adjusts the wear offsets automatically as explained above.  Then I do the finish cut with the same tool as the semi-finish tool.  The bore comes perfect every time, and there is no recutting per say (well, there is a semi-finish cut).  The big advantage is that the bore will never go oversized and scrap the part.  The trick is to take the exact same amount on the semi-finish cut as the finish cut, the exact same cutting parameters, so the tool is loaded the exact same way.

But for sure, what you did works great too, I like it!

[CuttingEdgeManufacturing]

I love the approach you talk about. alot of people just don't get that.

I think i was aware of the T10 option for the bore cycle, however yea it wont go in and recut the finish pass, so i wanted to do more of an automated approach.

[DarthBane55]

Yep I understand.  Just to make sure you understood what I meant though, it is automated right.  It does semi-finish, probe with wear offset adjustment, then finish.  The difference is that for you, you only need re-cutting if undersized, for me, it will do a semi-finish and a finish cut every single time (small time penalty).  Both methods work perfectly, just wanted to make sure you got that it was automated, this runs overnite that way, no machinist intervention.

[CuttingEdgeManufacturing]

yea i get it.

we just got a robot arm on a VF2SS this year so this is a very good tool to go with that.

[Richard.stubley]

Hi Both, just a quick note on this. If you have the manufacturing extension then probe geometry will do all of this for you. 

You can semi finish a bore with 0.2 stock to leave. You then choose this toolpath as your reference toolpath in the probe geometry toolpath and it will correctly adjust the nominals sent to the macro to expect the size to be 0.4 off the finished diameter. 

[CuttingEdgeManufacturing]

Any links to tutorials/ screencasts?

i dont re call a reference toolpath in probe operation, but its not impossible i overlooked it.

**EDIT

probe Geometry not probe WCS, the one only accesible under the extension. thats why i havent seen it. Good to know, however Extensions are not allowed for me as they are pricey.

[Richard.stubley]

If you do get the extensions here is a little tutorial on updating tool wear using Probe Geometry.

https://www.youtube.com/watch?v=PpY5Ddhx4B0&t=148s&ab_channel=AutodeskFusion360