Renishaw Probing Y Pocket Issue

This has gone all sorts of weird. I have run this program before.

The circumstance is that I have a rectangular tube that needs to be cut down, but it's welded to a plate that cannot be easily aligned, plus the tube is of course not perfectly square. To avoid hand-aligning each one (we usually do 2-4 at a time - they come in pairs) I wrote a short probing routine to set the center of the tube and the angle so it doesn't need to be perfectly square. The last time I ran this it worked perfectly. This time I made two small changes and it is now outputting the Y offset incorrectly.

Code:

G90 G94 G17
G20
G53 G0 Z0.

T40 M6
T4
G0 G54 X0 Y.5 <-- This used to be Y0, but has been changed to avoid a weld seam that previously was not on a centerline.
G43 Z6. H40
G103 P1
G65 P9832
G65 P9810 Z3.5 F100.
G65 P9812 X8.86 Q.25 S1
G65 P9812 Y4.95 Q1. S1 <-- this used to be Q.25 as a "just in case" overtravel, but changed to allow for the 1/2" offset in the beginning position.
G54
G65 P9810 Y-2.5 F100.
G65 P9843 Y-2.75 D6. Q.25
G65 P9810 Z6. F100.
G65 P9833
G103
G0 G53 Z0.


I first noticed the issue when the P9810 move to Y-2.5 stopped with an obstruction alarm. Changed it to -2.35, got it again, -2.2 and again, and then block skipped it entirely. After it ran successfully I noticed the tool was starting awfully far from the part, so checked X0 Y0 and it was a half inch down in Y from where it should be. I have no idea how this is happening. The probe is good, we calibrate regularly, and when the machine was turned off on Friday it had been working as expected.

Any ideas? The Inspection Plus manual (that I followed in the first place) says this should all be just fine.

I worked around it by putting a G65 P9810 Y0. move after the X Pocket routine and that seems to have cleared it up, but why would the initial positioning move (Y0.5) affect the centerline output this way?

Atomkinder said:

I worked around it by putting a G65 P9810 Y0. move after the X Pocket routine and that seems to have cleared it up, but why would the initial positioning move (Y0.5) affect the centerline output this way?

Click to expand...

That's how the macro works. It calculates the difference from where the part actually is, compared to where it is supposed to be (initial). Then adjusts accordingly.

Edit:
The reason they do that is so you don't need to have your origin set on center lines, or center of bore/boss, etc.

EG: Say you had a part with a raised web located at Y2.908
You can still pick up your offset, just moving to that position first, then running the cycle. The macro finds where "Y2.908" should be and adjusts accordingly.

Same with bores/bosses/all the rest. The feature you locate your part off doesn't need to be X0Y0. It can be where ever you want.

Probes are cool.

thesidetalker said:

That's how the macro works. It calculates the difference from where the part actually is, compared to where it is supposed to be (initial). Then adjusts accordingly.

Edit:
The reason they do that is so you don't need to have your origin set on center lines, or center of bore/boss, etc.

EG: Say you had a part with a raised web located at Y2.908
You can still pick up your offset, just moving to that position first, then running the cycle. The macro finds where "Y2.908" should be and adjusts accordingly.

Same with bores/bosses/all the rest. The feature you locate your part off doesn't need to be X0Y0. It can be where ever you want.

Probes are cool.

Click to expand...

As per the programming manual (that I missed previously and our HFO pointed out to me): "Position the probe to the expected centre line of the feature and a suitable position in the Z axis with the probe and probe offset active. Run the cycle with suitable inputs as described."

Ran into it again today trying to offset G55 from a position located by G54. My solution was to pull the G55 XYZ variables and do a little math: #5242=[#5222-.36] and then move to G55 X0 Y0 (had to probe a drilled hole for second operation on the back of the part).

Probes are cool but sometimes irritating

Atomkinder said:

Probes are cool but sometimes irritating

Click to expand...

Ditto on that. On our Okuma the system variable that stores the skip signal position is the "distance from where you started probing to where you touched the part", rather than the absolute position of the part. Totally threw me off at first.