Renishaw Probing Routines and Work Offsets

I am trying to understand how the Renishaw macros deal with work offsets.

Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

Something like this:

G65 P9832
G65 P9811 Z-.5 S1.
(Maybe Something here to get make the protected move in G54)
G65 P9810 Z1.25 F150.


I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

If it matters this is a Haas NGC with WIPS.

Thank you!

swinthrope said:

I am trying to understand how the Renishaw macros deal with work offsets.

Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

Something like this:

G65 P9832
G65 P9811 Z-.5 S1.
(Maybe Something here to get make the protected move in G54)
G65 P9810 Z1.25 F150.


I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

If it matters this is a Haas NGC with WIPS.

Thank you!

Click to expand...

Many ways to do this, here is one. The protected move does need a work offset, so can't be used at the beginning of a sequence. But generally, the first P9811 (single position measure) should start .500" (10MM) above the surface.

G65 P9832
G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
G00 G54 Z2.0 (Maybe Something here to get make the protected move in G54) (If you are comfortable, you do not need a protected move here.)
G65 P9810 Z1.25 F150.

Paul

LockNut said:

G65 P9832
G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
G00 G54 Z2.0 (Maybe Something here to get make the protected move in G54) (If you are comfortable, you do not need a protected move here.)
G65 P9810 Z1.25 F150.

Paul

Click to expand...

I'm thinking something like this


G65 P9832
G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
G00 G54
G43 H25 Z1.25 (use probe tool offset no.)
G65 P9810 Z1.25 F150.

swinthrope said:

I am trying to understand how the Renishaw macros deal with work offsets.

Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

Something like this:

G65 P9832
G65 P9811 Z-.5 S1.
(Maybe Something here to get make the protected move in G54)
G65 P9810 Z1.25 F150.


I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

If it matters this is a Haas NGC with WIPS.

Thank you!

Click to expand...

Here you go. This is a bit of code we use for the same thing, modified for your purpose.

T24 M06
T2
G00 G90 G54 X0 Y0
G43 H24
G00 Z1.25
G65 P9832
G65 P9810 Z0. F50.
G65 P9811 S2. Z0
G65 P9810 Z1.25 F50.
G65 P9833
G28 G91 Z0
M01

Lot of bad examples up in here.

It sounds like he wants to jog above the fixture, then set the offset similar to how you use WIPS.

If there is no existing workoffset, you wont be using 9811. P9811 assumes the offset is already set and needs updating.

You should know how far you want to go to set your offset, not just blindly use P9811 Z0 and see how far it goes, up or down. Sloppy.

Set your offset first, then update it. Like how WIPS works, tell it how far to go to reach the expected surface.


How far above are you starting?
#1= 0.5

#5223= #5023-#[2000+#3026]-#1
G43H#3026
G65 P9832
G65 P9811 Z0 S1.
G65 P9810 Z1.25
G65 P9833
M30

Few general remarks:
1. Any of Inspection Plus commands will generate alarm, when no active tool length offset compensation is set in the machine (G43H ***). It does not distinct which offset is set (probe or any other tool), so be sure that probe offset is active.
2. The routines UPDATE rather then SET the WCS. While measuring the bore for example, the actual WCS coordinates are updated by the X Y distances between starting point and measured center point. If one wishes to set X0 Y0 at this point, the X0 Y0 must be set prior to measurement at starting point.

PROBE was right about P9811 updating the work coordinates. Thank you. That was the key. I should have done a better job of RFML. From the manual: New work offset = active work offset + error for internal updates (updating the WCS you are in). So to update my G54 Z with Z0 at a probed fixture I jog to something less than .5" from the fixture and run the following:

%
O01011 (1011)
(probe a fixture from inside G54 and reset the G54 "internal" work coordinates)
N10 G90 G94 G17 G54
N20 G20
N30 G103 P1
N40 T10M6 (this is my probe tool number. Don't use this, use your own!!!!!!)
N50 G43 H10 (this is my probe tool number. Don't use this, use your own!!!!!!)
N60 #5221 = #5021 (Set X0)
N70 #5222 = #5022 (set Y0)
N80 #5223 = #5023 - #5083 -.5 (Set Z0 to the estimated height of fixture. This is current position - tool offset - the distance you think you are from the fixture. This puts your probe in a positive Z position. In this case .5)
N90 G54 (Call so the new variables get read)
N100 G65 P9832 (Probe on)
N110 G65 P9811 Z0 S1 (Touch off fixture - will calculate error and set fixture to 0 and new probe location to the true distance from the fixture )
N120 G54 (re-call to get new Z variable)
N140 IF [[#5023-#5083] LT 1.25] GOTO 160 (Just a double check)
N150 #3000 = 42 (Probe Will Go Down)
N160 G65 P9810 Z1.25 F5.
N170 G65 P9810 X-2.75 F5.
Add more probing here or whatever)

N180 G65 P9833
N190 M30
%

So PROBE what I understand from the above is the work offset stored in the offset page are copied into a working set for the program running. The Renishaw probe macros update the working set, but not the offsets stored in the control. In order to use the macros to set the offset page work offset you need to write the corrected values back into the offset page via the #52xx variables.

slipalong said:

So PROBE what I understand from the above is the work offset stored in the offset page are copied into a working set for the program running. The Renishaw probe macros update the working set, but not the offsets stored in the control. In order to use the macros to set the offset page work offset you need to write the corrected values back into the offset page via the #52xx variables.

Click to expand...

No, this is not true. The work coordinates are not copied, they are updated. I will try to explain how it works.
1. Let's assume part: 100 mm square, G54 WCS set in left lower corner. The G54 WCS register shows X-255.123 Y-155.456 (these are machine coordinates of the position of the left lower corner of the part). 20 mm diameter bore in the middle of the part, ie. its center at nominal X50. Y50. in G54.
2. You wish to set the G54 WCS in the center of the bore.
3. Your program should look like this:
G90G54
M6T30 (CHANGE TOOL TO PROBE)
G43H30Z[#5043-#11030-#10030]F30 (APPLY TOOL OFFSET WITHOUT MOVE)
G65P9832 (SWITCH ON THE PROBE)
G65P9810X50.Y50. F1000 (PROTECTED MOVE TO NOMINAL CENTER OF THE BORE)
G65 P9810 Z-5. F1000 (PROTECTED MOVE INTO THE BORE)
#5221=#5021 (SET G54 X WCS REGISTER WITH CURRENT X MACHINE COORDINATE.)
(THE G54 X WCS REGISTER READS NOW -205.123)
#5222=#5022 (SET G54 Y WCS REGISTER WITH CURRENT Y MACHINE COORDINATE.)
(THE G54 Y WCS REGISTER READS NOW -105.456)
G65P9814D20.S1. (MEASURE BORE, UPDATE THE G54 WCS SYSTEM BY THE DIFFERENCES BETWEEN THE MEASURMEMENT STARTING POINT AND THE FOUND CENTER POINT.)
G91928G0Z0 (RAISE THE PROBE)
G90
G65P9833 (SWITCH OFF THE PROBE)

Pay attention: omitting the lines in bold will result in update of the the corner position rather then bore center position by the differences between start point of the measurement and found actual coordinates.