Thread: Dynamic Probing Trouble

Hi All,
I am trying to do some probing while I have dynamic rotation active on my 5 axis Mazak. But it is not working I keep getting probe errors. Probe Obstructed, probe fail. I am not sure I can probe while G54.2P1 is active to begin with so I don't know if its my code or the machine. Any help would be great. The goal of this probe cycle is to touch a cast surface and place the deviation of its location into my Z shift. I have included my probe cycle and drill cycle.

Thank You,
Renishaw OMP60
Mazak Variaxis 630 5X
Inspection Plus Software



N484 M00
(8002 Z FACE DATUM SHIFT SET )
N486 G90
N488 T80
N490 M6
N492 G90G80G40G0
N494 G91G28Z0
N496 G90
( FIRST POSTION FROM YOUR DRILL CYCLE)
N498 G54G00G90X0.Y5.54A-90.C-180.
( SECOND POSTION FROM YOUR DRILL CYCLE)
N500 G43H80G54.2P1X0.Y5.54Z10.3A-90.C-180.
( ENTER Z LOCATION OF SURFACE +2" )
N502 G65P9810Z8.3F100
( ENTER Z LOCATION OF SURFACE )
N504 G65P9811Z6.3Q2.5
N506 G54.2P0G53Z0.
N508 G91G0G28Z0
N510 G30X0
N512 G28Y0
N514 G90
N516 #5203=#137
N518 M00 ( YOU MUST RESET DATUM SHIFT BACK TO ZERO )
( WHEN YOU ARE DONE USING IT OR MAKE SCRAP )
(TOOLPLANE NAME - TOP)
(.718 SOLID CARBIDE DRILL)
N520 T30
N522 M6
N524 G91G28Z0.
N526 G54G00G90X0.Y5.54A-90.C-180.S800M03
N528 M8
N530 M51
N532 M131
N534 G43H30G54.2P1X0.Y5.54Z10.3A-90.C-180.T26
N536 G98G81Z4.05R6.55F9.
N538 G80
N540 M9
N542 M05
N544 G54.2P0G53Z0.
N546 G91G28Z0.
N548 G28Y0.
N550 G30X0.

Couple notes...

Probing isn't set up for dynamic comp so it doesn't recognize G54.2 . You have to set up your offsetting first then calculate the shift by macro to input dynamic comp offsets.

Code:

N504 G65P9811Z6.3Q2.5

You need a "S" value for the offset to write to...

Then you made the common shift equal to the Z offset you're trying to set so now you're actually off by the Z position of the probing (if it could enter a value but since your probing is getting errors...).

From the program that's posted, I don't see why you need to run dynamic comp. You could just simply set Z at G54 with the added "S1" and go from there. You should just be able to do it this way and run G54...

Code:

N496 G90
N498 G54G00G90X0.Y5.54A-90.C-180.
N500 G43H80Z10.3
N502 G65P9810Z8.3F100
( ENTER Z LOCATION OF SURFACE )
N504 G65P9811Z6.3Q2.5S1 (Write to G54 Z)
N508 G91G0G28Z0
N510 G30X0
N512 G28Y0
N514 G90
N518 M00 ( YOU MUST RESET DATUM SHIFT BACK TO ZERO )
( WHEN YOU ARE DONE USING IT OR MAKE SCRAP )

I don't have any S code because I just want to get the difference from the programed Z surface vs the actual Z surface. I then want #147 or whatever the Z potion difference is to input into my Z shift run my tools then clear my Z shift out. I already have a probe cycle that sets my dynamic offsets this is just to help me with cast surfaces. The probe moves to the right spot right up untill the P9811 line?

Thank You,

Does it bomb out while executing the P9811 line? If so, my guess would be is that you need to increase your Q value to increase the search distance....

Still not sure why you need to use Dynamic offset here... ...

The probe never moves in the Z direction once it hits the P9811 line. I am probing this because I have found the axis of the hole using a 5 axis drill cycle inside of MasterCam but the part is a casting. So I am on the center of the hole but need to know how much deviation there is from where I programed the Z surface to where the casting Z surface is since NPT taps are very depth dependent.

Thanks,

Didn't we talk about this before? The stuff Joe mentioned didn't get it straightened out huh?

So, we need to figure out exactly where it's bombing out. But first thing, you can't probe with dynamic active because the macros aren't looking for dynamic values unless you've modified the macros to calculate the movement with dynamic. If your dynamic shift is large enough, the probe could be bombing out because the macro thinks you're at one place but the machine position says you're somewhere else. If this exceeds the value of the probing range, you get a probe open... that's my guess anyway. So, let's back up a minute and go from scratch here....

If I recall this correctly, you probe on a finished bore ID/OD with the part "up", then have to rotate the table and trunnion for some NPT holes around the OD. The casting varies so you need to know where the casting is because the depth of the NPT is relative to the cast surface. Is that about right? I take this bore isn't on center with the A or C axis?

Yes I was talking about probing before but that was a diffrent aspect. I am slowly building up my probe cycles. I do have a cycle set up now that sets the XYZ dynamic offsets for me and it works great Now I am trying to get to the next step. I wanted to be able to position the probe while dynamic rotation was active so I could touch off the cast surfaces that are on the OD of cast parts. Then I was going to transfer the deviation value into my Z shift offset run a few tools and set the shift back to zero. Right now after the probe gets two inches above the surface it gets an error so I reset the program. Then I go into handwheel mode zero my Z and look at my readout touch off the surface take the diffrence and put it into my z shift. This is working ok but it sure would be nice if the machine could do this on its own with out my help So I understand that the probe macros might have trouble in dynamic but is there some other way you can drive this probe? Seems like such a very simple thing to be able to probe like you can machine? I know I could probe before I go into dynamic but when I have holes a compound angles it seems like this would be more trouble than it is worth.

Thanks

Renishaw macros use absolute machine position standard work coordinates in its calculations and moves. Since G54.2 puts the parts in "space" relative to machine position, the numbers don't add up in motion. When your probe bombs out, I don't think it's bombing out on 9811, I think when it completes 9810 the value checks are off so it's giving you a probe open alarm.

With G54.2 on a 5axis, your part is essentially a gyroscope now so the calcs are pretty intense and convoluted at the same time. I'm not even sure if there are any machine variables available for you to read and use that will give you the tracking with G54.2 in motion. The only thing I can think of is you could ‘back door’ this a couple different ways…

The first way is using manual intervention similar to what you’re doing now only a little more automated. So the operation would run like this assuming you’ve already set the G54.2 shift:

N488 T80
N490 M6
N492 G90G80G40G0
N494 G91G28Z0
N496 G90
( FIRST POSITION FROM YOUR DRILL CYCLE)
N498 G54G00G90X0.Y5.54A-90.C-180.
N500 G43H80G54.2P1X0.Y5.54Z10.3A-90.C-180.
N502 G1G31Z8.3F100. (Uses skip signal for safety and not Renishaw macro)
#890=#5023 ( WRITE CURRENT Z )
M0
( MANUAL INTERRUPT )
( WATCH CNC SIGNAL AND TOUCH OFF PROBE TO SURFACE)
( THEN CYCLE START)
#891=#5023 ( WRITE SURFACE Z )
#801=[#891+ABS[#890]]+2. (WRITE Z SHIFT FOR STOCK )
G1G91Z.02F50. ( ESCAPE Z FOR PROBE )
G1G31Z2.F100. ( SAFETY Z OUT )
G0G90G53Z0
.
<CONTINUE FOR MORE HOLES CHANGING SET VARIABLE>
<EX: HOLE 2 = #802, HOLE 3 = #803, ETC, ET>
.
N506 G54.2P0G53Z0.
N508 G91G0G28Z0
N510 G30X0
N512 G28Y0
N514 G90

The set variables can be anything as long as it’s not one being used by the machine or software. I would also avoid using local variables for this (1-33) as well as #100 - #199. The above also assumes that you’re always starting at 2.0” above the theoretical surface which is what the last “2” is on this line: < #801=[#891+ABS[#890]]+2. > Then in your program, just add the variable number to your Z depth in the canned cycle:

G98G81Z[6.3+#801]R6.55F20.

The ‘escape’ moves are in G91 to ignore any comps. The first .02 move is only to get the probe off of the part since it will still be touching. The short move won’t destroy the probe in case it goes the wrong way and the probe won’t fault out right away due to contact. The next G91 move turns on the skip to clear the part.

The 2nd way to probe something like this is to use/make a probing spud (or spuds) that attach to the part (since it seems your part is floating) and probe that for the different offsets. But with the nature of your part as I see it, this method wouldn’t work for you. Just be careful running something like the above as I haven’t tried this one. Also, since the skip signal isn’t always on, be careful in Handle mode (as you already are).

I also have a Variaxis 630 with the same probe, but I don't do a lot of probing...I'm just starting to use it more. Psychomill's last post is a bit over my head, but I have another suggestion for a workaround.

When I need a little more control of the axes during indexing (i.e. with a tombstone, or with a large deviation vector) or if I need to use G05, I use dynamic comp to set to establish real work offsets rather than work in G54.2. Here's the basic approach:

1. Invoke G54.2 Px
2. While in position, write machine coordinates to G54.1 Py
3. Cancel G54.2 Px
4. Invoke G54.1 Py
5. Probe/machine away!

Don't know if that is usable in your application, but just thought I'd share another approach.

Thanks guys I will have to think about the last two ideas awhile before I can decide if this will work.


Thanks,

Ok this looks like it might work I changed a few things as noted below. But how do you know that #5023 will grab the machines current Z pos. I am looking in the manual and can't find this info. Now all I need is some work to try it out...

Thanks,

M00
(THIS CYCLE IS A TEST NOT PROVEN YET)
(8002 Z FACE DATUM SHIFT SET SKIP SIGNAL )
T80
M6
G90G80G40G0
G91G28Z0
G90
( FIRST POSITION FROM YOUR DRILL CYCLE)
G54G00G90

( SECOND POSTION FROM YOUR DRILL CYCLE)
G43H80G54.2P1

( ENTER Z LOCATION OF SURFACE +2" )
(Uses skip signal for safety and not Renishaw macro)
G1G31 F100.

#890=#5023 ( WRITE CURRENT Z )
M0
( MANUAL INTERRUPT )
( WATCH CNC SIGNAL AND TOUCH OFF PROBE TO SURFACE)
( THEN CYCLE START)
#891=#5023 ( WRITE SURFACE Z )
#801=[#891+ABS[#890]]+2. (WRITE Z SHIFT FOR STOCK )
#5203=#801
G1G91Z.02F50. ( ESCAPE Z FOR PROBE )
G1G31Z2.F100. ( SAFETY Z OUT )
G54.2P0G53Z0.
G91G0G28Z0
G30X0
G28Y0
G90
M00 ( YOU MUST RESET DATUM SHIFT BACK TO ZERO )
( WHEN YOU ARE DONE USING IT OR MAKE SCRAP )

You're still going to write it to the SHIFT column huh? <#5203=#801>
Which is OK... I usually try to avoid this in a program format but that's just me...

#5023 is the machine variable for current Z. It's always that. This and other variables are described in the EIA Programming manual. Look in the Macro section... should have a table showing this. Keep in mind that #5023 is the machine position but without the tool length in it. Since the macro in this case is only looking for position deviation, you don't care about the tool length.

There is another variable you can check out and that is #5063 which is the skip coordinate in Z. But I think that just retains the last machine position in skip so it may not help much here.

Make sure on this line you start at 2" above the theoretical Z or the math doens't work. If you change the start Z, you can change the math...
G1G31 F100.

What FP describes is another avenue but since you're still in G54.2 mode, you still can't probe. The only thing is... I'm not sure why you would start in G54.2 to set the work offsets.