What's new
What's new

In a Speedio, how do I do a location verification in program.

Houndogforever

Hot Rolled
Joined
Oct 20, 2015
Location
Boring
I have a few parts that I want to locate visually, have the speedio grab the probe, locate and verify location and change G54 X-location in machine, then run the part.

I reckon this is simple like the tool breakage check, however for me, I'm a virgin and haven't done this before.

Thanks
Jon
 
Are you trying to test if a part is present and skip some operations? Or are you just trying to update your WCS for a part that doesn't locate dead nuts?

Renishaw 9810 cycle with an M and some logic will allow to to test for a part being present. I think the same cycle for Blum is 8703 with a T...?

Alternatively if you know the relative coordinates of your part you can probe normally and set a bogus WCS and use logic to compare the expected vs actual coordinates and use logic to do this or that; sometimes I prefer to set extra WCS so I can watch values change when proofing a program and make sure I'm not going to make sparks.
 
In this particular case, a part will be held in an Orange delta vise which will locate both Y and Z, however X would be set by a stop on the left or right end.
However I need to cut those ends too.
So I will know where it approximately is, and want the probe to modify my location and then run the program for that opp.
 
Are you set up to run the 700 series programs which call P8700 as the main macro or something else? Typically, you would set your work offset as normal, then in your program, call the probe with a tool change like an ordinary tool and tool offset (no spindle start), position the probe where you want it to start measuring and then add the X, Y, Z or bore or whichever cycle you want to use, and it will update the work coordinate each cycle.
 
I can post or email you the programs I use to do that in the morning if you want. I am using the probe macros I got for my Renishaw probe. I do this when I am running a few parts and don't want to probe manualy.
 
If just locating an X wcs update, this is what I use. You need to manually set the initial WCS of course. Also use it to check say 3-4 parts G54-57, duplicate this then add the S2, S3.... Make sure you have P8810 (protected position move) and P8023 and turn down the rapids and feed when initially testing. The Z2 at the end is height above part before I move to the next WCS.

G0 G80 G90 G54 G40
G100 G54 G43 T99 H99 X-.5 Y-.6 Z.25
(S1=G54)
(S148=G54.1 P48)
M402
G65 P8810 Z-.25 F10.
G65 P8023 A5. S1
M403
G0 Z2.
 
I probe all ops, all the time (pretty much). For Op 1, it makes sense to make sure the blank was pushed to the stop correctly, and might as well check it for size while you're at it. If you are probing for X location, you already have the data:
(THIS IS FOR BROTHER AND BLUM)
(TOOL CHANGE ETC DONE IN MAIN PROGRAM)
N1000 (PROBE OP 1 BLANK LENGTH)
G0 G90
G65 P8703 Z.25 M1
G65 P8700 X1 S2.8 Z-.5 W-1 M3 (PROBE X CENTER AND SET WORK OFFSET)
G0
G4 P.1
G4 P.1
G4 P.1
IF [#106 LT 2.78] GOTO1001 (IS BLANK TOO SHORT?)
IF [#106 GT 2.81] GOTO1002 (IS BLANK TOO LONG?)
GOTO 1003

N1001 (ALARM)
G0 G91 G28 Z0. (HOME SPINDLE)
G90
#1107 = 0 (TURN OFF PROBE RECEIVER)
G4 P.1
#1106 = 0 (TURN OFF PROBE)
#3000 = 1 (BLANK TOO SHORT)

N1002 (ALARM)
G0 G91 G28 Z0.
G90
#1107 = 0
G4 P.1
#1106 = 0
#3000 = 2 (BLANK TOO LONG)

N1003
 
G65 P8700 X1 S2.8 Z-.5 W-1 M3 (PROBE X CENTER AND SET WORK OFFSET)
G0
G4 P.1
G4 P.1
G4 P.1

I'm confused. Won't the M3 turn the spindle on with the probe in?

Also, what are the G4 P.1 lines for? I thought G4 was dwell. Why dwell 3 times?
 
This is the program I use to probe with. I like to do my moves with the machine coordinates vs using an offset to remove variables. Grab probe, move to the start point, call macro, maybe call M98PX to run the part program automatically if doing more than a few, then M2. Change the probe macros called according to what you want to probe. I am new to this so keep it simple. You could also insert this into the beginning of your part program.

(OUTSIDE WIDTH X OR Y)
G0G40G49G80G90G94
G100T22
G53X-14.76Y-10.03Z14.65
/G65P8700S7.8W54.X1Z-.5
M1(CHECK Y POSITION)
G65P8700S3.W54.Y1Z-.5
M2
 
G65 P8700 X1 S2.8 Z-.5 W-1 M3 (PROBE X CENTER AND SET WORK OFFSET)
G0
G4 P.1
G4 P.1
G4 P.1

I'm confused. Won't the M3 turn the spindle on with the probe in?

Also, what are the G4 P.1 lines for? I thought G4 was dwell. Why dwell 3 times?
In Blum speak, M1 turns the probe on, M3 keeps the probe on, and M2 turns the probe off. This keeps the probe from cycling on/off between every measuring move.

G4 lines are to keep the control reading over the macro stuff coming after them.
 
He still hasn't specified if he has Blum on Renishaw cycles installed...
The make of the probe does not matter, you can have a Renishaw probe and still run Blum cycles, he needs to provide that info before any of these shared cycles will be helpful.
There are manuals available for both, finding and reading the appropriate manual will probably be more helpful than being given a cycle and not knowing how to modify the alphabet soup to fit his needs.

OP, do you have a bunch of programs saved to memory 700-720 (ish) or 8700? If those programs have G65 P8700 in the first couple of lines you are running Blum cycles. P8700 is the master probe cycle, it will be followed by a bunch of letters that will do things like measure single or multiple points and set WCS, the manual explains how to do this pretty clearly so you can write a cycle to probe exactly how you want. 703 and up are templates for the different cycles available which you can examine and adapt for your needs as well.
 
Are you using a CAM package such as Fusion? Fusion has integrated WCS probing and it's quite straight forward to use.

Note that Blum integration was very poor (broken) in my post (Brother). I had to make quite a lot of fixes. You can see the changes I made in the change log.



If you want to see some more cool stuff you can do with the probe, see here for auto clocking the orientation of a round part:

 
Put an M159 in place of the G4 pauses; that is the Brother code for prohibiting look-ahed beyond that po
How do you turn it back on?
Manual says its a 'one-shot' code, is it just on to block lookahead for the following line and then lookahead automatically resumes?
 
That's correct

What's happening is that the control reads [a bunch] of lines ahead of the current position. It evaluates all the commands on those lines, which can have surprising consequences, eg if you store the machine location or current data in some variable, then this actually happens while the machine is still running an earlier command (so instead of reading the current location of the table, you would be reading it as it was several lines earlier). So if you absolutely need something to only be executed at the point the control reads that command, then stick an M159 in front of it. Broadly you only need this if you need this..

Its not clear to me that any M159 is needed in the referenced program though? (So this discussion is somewhat theoretical) Also the hard coded pause next to turning off the probe seems a bit brittle, there is a way to do an M2 call into the Blum programs and it has spaces in it for machine specific config, eg pauses. That would be preferred in general. However, if you are doing this in production, then the Blum macros are quite slow and conservative!
 
I know with the renishaw probing I have had some issues with look ahead (or at least that is what renishaw thinks) as the standard programs that come with the brothers have some issues.
 








 
Back
Top