What's new
What's new

Renishaw Inspection Plus

Mike Ortega

Aluminum
Joined
Aug 20, 2007
Location
Sunnyvale, Ca
Anybody ever used this software on their VMC. I'm using the general probing software on an 08' VF2SS. Just wonderign how the Inspection Plus works.
 
What info are you looking for? Inspection Plus software is the most common one out there for machine tool probing with Renishaw probes.

Just curious how it's used. Do you use templates like using VQC or do you load the geometry from your cam program and it inspects and compares to that?
 
Anybody ever used this software on their VMC. I'm using the general probing software on an 08' VF2SS. Just wonderign how the Inspection Plus works.
The measuring routines suppliled with HAAS are basic part only of Renishaws Inspection Plus. They do not include the Vector measuring ability and neither some special measuring cycles. In general Inspection Plus is set of macro routines resident in machines control. It can measure some gemetric features and store the results in variables or print out the report. If you are interested in generatig the measuring routines on your CAD model and then compare the measurd results with the model you will have to use Productivity+ or OMV packages from Renishaw.
 
Program probing

Some controllers come with built in macros that are called with a G65 PXXXX plus arguments. There are some third party suppliers that will come in and build the macros for you, at a cost. In Siemens PLM NX6 version, you will be able to program probing graphically.
 
Some controllers come with built in macros that are called with a G65 PXXXX plus arguments. There are some third party suppliers that will come in and build the macros for you, at a cost. In Siemens PLM NX6 version, you will be able to program probing graphically.

Do you have any more information on how they plan to program the probe? I'd certainly like to see the code it spits out.
 
I use MasterCam to program the Probe.... Most CAM systems can deal with probe programming one way or another, ... you just might have to be a little creative. Some systems have integrated capabilities or add-ons available for a more streamlined programming such as Siemens/UG or Gibbscam, etc.

You can do full inspection even with just starting from the Inspection Plus package. The only thing is you'll need to write some of your own macros or some simple math and comparitive functions to use it as an inspection tool. Inspection Plus is more of a "Verify" plus IMO but there is a lot that can be done with it. However, if you're looking more towards using like a CMM, buying the right software packages or paying an aftermarket company for macros would definately make things easier to deal with and pay for itself. Some of these can be migrated or packaged to CMM software such as PC-DMIS and such....
 
I use MasterCam to program the Probe.... Most CAM systems can deal with probe programming one way or another, ... you just might have to be a little creative. Some systems have integrated capabilities or add-ons available for a more streamlined programming such as Siemens/UG or Gibbscam, etc.

You can do full inspection even with just starting from the Inspection Plus package. The only thing is you'll need to write some of your own macros or some simple math and comparitive functions to use it as an inspection tool. Inspection Plus is more of a "Verify" plus IMO but there is a lot that can be done with it. However, if you're looking more towards using like a CMM, buying the right software packages or paying an aftermarket company for macros would definately make things easier to deal with and pay for itself.

Do you just have a post set up to call inspection plus macros? Or do you have it call your own home brewed macros?
 
Will the inspection plus software generated the needed macro programs or does a 3rd party have to create the macros programs the the inspection plus software will ask for?
 
You typically write a program that positions the probe and then runs the macro called from inspection plus to perform the actual calculations and update your offsets.

Here's a typical probed routine used to accurately locate the centers of some bores for the last op of a part. The entire routine is documented in the program notes and should be self explanatory. The part actually is finished with a tolerance of
-0.000 / + 0.0002" in thickness and parallelism, with the remainder + / - .001"
The actual probing routine uses O9810 (protected positioning move) from the Renishaw macros and O9814 (find center of bore measurement cycle). The offsets used to position the probe come from the setup in the machine and are touched off using the Renishaw Easyset macros.

O6515(ROBOGUIDES-LAST OP)
(SHARP SV6332)
(FINISH THE 3RD OP OF THE)
(ROBOGUIDES)
(FINISH THE ALUMINUM BRONZE)
(WEARPLATE SIDE)
(AFTER COOLANT PORTS HAVE BEEN)
(DRILLED)
( )
(VERIFIED BY STU JAN 2014)
( )
(THIS PROGRAM FINISHES 2 GUIDES AT A TIME)
(IN THE SHARP)
( )
(BOTH FIXTURES USE THE CENTER)
(OF THE GUIDE MOUNTING LAND AS)
(THE X0 / Y0 OFFSET LOCATION)
(BUT THAT IS HARD TO MEASURE ACCURATELY)
(SO THE X/Y OFFSET FOR)
(LEFT VICE USES G55)
(G55 X/Y OFFSETS ARE)
(NEAR THE MILLED WITNESS FLAT)
(ON THE LEFT REAR CORNER)
(OF LEFT HAND FIXTURE)
(+ 6.0964 IN X)
(AND -4.8839 IN Y)
(TO ROUGH SET THE CENTER OF THE)
(MILLED CIRCLE IN THE BORE OF GUIDE)
(AS G57)
(ULTIMATELY THE PROBE WILL SET)
(THE CENTER OF THE BORE AS THE)
(PART OFFSET, ACCURATELY WHICH IS)
(G57 FOR THE LEFT PART)
( )
(RIGHT VICE USES G56)
(G56 X/Y OFFSETS ARE)
(NEAR THE MILLED WITNESS FLAT)
(ON THE LEFT REAR CORNER)
(OF RIGHT HAND FIXTURE)
(+ 6.0964 IN X)
(AND -4.8839 IN Y)
(TO ROUGH SET THE CENTER OF THE)
(MILLED CIRCLE IN THE BORE OF GUIDE)
(AS G58)
(ULTIMATELY THE PROBE WILL SET)
(THE CENTER OF THE BORE AS THE)
(PART OFFSET, ACCURATELY WHICH IS)
(G58 FOR THE RIGHT PART)
( )
(FOR THE GUIDES MADE IN JAN 2014)
(G56 X WAS 11.2133)
(G56 Y WAS -16.2125)
(G56 Z WAS 6.6840)
( )
(G57 X WAS 37.3713)
(G57 Y WAS -16.1308)
(G57 Z WAS 6.6840)
( )
(THIS PROGRAM AUTOMATICALLY SETS)
(G57 AND G58 IN THE MACRO FROM)
(THE STORED G55 AND G56 OFFSETS)
(G55 AND G56 ARE REQUIRED TO FACE THE)
(FIXTURE PLATE BEFORE USE)
( )
(USE 22.25 X 10 X 2 INCHES THICK 6061)
(FIXTURE PLATES)
(MOUNTED HORIZONTALLY IN A PAIR)
(OF KURT VICE JAWS)
( )
(USE O6510 TO)
(MAKE A .003 SKIM CUT TO CLEAN)
(UP MOUNTING SURFACES AFTER)
(MOUNTING FIXTURE OR)
(CHANGING INSERTS IN)
(MIL-TEC DEDICATED FINISHER)
(TO ENSURE GUIDES ARE ON SIZE)
( )
(TO ENSURE THAT THE GUIDES ARE THE)
(PROPER THICKNESS)
(YOU SHOULD DETERMINE THE Z ZERO OFFSET BY)
(TOUCHING OFF THE SURFACE)
(WITH THE SAME MIL-TEC FINISHER)
(THAT WILL BE USED TO FINISH THE)
(MOUNTING PAD SURFACE OF THE GUIDES)
(SET THE Z OFFSET FOR 06510)
(FOR G55 AND G56 SO THAT THE)
(FINISHED SURFACE IS AT Z 0)
( )
(AFTER MILLING BOTH FIXTURES)
(LEAVE THE Z OFFSETS ALONE)
(THIS PROGRAM SETS THE G57 AND G58)
(Z OFFSETS AUTOMATICALLY BY)
(ADDING THE DESIRED GUIDE THICKNESS TO)
(THESE OFFSETS IN THE SECTION BELOW)
(WHERE THE MACRO SETS THE INITIAL)
(G57 AND G58 OFFSETS)
(THEN UPDATES THEM WITH THE PROBE)
(TO ELIMINATE POSITIONING ERROR)
(IN THE FIXTURE)
( )
(SHIFT THE Z OFFSET UP THE DESIRED)
(GUIDE FINAL THICKNESS)
(FOR THE ROBOGUIDES MADE IN JAN 2014)
(THE MACHINED PADDLE SECTION)
(SHOULD FINISH AT 1.422 INCHES THICK)
(SO THE OFFSET SHOULD BE SHIFTED UP)
(1.422 FROM THE G55 AND G56 OFFSETS)
(USED TO MILL THE PADDLE SURFACES)
(TO SIZE)
( )
(NOTE - THIS PROGRAM WILL AUTOMATICALLY)
(ADD THE 1.422 INCHES TO G55 AND G56)
(TO SET G57 AND G58 WITH A MACRO)
( )
(#5241 = G55 X OFFSET)
(#5242 = G55 Y OFFSET)
(#5243 = G55 Z OFFSET)
( )
(#5261 = G56 X OFFSET)
(#5262 = G56 Y OFFSET)
(#5263 = G56 Z OFFSET)
( )
(#5281 = G57 X OFFSET)
(#5282 = G57 Y OFFSET)
(#5283 = G57 Z OFFSET)
( )
(#5301 = G58 X OFFSET)
(#5302 = G58 Y OFFSET)
(#5303 = G58 Z OFFSET)
( )
(SET INITIAL WORK OFFSETS)
(LEFT PART - G57)
#5281=#5241+6.0964(G57 X OFFSET)
#5282=#5242-4.8839(G57 Y OFFSET)
#5283=#5243+1.422(G57 Z OFFSET=G56+GUIDE THICKNESS 1.422)
( )
(SET INITIAL WORK OFFSETS)
(RIGHT PART - G58)
#5301=#5261+6.0964(G58 X OFFSET)
#5302=#5262-4.8839(G58 Y OFFSET)
#5303=#5263+1.422(G58 Z OFFSET=G57+GUIDE THICKNESS 1.422)
( )
(CALL PROBE #1 TO SET BORE)
(FOR LEFT PART - G57)
(USES THE ROUND BALL STYLUS)
T30M6(CALL PROBE 1)
G0G90G57X0.Y0.(MOVE PROBE TO CENTER OF BORE LEFT PART)
(PROBE ON SEQUENCE)
M98P9021(PROBE 1 ON)
G43H30Z5.(MOVE PROBE TO 5.0" ABOVE WORK)
G65P9810Z.125F50.0(PROTECTED POSITIONING MOVE TO CENTER OF FIXTURE ALLOWANCE SCRAP)
G65P9814D4.0S4(MEASURE BORE AND SET G57)
G65P9810Z5.0F200.0(PROTECTED POSITIONING MOVE ABOVE PART)
( )
M1
T2(STAGE TOOL)
(USE PROBE #1 TO SET BORE)
(FOR RIGHT PART - G58)
(USES THE ROUND BALL STYLUS)
G0G90G58X0.Y0.(MOVE PROBE TO CENTER OF BORE LEFT PART)
G43H30Z5.(MOVE PROBE TO 5.0 INCHES ABOVE WORK)
G65P9810Z.125F50.0(PROTECTED POSITIONING MOVE TO CENTER OF FIXTURE ALLOWANCE SCRAP)
G65P9814D4.0S5(MEASURE BORE AND SET G58)
G65P9810Z5.0F200.0(PROTECTED POSITIONING MOVE ABOVE PART)
G91G28Z0.
(TURN PROBE OFF)
M98P9020(PROBE OFF)
( )
(MOUNT SAW GUIDE TO FIXTURE)
(WITH FIXTURE ALLOWANCE FACING UP)
(TIP OF GUIDE FACES TO THE RIGHT)
(SECURE THE GUIDE THROUGH THE)
(1/2 INCH DRILLED HOLES)
(IN THE SCRAP PLATE TO THE LEFT OF THE BORED HOLE)
(WITH A LARGE PLATE WASHER)
(THROUGH THE 1INCH COOLANT PORT HOLE)
(AND BOTH HOLES IN THE PADDLE SECTION)
(THE HOLES ON THE TOP AND BOTTOM)
(OF THE MOUNTING LAND SHOULD)
(BE LEFT OPEN SINCE THEY GET)
(THE FIRST COUNTERBORES MADE)
( )
(TOOL LIST FOLLOWS)
 
I put together a quick chart that notes the settings for the Renishaw Easyset macros for use in machines that don't have automated probing routines. On our Fanuc machines I assign M85 to call up the Easyset macros in O9023.

probe-easyset.jpg
 
Stuart -
Nice chart - any chance I could get a copy in a format I could edit for our machine?
Also, is it easy to map an M-code to a macro? Any quick hints how to do that? Would be handy instead of always typing G65 P9703...
Thanks - Jon
 
I never saw the Renishaw chart before, thanks! Of course the spindle is pointing the wrong way for my horizontal. You trying to confuse me? ;-)

Getting an M code that will run a program is super simple in a Fanuc control. Parameters 6080 - 6089 allow you to store an M code that is mapped to a 9000 level program from O9020 - O9029.

Lets say you have M85 that's not used for anything. You could stick 85 in parameter # 6080 and when you type M85 it will call program O9020. You simply rename easyset to program O9020. If parameter 6080 is used, try one of the others (look to find one with nothing in the parameter, it usually means it's available. ie. parameter 6089 calls program O9029.

Incidentally you can also map it to a G code if you wish Parameters 6050 - 6058 are mapped to O9010 - O9019 and work the same way.

I originally drew my chart in Corel Draw if that helps you out, I can give it to you in that format.
 








 
Back
Top