using MMC in probing

[landscnc]

We are probing 24 holes .420 +.004-.003 .004TP M. Any thoughts on adding the MMC into renishaw probing which does the TP only. The parts are round with 24 thru slots 1.5 thick and S.S.. They are moving at final machining and we need all the bonus we can get before sending data. We are using G65 P9823 since the slots run thru some holes and into all outter holes. We can only probe 3 points in all holes.

[Guest]

Moved to the correct forum

[Guest CNC Apps Guy 1]

YOu should be able to probe 4 points in a hole.

[landscnc]

YOu should be able to probe 4 points in a hole.

Not with 9823 but thats not the point. I want max material bonus

[Guest CNC Apps Guy 1]

In the past when I've needed the bonus tolerance like that, I've machined the feature over/under intetionally, then captured current wear offsets, re-write wear offsets and remachine using 75% of the tolerance available. I like to leave myself a little cushion just in case. Then probe again to make sure I'm still within tolerance. Then write the old offsets back.

 

HTH

 

 

[Ron Branch @ 5th Axis]

Well there is lies the problem. Renishaw is meant for collecting what you got. Trying to do something with it after words is the hard part. If you had Verisurf you could collect the data then bring that collected Data into the Mastercam file and we could show you the true position quicker than it took for me to type this message. You could try collecting it and using the macro variables to maybe store and average point of each feature. Then use the average point of each feature back to the nominal. Then make some spread sheet that does some math for you, but sounds like a lot of work. With Verisurf we would just take the points you got show the difference. Then you could best fit all the data back to the model and see the results real time on the part inside of Mastercam and done. With what you got will take some work.

 

Oh and do not forget the smaller you make the hole the more Max Material Bonus you got. The larger you make the hole the less Max Material Bonus you got.

 

HTH

[iowajim62]

They are moving at final machining and we need all the bonus we can get before sending data.

 

Are they moving or is the machine not holding position ? Might want to check that the machine isn't the culprit...

I have seen patterns of features out because of the machine before, and a round part with a circular pattern set of features would allow for the worst case to show the machines backlash/slop in both X and Y....

[landscnc]

Are they moving or is the machine not holding position ? Might want to check that the machine isn't the culprit...

I have seen patterns of features out because of the machine before, and a round part with a circular pattern set of features would allow for the worst case to show the machines backlash/slop in both X and Y....

No the parts are moving you can mic the O.D. and see it. We even rough, release, then start final finishing and they move some more. Its some crazy SS for nuclear work.

[McLaren]

Oh and do not forget the smaller you make the hole the more Max Material Bonus you got. The larger you make the hole the less Max Material Bonus you got.

 

That sounds backwards to me. Shouldn't you say that the larger the hole diameter, the more bonus you have? The position is based on Maximum Material Condition, not Least Material Condition. So you have a true position of .004" when the hole is at .417". With the hole at .424" you would have a true position of .011". Seem right?

[McLaren]

In any event it would be:

True position with MMC = True position result - (measured hole size - minimum hole size)

 

Or:

True position allowed = True position tolerance .004" + (measured hole size - minimum hole size)

 

Now I'm just getting myself confused. What number do you want?

[Guest CNC Apps Guy 1]

You guys are overthinking it. Ron, with all due respect, what is inspection going to do for him if he has to manually enter number comp numbers and re-machine the feature to get it within tolerance anyway? I'm guessing that he wants to automate this process, anything besides a probe system is going away from that automation.

 

Do this and be done with it already;

 

%
<PROBE-AND-REMACHINE-SAMPLE>(BORE DIA. CHK. AND RE-MACHINE)
(******SAMPLE CYCLE ONLY DO NOT RUN ******)
M0
M0
M0
M0
M0
M0

#190=1 (ORIGINAL OFFSET VALUES CAPTURED 1 = YES)

(NOTE: TOOL IN SPINDLE NEEDS TO BE CAPTURED...) 
(IN A MACRO VARIABLE <#516 FOR EX.)

(MACHINE FEATURE)
N1T1M6
G17
G5.1Q1
G0G54X0Y0S2500M3
G0G43Z5.H#517
G1G41D#518X07Y0F150.
(MACHINE FEATURE)
G40X0Y0 
G5.1Q0
G91G28Z0M5
G49
G90
M1

N101(CTR OF BORE TO CTR OF BORE TRUE POS.) 
T120(RENISHAW PROBE) 
M6 
G54 X0 Y0
G43H120 Z1.5
G90
G65P9023A1.D1.0 X0 Y0
G91G28Z0
G49

IF[#190LT1]GOTO111 (IF YOU DO NOT WANT TO RESET WEAR OFFSET PERMANENTLY GOTO LINE 111)

(ESTABLISH EXISTING RAD WEAR OFFSET VALUE)
#193=#[12000+#516] (DIA/RAD WEAR VAR CAPTURE)

(CHANGE DIAMETER COMP VALUE - WEAR)
N111
IF[#138GT.5099]GOTO9001(IF THE HOLE IS TOO LARGE - .5099 FOR EXAMPLE - PART IS SCRAP)
IF[#138LT.501]GOTO112(IF THE HOLE IS TOO SMALL - .501 FOR EXAMPLE - WE CAN USE TOOL COMP) 

GOTO12 (GO TO NEXT TOOL - FEATURE IS IN TOLERANCE)

N112
#12001[[#138-.500]/2](RAD VAR FOR TOOL 1 - AMT TO COMP - .500 = NOM TOOL DIA.)

GOTO1

G90 
M01

N12T12M6 (NEXT TOOL)
#190=0 (RESET ORIGINAL VARIABLES CAPTURED)
#12001=#193 (DIAMETER WEAR GEOMETRY VARIABLE RESET)

G17
G5.1Q1
G0G54X0Y0S2500M3
G0G43Z5.H#517
G1G41D#518X8.07Y6.11F150.
Y-6.11 
X-8.07 
Y6.11
X8.07
G40X0Y0 
G5.1Q0
G91G28Z0M5
G49
G90
M1


N9001 #3001=2(BORE TOO LARGE - OUT OF TOLERANCE)
M98P9901
M30

 

JM2C

 

: p

[landscnc]

Some holes on the machine kick out due to true position outage. Same holes on the Merlin CMM are ok with MMC added in. I want the probe on machine to figure in MMC. Will Verisurf figure it than send that data to our DNC.

[McLaren]

I've never probed on a machine, so I'm talking out of my a$$, but my guess is;

1. probe the hole

2. take the size and subtract the minimum hole size from it i.e. (.423-.417=.006)

3. add that into your tp callout (.004+.006=.010)

4. use the new value to check position.

[Guest CNC Apps Guy 1]

Actually mclaren, when you probe a feature, many characteristics get captured. Location, size, deviation, AND True Position. I'm sitting in SeaTac right now otherwise I'd copy and paste. IIRC, it measures TruePo @ RFS.

 

HTH

[Guest CNC Apps Guy 1]

Landscnc, it would probably not be too difficult to calc @ MMC. Just do a formula with the variable output table measurements and go from there.

 

HTH