Probe question again...

[bassn_07]

It's been about a week after my first introduction to probe training on my Mazak 5 axis. I already love this thing, for example, there has been a part that usually takes 2 to 3 parts to get it right due to tight tolerances. Not to mention the time it took to have the inspectors check it. Now with the probe I nailed it on the first part, truly awesome. There is one question I have for the probing guru's out there, is there a way to add the deviation to my G10 program? I always use two programs, 1 is my G10 program and the other being my main. This the way my post outputs the programs and I like it, but I would like to write the deviation automatically. Make sense or am I just talking out of my a$$? Any help would be appreciated.

[crazy^millman]

Are you talking about G10 for position deviation? Are you talking about for tolerances in the probing operations to the relative part? Can you be a little more specific maybe be some sample code???

 

HTH

[bassn_07]

Yes, I'm talking about G10 for position and deviation. As for the tolerances, I would like to take the probing tolerance deviation from nominal and add or subtract that difference to my G10 lines. Here's a sample code with a few added notes. I'll add info to what I'm trying to achieve.

 

O14605341(M6-146053-OP3-G10)

(MAZAK VERIAXIS 630-5X)

(MACHINE NUMBER---)

(PALLET NUMBER ---)

(TORQUE VALUE ---)

(PART NUMBER ---)

(PART NAME ---)

( ---)

(PROGRAM BY ---)

(DATE - 20-12-07 TIME - 11:44)

(PROVEN DATE ---)

(CYCLE TIME ---)

 

/7GOTO6666

M00

N6666

 

G0G90G17G20G40G49G80G94

 

(TOOL OFFSETS)

G10L13P11R0

G10L13P164R0

G10L13P163R0

G10L13P13R0

 

G10L13P25R0 I would like to add a value to R value. I was thinking of something like this but not sure. R#800 / I would right my probe deviation to this variable.

 

 

G10L13P32R0

G10L13P40R0

G10L13P109R0

G10L13P64R0

G10L13P52R0

G10L13P65R0

G10L13P179R0

G10L13P166R0

G10L13P54R0

G10L13P178R0

G10L13P161R0

G10L13P68R0

 

G10L13P73R-.0001(.2382 FACE HOLES R0)

G10L13P273R-.0008(.2382 SLOT R-.0007)

G10L13P53R-.0004(SIDE HOLES EXCEPT DEEP ONES R-.0003)

 

G10L13P169R.0006

G10L13P86R0

G10L13P69R.003(.236 DEEP SIDE HOLES = R0)

G10L13P111R0

G10L13P172R0

G10L13P42R0

G10L13P173R0

G10L13P174R0

G10L13P170R0

G10L13P171R0

G10L13P35R0

G10L13P29R0

G10L13P36R0

G10L13P180R0

G10L13P175R0

G10L13P17R0

 

G10L11P11R0

G10L11P164R.002

G10L11P163R-.016

G10L11P13R.0019(R.0019)

G10L11P25R.0032

G10L11P32R0

G10L11P40R.015

G10L11P109R0

G10L11P64R0

G10L11P52R0

G10L11P65R0

G10L11P179R.005

G10L11P166R0

G10L11P54R0

G10L11P178R0

G10L11P161R0

G10L11P68R0

G10L11P73R0

G10L11P169R0

G10L11P86R0

G10L11P69R0

G10L11P111R0

G10L11P172R0

G10L11P42R0

G10L11P173R0

G10L11P174R0

G10L11P170R0

G10L11P171R0

G10L11P35R0

G10L11P29R.003(DATUM -D- =R.0028)

G10L11P36R.008

G10L11P180R.010(3/4 L SPOT)

G10L11P175R-.001

G10L11P17R0

 

(WORK COORD OFFSETS)

G10L2P0 X-12.4015 Y-12.4015 Z-27.1666

 

G10L20P2 X.0011 Y-.0005 Z-.0024

 

G10L20P3 X.0029 Y-.0011 Z.001 (DATUM-A-)

 

G10L20P4 X-.003 Y-.0020 Z0.

 

G10L20P5 X0 Y-.0008 Z.002 (DATUM-D-)

 

G10L20P6 X.0029 Y-.0011 Z-.0012

 

G10L20P7 X0 Y-.0008 Z0.

 

G10L20P8 X0. Y0. Z-.0013 (DATUM -F-)

 

 

G90

M98P14605343 (MAIN PROGRAM)

M0

 

G90

M98P6054 (PROBE CHECK)

M0

 

G90

M98P14605344 (RE-RUN T13 AND T29)

(PROBE WILL WRITE DEVIATION TO Z IN P3 AND P5)

M0

 

G10L2P0X0Y0Z0C0A0

 

G90M30

[Greg Williams]

Can you have the probe update your tool offset?

[Greg Williams]

Can you have the probe update your tool offset?

[crazy^millman]

Bass Where do you now currently get all of this information from?? Specifically do you get this out of the machine or out of Mastercam? The thing I am trying to understand is are you measuring a casting or forging and then taking the difference of that from where you expect it to be and then adjusting your program to run?? Are you measuring a machine parts and then adjusting for variance in where it should be to where you need the program to run?? Expanding on the last in other words are you programming from center line in Mastercam and once you get to the machine you are having to adjust for differences or are you programming from faces and needing to adjust according to where that face is falling in at on the machine??

 

Deviation can come from many different places and sorry, by reading the G10 line you put out there you did not get across to me where you are seeing it, how you are seeing it and then how you are using the probe to measure and then adjust to those changes. I do know G10 line commands off the top of me head to know what each specific one is doing as well. I get the fixture offset one, but I would think you would have some math in your macro here that would take the measure position and then compare it to a know position then do a adjustment off of that result to then either shift the work offset or adjust the tool offset according to what you are trying to accomplish again deviation can come from anywhere and I just can see with the little bit of information you have provided how you are handling it and then using it from that point.

 

Edit:

 

Ok I see where you have many work offsets so this leads me to think you are measuring a bunch of faces then you are machining each one of those faces using work offsets if this is the case this goes well out of the way I program parts. I would measure a face then I would look ot adjust the tooloffset to remachine that face. I assume you got all of the Renishaw macro cycles with this probe. So if you are machining Datum Z you could take a cut to .005 above the surface in your program. You could then do a single surface measure and use .005 as the expected amount. You would then measure that surface if the surface was off .0005 then the tooloffset would be adjusted by .0005 and then you would run the finish pass to hit that surface dead nuts. I have done this on a few projects, but a lot of people hate to see a tool run part of the operation, and then come back probe it and then finish the rest of the operation. What I see what people like is to finish the part leaving everything heavy by a couple thou then run a probing routine and then adjust the tool offsets from there. If you have some really tight face or areas you are trying to hit then the cut heavy, the measure, then finish cut should do what you are after without adjust work offsets. I would then have a known length I would G10 in at the top of my program that you know will always cut heavy for the finish tools and then I would make it where every part was finished this way.

 

Simple statement would be:

#800 = 12

#801 = 12.4576

G10P#800R[#801+.005]

 

This is if you are using Type A for your tools, which it looks like you are using Type B for your tools so then it falls under that and if using type C then it falls under that. To hopefully answer that question above about related to the R value.

 

End of Edit:

 

 

Sorry I can not be of more help.

 

[ 10-11-2008, 01:43 PM: Message edited by: Crazy^Millman ]

[iowajim62]

Rons guesses are good ones and he looks to be on the right track to helping. However like him, I'm lost on the tool and cutter comp G10's.

G10L20P? is your work offsets

G10L11P?R? is tool length

G10L13P?R? is cutter compensation

Is this right ? If so, the next question is.

Are the tools resident or do they get changed for each job ? I'm guessing they stay by the higher numbers I see above. ie G10L11P180R.010(3/4 L SPOT)

If that is the case then next would be that I will recommend that you leave tool and comp adjustments in the machine and adjust programs as needed not the tools. Your probing should adjust the position of the part/workoffsets to give you a good part. And a much easier way to program.

 

Sample of how I program probe for 4 parts on horizontal tombstone with resident tools.

 

(3XX ITEM 2 PRE-BRAZE-MILL-OP)

(X0Y0=CENTER OF PART)

(Z0=TOP OF PART)

(T37 .515 33/64 HSS JOBBER DRILL)

(T08 1/2 3 FLT ENDMILL 1.5 LOC .03R)

(T49 .375 3 FLT CARBIDE E.M. 1.0 LOC)

(T39 .25 3 FLT CARBIDE E.M. .75 LOC)

(T24 1/4 X 90 DEG SPOTDRILL)

(T25 .173 # 17 HSS DRILL)

(T51 .1495 #25 HSS JOBBER DRILL)

(T52 .1875 CARBIDE REAMER)

(T53 .1562 CARBIDE REAMER)

(T55 .1875 3 FLT CARBIDE E.M. .375 LOC)

(T50 .25 3 FLT CARBIDE W/.03R .75 LOC)

(T33 .25 CHAMFER MILL)

(T21 1/2 X 90 DEG SPOTDRILL)

(T65 .4375 7/16 HSS JOBBER DRILL)

(T40 .203 HSS JOBBER DRILL)

(T20 .02 ENGRAVING TOOL)

(*)

(SERIAL NUMBER CONTROLLED BY H505)

(PARTS COUNTER CONTROLLED BY H506)

IF[#10505GT#10506]GOTO9990

(*)

M1

G90G10L20P31X0.Y15.407Z9.600B0.

G90G10L20P32X0.Y15.407Z9.765B0.

G90G10L20P33X0.Y15.407Z9.600B0.

G90G10L20P34X0.Y15.407Z9.765B0.

(*)

M1

G0G28G91Z0

G0G17G40G80G90

N76T76M6(MP700 RENISHAW PROBE)

M22(UNLOCK)

G0G54.1P31G90X0.0Y0.0B0.

M21(LOCK)

G43H76Z8.

T37

G65P9832(PROBE ON)

G65P9810Z1.F100.

G65P9814D12.68Z-.3R0.2S131(SET P31 X0Y0)

G65P9810X-3.5Y0

G65P9811Z0S131(SET P31 Z0)

G65P9810Z4.

G0G28G91Z0

M22(UNLOCK)

G0G54.1P32G90X0.0Y0.0B90.

M21(LOCK)

G43H76Z8.

G65P9810Z1.F100.

G65P9814D10.14Z-0.2R0.2S132(SET P32 X0Y0)

G65P9810X-2.5Y0

G65P9811Z0S132(SET P32 Z0)

G65P9810Z4.

G0G28G91Z0

M22(UNLOCK)

G0G54.1P33G90X0.0Y0.0B180.

M21(LOCK)

G43H76Z8.

G65P9810Z1.F100.

G65P9814D12.68Z-.3R0.2S133(SET P33 X0Y0)

G65P9810X-3.5Y0

G65P9811Z0S133(SET P33 Z0)

G65P9810Z4.

G0G28G91Z0

M22(UNLOCK)

G0G54.1P34G90X0.0Y0.0B270.

M21(LOCK)

G43H76Z8.

G65P9810Z1.F100.

G65P9814D10.14Z-0.2R0.2S134(SET P34 X0Y0)

G65P9810X-2.5Y0

G65P9811Z0S134(SET P34 Z0)

G65P9810Z4.

G65P9833(PROBE OFF)

G0G28G91Z0

M1

(*)

G0G28G91Z0

G0G17G40G80G90

N37T37M6(.515 33/64 HSS JOBBER DRILL)

M22(UNLOCK)

G0G54.1P31G90X-.13Y-.06B0.S1600M3

M21(LOCK)

G43H37Z1.M8

T8

G83G98X-.13Y-.06Z-.695R.1Q.2F6.

G80

G28G91Z0

M22(UNLOCK)

G0G54.1P33G90X-.13Y-.06B180.S1600M3

M21(LOCK)

G43H37Z1.M8

Z.1

G83G98X-.13Y-.06Z-.695R.1Q.2F6.

G80M9

G28G91Z0M5

/9G65P9863H-.02(TBC)

M1

(*)

(ROUGH .3185 C/BORE)

N8T8M6(1/2 3 FLT ENDMILL 1.25 LOC .03R)

G0G28G91Z0

G0G17G40G80G90

M22(UNLOCK)

G0G54.1P31G90X-.13Y-.06B0.S9500M3

M21(LOCK)

G131R5(AI-NANO LOOK AHEAD ON)

G43H8Z1.M8

T49

M115

M98P1301

G130(AI-NANO OFF)

G28G91Z0

M22(UNLOCK)

G0G54.1P33G90X-.13Y-.06B180.S9500M3

M21(LOCK)

[crazy^millman]

Jim if you are constantly moving the part to adjust things how do you keep them all in relation to each other?? If you are doing one side on one offset and then you have dimensions related to that side wouldn't you have ot then probe that surface after it is machine ot get the other feature in relation to that. By probing the machined surfaces and machining them in the correct position on a 5 axis machine you then have less of a risk of losing true position requirements on the part. It I am machining 4 sides on a part on 4 or 5 axis machine I always program using one work offset. Then adjust the tools to make the part right now move it 10 ways to get the part right I am worried it will loss some locations and possbily scrap the part.

 

I can see the flip coin of that is well what if one side cut .002 heavy and the other side cuts .005 heavy if you adjust for the .005 side you scrap the .002 side. That would tell me there is something wrong with the machine, set-up, or tooling, and in that case you would have to do as you are saying probe each index position before machining and then machine that index position then index machine probe that position then machine and so forth again I think a lot of wasted movements. If the machine is dialed in and the tools cutting the way they should then using many different work offsets for many different indexes just seems odd to me is all.

 

Again just my 2 cents for what it worth.

[iowajim62]

Ron,

Yeah I follow what your saying about updating the offsets for 1 part after machining from one face and then updaating offsets for the other faces. I was showing a sample of probing for 4 parts with one on each face of the tombstone. Again I agree with you on how to machine a single 4 or 5 axis part with multiple work offsets adjusted after machining from the initial work plane/face. I would want to keep the tools length and comps set/adjusted in the machine and use the probe to only update work offsets. As tools wear you adjust them in the machine.

 

I think were on the same page and you were thinking I was talking about 1 part not 4.

 

Hope that is clearer. And for what its worth, I always read and learn when you write or speak.

 

Oh yeah Congratulations on gettin Published

 

Here's what I'm talkin about Ron

 

[crazy^millman]

Yeah Jim that fills in the missing piece of the puzzle for me and since he is talking about a 5 axis machine I have been thinking along the lines of a single part not multi-parts and if that were the case then I would do as you are saying as we both agree on that. Adjust the work offsets for each face as need be, then adjust the tool offsets to make each part correct. It did not enter my thought process you were giving an example for parts of different faces sorry about the confusion.

 

Jim I learn things as I try to explain things to others. You sometimes just do things becuase they seem right, but the thing I like about this place is I have to slow down and think about what I am saying and in the process either confirm or prove things wrong I did or do. When we quit learning we need to go do something different becuase when we think we know it all, we really know nothing.

 

quote:

---

As tools wear you adjust them in the machine.

---

This is where I was talking about the single surface adjustment of tooloffset. It you are running lights out and want to make good parts without having an operator there this is part of the missing piece of the puzzle. You can even go as far as writing support in the program that if the surface devation adjusts to much the tool is then changes to a back-up tool. some people have tool life managment features on their machines. What do you do when you do not have this? Well you can write Macro logic in the post to support this.

 

#14 = 20

T#14

if #800 > .01 THEN GOTO 1000

N1000 [#20 + 20]

So if the vaule collected through a measure grows bigger than .01 then the program will adjust the tool by 20 to the backup tool and keep running. Now I would have some work with sub programs and main programs so that I defined everything in my main and would run subs as my light out operation. Tool detection would be a must as well.

 

 

[bassn_07]

Millman,

 

Thanks for the detailed response. I'm still very new to both the 5 axis and Mastercam, I've only been doing this for a few months. Also, before my training last week I've never used a probe. This is why I'm having a hard time explaining exactly what I'm trying to achieve. I do appreciate you taking the time to decipher what I'm trying to explain

 

quote:

---

Bass Where do you now currently get all of this information from?? Specifically do you get this out of the machine or out of Mastercam?

---

This is all from Mastercam with a few edits. This is a post that was modified by previous programmer and it work very well.

 

quote:

---

Are you measuring a machine parts and then adjusting for variance in where it should be to where you need the program to run??

---

Yes, I'm machining the part and leaving material on areas to be checked with the probe. After checking I write the deviation to appropriate offset and re-run the tools tied to that operation. Most parts we do on this machine are very expensive tight tolerance parts that require a lot of care.

 

Here's a probe program I wrote that checks the distances from a datum feature. In this program I'm attempting to check the distance and have the deviation added or subtracted from the appropriate offset. In this case it's my Z value in both P3 and P5 extended offsets in my G10 (at least that's what I call it) program.

 

This program worked very well for what I was trying to do, it may not be the best but it's one of my first ones. One thing I was trying to do, which was the main reason of my post, is measure a web feature that has been roughed out and write that deviation to my R value on my G10L13P25R0 listed in the program. Once again I'm sorry if I can't get my question across but this is a definite learning experience I'm going through right now. Thanks again for time and patience.

 

M6T71

M19

M1

M46

M43

G0G54.1P20G90M9

( PROBE WITH 3MM STYLIST)

C0.A0.

X2.1142Y1.5307

G43H0Z9.

G65P9810Z7.3F25.

G65P9814D.238H.0003 (.238 BORE)

#550=#133

#551=#143

G65P9834

G65P9810Z9.F25.

G65P9810X3.Y-5.2087F50.

G65P9810Z7.3F25.

G65P9811X2.5079 (CHECK DATUM -B-)

G65P9834X.3937H.0005 (.3937 +/-.0005 DISTANCE AND TOLERANCE)

#552=#138

#553=#141

G65P9810Z9.F50.

#143=[#-143]

#7083=#7083+#138

G65P9810X-3.2874Y7.5F50.

G65P9810Z7.7F25.

G65P9811Y7.0079F50. (CHECK DATUM -A-)

G65P9834Y5.4471H.0005 (5.4471 +/-.0005 DISTANCE AND TOLERANCE)

#554=#138

#555=#143

G65P9810Z9.F25.

#143=[#-143]

#7043=#7043+#138

G0G28G91Z0

(CHECK 140MM = 5.5118)

G90G0G54.1P21

C0.A-90.

X3.937Y-6.949

Z8.

G65P9810Z7.F50.

G65P9810Z4.9

G65P9814D.236 (.236 BORE)

#556=#133

#557=#143

G65P9834

G65P9810Z9.F50.

G65P9810X9.4488F50.

G65P9810Z4.9

G65P9814D.236 (.236 BORE)

G65P9834X5.5118H.0005 (5.5118 +/-.0005 DISTANCE AND TOLERANCE)

#558=#138

#559=#141

G65P9810Z9.F50.

G0G28G91Z0

G0G28G91X0Y0

G28A0.C0

M99

[crazy^millman]

No problem trying to help you out here. It looks your machine has the Renishaw probing cycles. These can be your best friend for the things you are trying to accomplish.

 

Take the single surface probing. If you do a single surface probing and tell it the tool then it will update the tool offset by the difference. Well you can do the same thing with a web measure. You could write a macro that takes the measured distance and then uses the know difference to come up with the deviation and adjust the wear offset by the amount desired and have the machine do all of the adjustments without you even touching the screen. Expensive sounds fun, like $80k a piece casting??? I can see your caution and that is a good thing. I am always weary of making mistakes and hate it when I do. I am not perfect, and run from those that say they are. You have the right attitude and approach with this problem. Sounds like you got a good post from someone who knows what they were doing when they set it up. The best advice I can give you is make a dummy part and practice on it. Make up some features and do all your experimentation on that. Then when you get it all figured out you have something you can trust.

 

May seem impossible, but if you present this in a way to the current management to understand this helps them, the company, and of course you then will be on board to make it work in a more practical way.

 

T is the control in those cycles for tools. You can also extract Data from the cycles and use it for things. Do some reading on the cycles and see where and what you can pull out of them to use how you need to make the thing do like you want. You have some good ideas hardest thing with most ideas is getting them to work the way we want, that is what separates those of us from the talking about it people to the doing it people.

 

Oh BTW your work on this section of code looks spot on.

[bassn_07]

Thanks Millman. Like you mentioned, I have many ideas but getting them to work will take time and patience. We use a Renishaw MP700 probe which is supposed to be a high end one and my end goal is to fully utilize it. My machine has 6 pallets and tons of tight tolerance work that will be utilizing the probe. For example, before the probe we had a job that always takes some time to dial in (.0012 true position) and at times it would cost us a part. On this last run I utilized the probe and nailed my first part...very rewarding.

 

As for the offsets, since we run many pallets we always offset in the program due to total control over every tool being used in multiple parts. This is why I would like to take the probe deviation reading and add it my program instead of my machine offset. Lets say I would like to write to a R value in my program and wrote my probe deviation to macro variable #800 = (.0005 deviation). My R value would look like this - G10L13P25R0 and I would like that R value to read macro variable #800, would be as simple as R#800 and to throw more confusion into the matter I would need to divide that by 2. If all this sounds lame please excuse the ignorance but I just would like to know how far I could go with this probing thing.

[iowajim62]

bass,

 

quote:

---

We use a Renishaw MP700 probe which is supposed to be a high end

---

Yes this is the better one. It uses strain gauge sensing technology. Very Nice

You may want to check on whether or not it was calibrated with O9803 or O9804 (Chapter 6 in the manual) if you have any issues with accuracy. O9804 uses 12 points instead of 4.

 

quote:

---

My R value would look like this - G10L13P25R0 and I would like that R value to read macro variable #800, would be as simple as R#800 and to throw more confusion into the matter I would need to divide that by 2

---

try this for dividng by 2

 

#800=[#800/2] then this

G10L13P25R#800

[bassn_07]

Thanks Iowajim. I referred to the manual on 9804 and it's listed for Calibrating on a Sphere. If I did have the option to use 12 points over 4 I would definitely use it.

 

Thanks for the info. I'll be doing some testing tomorrow.

 

One more question if I could, when I use T in the macro does it actually update the tool offset or the wear in the Z axis?

[crazy^millman]

Yes if you use the T it will update the offset of the tool. You can write your own logic to have it update the wear.

 

HTH

[iowajim62]

Bass,

 

Yeah O9804 is to calibrate on a ball very nice for 5 axis but you don't have to. The O9801,O9802,O9803 is fine.

 

As far as I know T is the tool offset not the wear value for all the probe macros. (Chapter 3)

 

My manual is H-2000-6137-0A-B. These macros haven't really changed since I started using Renishaw probes back in 1996. There was a revision in 1998. What manual do you have ?

[bassn_07]

Iowa,

 

I have the exact same manual as you. I also have something called Easy Plus. It's something my trainer loaded, it simplifies the basic probing moves. I really don't use it though because I'm needing something more than the standard probing moves.

 

I tries something on Friday that worked quite well. I was attempting to hold a 15" long feature parallel to my Datum surface (.0005 max). One part would be decent and the next a little bit out. What I did was indexed the A axis (trunnion) @ 90 and cut the my Datum surface. Then I indexed back to A0 at C180 and used Macro 9843 to get that surface parallel to my X axis. I then wrote that angular difference to the appropriate offset and indexed back to A-90 without moving my compensated axis and cut the side opposite to the Datum surface. The next few parts turned out dead nuts, then I went home on a good note. Is this overkill? The whole probe procedure added about 10 - 15 minutes to the cycle time but for a $3,000 dollar part I think it's worth it. Hopefully my discription is good enough to understand. I'm just excited with my new found tool and would like to utilize as much as possible to reduce our scrap ratio on the tighter tolerance parts.

[crazy^millman]

Well I tell people this about scrap. It cost 3 times the part to get back to where you were. It is the cost upfront, the cost to get to where you are, and the cost of time you could not put on the next job. So if you scrapped 3 of those it would cost your company $27k Yeah I think 10-15 minutes is perfect, and tell anyone that says it is not to get out the $27k and you will do it their way.

 

Good job like to hear stories like that!!!!!

 

What part of the country are you in BTW.

[iowajim62]

quote:

---

The whole probe procedure added about 10 - 15 minutes to the cycle time but for a $3,000 dollar part I think it's worth it.

---

that's exactly what probes are for

 

15 minutes on a machine that is prolly quoted at $100-$150 per hour and possibly as high as $200 per hour works out to $25-50 per part. i would say that is time well spent when it's a $3000 part.

[bassn_07]

Millman,

 

I'm from San Jose, Ca., just like Iowajim62.

 

Iowajim62,

 

I just noticed that we are from the same city, what a small world.

[crazy^millman]

I am in Brea, Ca. I am a transplant from Florida.

 

Yeah I have met a few members from the board over the years. Good luck with all of this and sometimes we have to stand our ground and if we can produce result most people will see it our way. If we are full of horse pucky then they will not.