Meldas CNC 5000 CII

[McRae]

I am implementing a system of offline tool measurement and want to generate a downloadable tool length offset file. The parametric nature of the fanuc lets the offsets fall into place simply but I have scoured the limited manuals that I have for the machine and can't find either a G10 or other method to access the tool offset register from a program. Are there any suggestions/solutions avail?? Sorry for the non-M/C related question but this is a collection of bright people.

MfgEng

[bryan.davis]

not familiar with your exact controller, we use a mitsibushi 625 which may or may not have similarities.

can you use variables on your controller, ie #nnn etc, if so then you should find that the variable number of the tool offset registers are listed in your manuals, if this is the case then your program for registering the tooloffsets would look something like below (variable numbers are made up)

O1001

#5111=123.456

#5112=456.789

#5113=741.258

ETC

If you can use variables, but cant find the appropriate numbers Ill look them up next week, Im fairly certain they would be the same as the 625, since the 625 is the same as the fanuc..btw this method works on fanucs too.

Alternatively do away with all ideas of offline toolsetting and use renishaw TS27 probing instead, that way you NEVER have to bother about a tool offset again!

[mcrae_andrew]

Renishaw Tool Probes - a machine tool makes an expensive CMM/Height Gauge.

[bryan.davis]

If you look at it that way then yes, but the advantage of the TS27 are that you NEVER have to worry about tool length offsets again, and you also bypass all of the uncertainty that goes along with tool length measuement.. ie has the tool been measured, has the measurement been read correctly by the operator, has it been inputed into the controller correctly.

Inspection probing can also been seen as an expensive CMM, but the point is you dont use it as a CMM, and besides by the time a CMM registers any fault or error in a part its more often than not too damn late!.

Where the MP10 pays is in setting up workpieces, especially if you have axis rotation on your machine and never have to spend the time bashing a 1 ton billet with a sledgehammer in order to clock it square. The second area it pays is in closed loop machining, or having your machine tool manage its own SPC completely automatically.

Combine the MP10 with the TS27R and you have 100% peace of mind in all matters relating to offsets, If I could have pocketed the past costs of each and every error made due to botched tool and workpiece offsets made by myself or my workforce I would be very rich now!

[mcrae_andrew]

bryan.davis - What type of components are you manufacturing? I can see the advantage of using the probe to set the work offsets and to do things internal to the process. Tooling and setup that can be moved offline is the end goal of a setup reduction project. What is your typical setup time with the ren.probe system?

Interested to know

Andrew

[bryan.davis]

We manufacture plastic injection mold tools up to 12 tons.

Typically we can be working on plates that weigh in excess of a ton, and sometimes we actually put an entire tool on a machine to do work that dosnt require stripping down, these jobs can weigh 7 tons.

for general jobs that can be held down with simple finger clamps out setting time is next to nothing. And to demonstrate this Ill describe a typical job setting scenario

1 job is lifted on machine bed

2 clamped down

3 operator measures distance between leader pin holes and diameter of holes using tape measure, these valuse are entered into parameters of our probing program (this is a custom program I developed, not renishaw standard)

5 probe is loaded from carosel and manually moved to approximately center of first leader pin hole about 5mm above top surface of plate.

6 press start button and let probe program run!

and thats it, the whole process can take less than half an hour! we dont need to do any tool length measurements, just put the tool in the holder and load it in the carosel, we dont need to spend an hour or so bashing about with a hammer to clock the job square as the probing tells us the angle error and we enter that value into a G68.

NOTE as policy we use leader pin holes on mold plates to descern datum, this makes sense when you consider that these features are consistant throughout all plates in any one tool. Ive also developed similar routines for picking up jobs from rectangular pockets, internal/external corners, circular features etc. the renishaw package gives you the basic tools for the job, but you need to spend a little time developing fully automatic routines to get the best out of it!

just today I set up a machine to spend the entire weekend machining 10 meters of 3mm ribbing slots 15mm deep, experience tells me that its going to break a lot of cutters and it going to be a complete bitch of a job, but with the TS27R Ive set the machine up to regularly check the tool for breakage, and if so load up a new tool, Ive got 6 cutters set up, so I only need to go visit the machine once a day to be sure Im going to get a lot of lights out machining done.

IMHO renishaw probing may make a machine an expensive height gauge and CMM, but a machine without ranishaw probing WILL spend a lot more time idle than one with!

[Tony]

Bryan

Thank you for your "Check for tool breakage "

tip with the TS27.

It is really nice to just run the Tool Magazine through the probe and GO!

Tony

[mcrae_andrew]

Bryan,

This is a great application case study for tool lengths made right on the machine tool. The Job Shop type application is where the offline tool setting, measurement, and offset file loading works best. For example, to machine a typical housing with holes drilled and tapped, milled features and bored diameters (Length and Diameter are set) and the tooling can be run on any of 5 similar types of machines (HMC or VMC depending on number of sides needing access). The thread started off with MfgEng looking for some type of a parametric access to the Meldas.

As a side, I am currently reading Mike Lynch's Parametric Programming and Probing Techniques. Good read and I hope to develop some of the probe cycles you mention.

Andrew

[Reece L Gibson]

I don't care if your running 100 ton part,you still have measure a new tool for the gage length offset to place it in the pot of the tool changer. And a Macro is locating the zero point of your part.

This was intoduced to me in the Mid 70's and is not uncommon.I teach pre-setups in our advanced course where we write the Macro to pick up the zero point of the work piece and store it in the fixture offset. It depends what enviroment you are in whether you have a 150 tool changer or just 20 pots. Any time a new tool is intoduced you have to measure it and get it in the control some how via RS-232 or by hand at the control,or through the program.

I show how to set this system up and manage it and can produce 5-10 min set-ups for what ever machine.

Back to your question the G10 function is a option but is always enabled. I works like this:

G90G10L2P1X-23.475Y-14.5467Z-12.7487

in this example L1=tool offset,L2=Fixture Offsets

L3=Parameters,P=fixture offset number P1=G54 P2=G55 so on If If you Use G91 it will add or subtract to the value this is currently in the offset bank. Every time the control read this line of information it will write the values the the proper offset bank so place this code in strategic place in the program. You can rewrite the fixture offset as many time as you like in the program

Hope this Helps

[Guest CNC Apps Guy 1]

quote:

---

I don't care if your running 100 ton part,you still have measure a new tool for the gage length offset to place it in the pot of the tool changer.

---

I would have to disagree to some extent. You do not need a precise measurement, just a rough one, +1.000 -0.00 is close enough for the initial tool length. Once it goes into the tool length measurement macro it then updates the value and moves on.

Here's an example macro that works on a Mori Seiki.

:9019 (AUTO TLM PROGRAM)

G00 G40 G49 G80 G90

G91 G28 Z0.Y0.X0.

G30 X0.Y0.Z0.

N100

T1

M6

M19(SPINDLE ORIENT)

G324 X1.Y1.B4.0H1F8.R3 T2

G91 G30 Z0.X0.Y0.

N200

T2

M6

M19

G324 X0.Y0.B9.5H2F8.R3 T3

G91 G30 Z0.X0.Y0.BO.

G90

M99

The M19 is to orient the spindle.

The G324 is the macro call, X and Y are offsetting the tool in case of a facemill for example to make you touch an insert not the cutter body. The B value is the approximate gage length of the tool. The H is the height offset to be written to. The R is the number of hits to take, and the F is the feed to move into the probe.

JM2C

[ 11-03-2001: Message edited by: James Meyette ]

[bryan.davis]

In actual fact you DONT have to measure a tool for a guage length at all!

I preceede the renishaw tool length probing macro with my own macro that does an automatic guage length measurement, when I say I can put any tool into any toolholder and put it into the machine without any concerns for its physical length I mean exactly that!

[Reece L Gibson]

Are using the machine to measure tool lengths on the machine? Many would agree that thats a waste of time, 5 sec is 5 sec,that wasting spindle time.

If you are running unmanned I can see this, but if you plan your tool life management right you do not use the machine to measure your tooling.

If you run lights outs or run castings I can see using the probe to pick up cords that thats about it

Hey James mail a copy of that macro,I would like to take a look at it

By the way how amny compatible "G" codes can be in one line on a Fanuc Control? In your example you have 4

[bryan.davis]

REF G codes, if memory serves you can have 1 gcode from each group (see manual for groups) on a single line, if you have more than one g code from each group then the controller will only act on the last one.

yes 5 seconds is 5 second, but 5 seconds is next to nothing when you are running a toolpath that has a runtime in excess of 100 hours.

Planned tool life management is OK if you are running batch production, and then only really if its fairly large batches of materials that are easy to predict, and with ideal toolsetups, a combination of criteria that Ive always found rare, but know do exist.

And dont write off probing on batch production too quickly, probing could indeed add 5-10 seconds to each tool operation and effectively add 10p to the cost of the finished part, but too often Ive had entire setups stuff themselves up because tool 1 broke, and tools 2,3,4,and 5 have smashed into steel that tool 1 should have removed with a resultant cost in excess of £500., or some 5000 probing operations!

And finally whats £1. worth of probing when you are working on jobs that are worth in excess of £5,000, Ive found that when working on high value jobs setters will take a LOT of time on ensuring setups are correct, however, a well set up probing system gives them the confidence to set and forget, as I previously mentioned, I can set up jobs in less than half an hour, without probing similar jobs could take 4-8 hours!

[Guest CNC Apps Guy 1]

quote:

---

And finally whats £1. worth of probing when you are working on jobs that are worth in excess of £5,000

---

That right there says it all. Probing is not for every application but for many applications it is sorely needed.

There are not 4 G-Codes on any line in the sample program. The most I see is two, G91 and G28.

As far as I know, as long as no codes conflict, there is no limit to the number of G-Codes on one line. On that note on my Mori Seiki SH-XXX's we have the ability to have multiple M-Codes on one line as long as they do not conflict.

The program I submitted is it, there's no macro, well I'm sure there is somewhere but that program is specific to Mori Seiki Machine tools with tool probing. The G324 activates a macro that is hard coded in the control (similar to how canned cycles are hard coded).

[ 11-04-2001: Message edited by: James Meyette ]

[Reece L Gibson]

Well James, yes there is a Macro and they hide it in the control so you can not edit it and screw it up. There is a parameter to let you edit this type of program which is in the 9000 program range(which is made by the company that makes the probe, Renishaw is one of the most common)They do not wanting you to see it or change anything in it for it can have an effect on how the machine will react. Most tool changes(M06) is nearly a macro being called by an "M" code. You can create your own "canned" cycles and give it your own "G" code of your choice.

One project is when you have a twin arm tool changer and you want to Re-run the same tool that is in the spindle over, most controls you have to start the program below the "M06" commnad for it will change the tool in the ready *** which is what you do not want. We re-write the tool change program to decide if the tool you are calling is in the spindle or not, there fore by passing the tool change. There is a lot of power is the control which very few are aware of.

Parametric programming was developed for the machine tool builders to access devices like your probe, they do not tell you these things.

[Guest CNC Apps Guy 1]

What I should have said, knowing full well what resides in the control is; the probing macro is not user customizable(sp?) 9XXX programs can be called by G-Code and those codes/program number are located in the Fanuc Parameter manual. I don't remember them off the top of my head. Many times when a machine tool is sold with a Fanuc control, the 9XXX programs are hidden so you need to enable viewing of them by parameter change. Don't remember what parameter that is either off the top of my head. That's why they make manuals, for when people like me forget.

We have mada a macro that when a tool change is called it Zero Returns the Z Axis before and it does a few other things.

[ 11-05-2001: Message edited by: James Meyette ]

[Reece L Gibson]

E-mail them to me ,I would like to see what they look like.

Should not be a problem should it?

[Guest CNC Apps Guy 1]

They are not user VIEWABLE either to the best of my knowledge.

So, no I can't e-mail them to you. Sorry.

[Reece L Gibson]

Can I get a copy of the Macro you made, you the zero return thing and some other stuff

I am always interested in how other people do things Please?????????????

[McRae]

To Clarify my origional post, the intent is to have an automated system using a presetter to measure tools offline, to have an offset file created by the presetter and then to have our DNC system send this information into the machine tool. While the Touch Probing and Length measurement macros are nice, the fact remains that each machine is still required to generate its own offsets. In comparison, the measurements that Bryan.Davis is making reference to would take longer to do than the operation itself (ie Spot Drilling) and so excludes itself from consideration (For My Example...) where it makes perfect sense for his application (>.001% of runtime).

The information compiled to date is fantastic and I thank everyone for their help. MillTurn - mcrae_andrew has mentioned a book Parametric Programming and Touch Probe Techniques for CNC Machine Tools - Mike Lynch Author, SME Publisher. Read this as it will help you develop your own applications.

MfgEng

[Reece L Gibson]

I agree with you MFG-ENG, I show how to use a electronic height master and measure tooling off line, (machine is still running the current job)store the offset values(positive numbers)in an ASCII file ,have the post import the ASCII file into the program using the G10 function and make a set-up cart with all the tooling ready and waiting for the person to assemble.

Works out very well,but takes strict mangement and is not for every shop. Sometimes it is not possible(need a lot of tool holders)and not feasable depending on the enviroment you are in.

This is an old agrument and to me it is your choice,It does not matter to me. All I do is simulate both enviroments and the student will have to adjust to what ever the current work place is doing.

As long as they are aware of the many different ways to set tooling on machining centers to prepare them for Industry.

[McRae]

Thank you all for posting such great responses and discussions. Bryan.davis, I should like to visit your shop someday as it sounds like you have a great system for lights out manufacturing.

Next topic should be the benefits of an FMS cell and all that relates to Quick Response Manufacturing and how we can apply Mastercam in that enviroment.

Again Thanks, Topic Closed

Mfg Eng