G10 Work offsets, lean manufacturing

[roccet]

We are currently going through a revamp. Lean manufacturing is on the agenda. With that in mind

I would like to implement standard work offsets.

Its been a very long time for me. This shop does 99% of there work in vises and setup times are extreme and a killer. I am in the pursuit to cut setup times 75% I am currently trying to show/explain the benefit of standard offsets. I would like as much input from people that use standard offsets as possible.

We are currently going preset tool offsets manually offline and attempt to upload the offsets with each program we have not done this yet but plan to by the end of next week.

Thank you in advance.. and any advice is appreciated . Even if its just something you have tried.

[Rick Henrickson The Boeing Co.]

you tooling and documentation have to be in order but yes this is a great time saver, one way to really see where your setup times are being used is to video tape the operators setting up and what they are going to get, stalling because there are questions and the documentation is not clear. You need to make sure the jobs are kitted correctly and that you can repeat locations every time.

[Guest CNC Apps Guy 1]

Yes, it works and works well.

 

Below is how to write work offsets;

(WRITING TO G54 WORK OFFSET)

 

(L2 = G54-G59)

(P1 = G54)

(P2 = G55... ETC)

 

(L20 = G54.1P1-P48)

(P1 = P1)

(P2 = P2... ETC)

 

G90G10L2P1X0.0000Y0.000Z0.000

G11 (END WRITING PARAMETERS)

 

 

Writing to Tool Length Offsets

(WRITING TO TOOL LENGTH OFFSETS )

(FOR TOOL LENGTH OFFSET C... )

(USING POSITIVE TOOL LENGTH OFFSETS )

( )

(L10 = TOOL LENGTH OFFSETS )

(L11 = TOOL LENGTH WEAR OFFSETS )

(L12 = TOOL DIAMETER OFFSETS )

(L13 = TOL DIAMETER WEAR OFFSETS )

(P1 = H1 - H WEAR 1 - D1 - D WEAR 1 )

(P2 = H2... ETC )

(R = VALUE )

( )

(SAMPLE USES POSITIVE TOOL LENGTHS = )

(DISTANCE BETWEEN FACE OF SPINDLE... )

(... AND TIP OF TOOL )

( )

G10G90L10P1R9.9999

G10G90L10P2R9.9999

G10G90L10P3R9.9999

G10G90L10P7R9.9999

( )

G11 (END WRITING PARAMETERS)

 

Build up a model of you machine table and put your parts in "Machine Space" and you'll have a pretty close number right out of the gate for a work offset.

 

Try to use "library tools". Sit down with your programmers and figure out what the most common tools you use are and set from there i.e. T1 is ALWAYS a 2" Face mill, T2 is ALWAYS a 3/4" Rougher, T3 is ALWAYS a 1/2" finisher, etc.... GO from there and you can get to your goal of drastic setup reduction.

 

Use a common work holding method whenever possible (NOT a vise) and use common stock sizes. You can often get price considerations. If a good portion of your part are Material X and fit in a certain block, though you may have more material to remove on some parts than other, no biggie, you just machine it off, but it allows you to have a common work holding method.

 

There are lots of low-cost/no cost ways to reduce the time it takes to manufacture something.

 

HTH

[roccet]

This is GREAT feedback. I love it. thank you so much i hope to hear more. I completely agree with both of you its just much easier to be on the same page as others and not such a pioneer on this subject that has been proven out over several years. Any cost reduction is money in our pocket and savings to the customer.

[MLS]

+1 to standard tools in the machines at all times.

 

30 standard tools will machine probably 90 percent of the work assuming the type of parts you do don't fluctuate wildly of course.

 

Standardizing how you locate parts, where origin is set, etc. in programming can help alot too. If every program origin for every program is the same locating hole, or edge of a vise, etc. this will help too.

 

If you are using multiple vises an idea is to use prefabbed subplates with the vises already aligned and mounted. That way you can throw the sublplate on the table, pin and bolt it to the machine and go instead of spending all the time to align them.

 

Personally I am not a big fan of vises, but they do have their place. I'd prefer using technigrips for most operations on small parts. Start getting into mid to large parts(30 to 60 inches long and the rules change. Longer even than that and you can pretty much throw standard tooling out the window, but still design your tooling in a way that is consistent with how other parts in your shop are set up.

[Chris Rizzo]

Chk your email.

[chris m]

+1 for subplates; that helps eliminate a lot of edge-finding and indicating time picking up WOFS zero. If you know, within .030 or so, where the part is supposed to be, it makes things a lot easier. Personally I am a big fan of spindle probes for WOFS setting; you can use G10 to get in the ballpark and then probe the part or fixture [once] and be off to the races.

 

[ 08-04-2009, 03:11 PM: Message edited by: chris m ]

[roccet]

absolutely..

 

Big fan of g10. big fan of tool presetting.

not a big fan of vises

we have a prob on one machine looking into getting probes for all machines.

 

My personal experiences are with main and sub plates with about 10% of the work being vises.

This shop has 99% of there work setup in vises.

 

A bit of a challenge and baby steps are in order.

but the company is more than willing to expand there knowledge. So for me and the company its an open door for opportunity. I just have to get all my ducks in a row and help do this right from the beginning.

 

OMEP has been a great help but, we have a long way to go and are leaving a lot of decisions up to us.

OMEP is an organization that helps companies with stream lining manufacturing processes here in oregon.

[John Morris]

Standard set of tools is good start, we have 1-10 standard on all our mills, works out great. We have a spot drill, edge finder or probe (depending on machine), Drill chuck, 1/2 rough, 1/2 carbide finish EM, 3/4 Rough and finish, a facemill and square shoulder insert cutter. It's not uncommon to due an entire job but just adding a couple of drills and or taps and go.

 

As far as "going preset tool offsets manually offline and attempt to upload the offsets" , I cringed a little. If the measuring device is accurate and interfaced in some way to digitally send the information to the machine you should be fine. If you plan on having a human punch in numbers to the control I would run screaming from the room. One missed keystroke and you'll be crying.

 

All but one of our machines have tool measuring probes but even on the one that does'nt we measure each tool as it is installed and average time to install and measure a tool is less than 60 seconds.

 

As far as setup times being a problem do some studies as Rick mentioned, see where the real time bandits are and get a baseline before making changes so you can see real changes.

 

For example follow the tool prep all the way through on a couple of jobs and find out how long it takes. On average it takes us 4-5 minutes per tool to locate the tool (described on a tool list), find the appropriate tool holder, load tool in holder, load in machine and measure. All but the last step of loading in machine can be done while the machine is running. If the machine is sitting idle while this happening there is a huge issue that needs resolving 1st.

 

The work offset idea can be good idea, but again find out how long it takes to indicate, edgefind or probe your work coordinates before you make changes to procedure.

[roccet]

Thank you john you just answered several questions

clearer than i could and are currently meeting about those exact issues.

[Rick Henrickson The Boeing Co.]

Probing is great use it correctly many people get carried away it is still a machine tool not a CMM for lights out we pick specific tight tolerance places only to check not a full part eval.

 

I wish more and more shops would adopt this we need to take back being a country that can produce!!!!!

 

any help you need feel free to ask we can make parts in the US as cheap as anywhere else if we all do it right!

[chris m]

You don't need to confine your standard tools to just the tools that will fit in the carousel, either. We have many different 'common features' such as reamed holes, tapped holes, etc, but there are too many different combinations to fit all of the tools in our [20] or [25] station ATC machines. We have spent the money to buy collet chucks and collets to dedicate for these tools and leave them all built in a wagon next to the machine for quick loading. The tools are numbered and have a gage length inscribed that the tool must be set to when the drill / endmill / reamer is replaced; touch the tool off once when you create it, record the offset, and use G10 or variable setting in your programs from then on to avoid the operator touching off or manually inputting offset data in the machine.

 

Manual data input = thump

[latheman]

****************************************

any help you need feel free to ask we can make parts in the US as cheap as anywhere else if we all do it right!

*****************************************

AMEN BROTHER!!!!!!

[metalmilita]

CNC Apps Guy this works on our 4 offset column machine, but it doesnt on our 1 offset column machine. Same controller.. 16i-MB

 

It says improper G-Code.

 

Does it make a difference because it's not 4 column?

[Guest CNC Apps Guy 1]

Tool Offset C, is geometry and wear for Lentgh and Diameter/Radius. Not exactly sure what values to use on Tool Offset A. I've never used Tool Offset A. Always had B or C.

[DanaEd]

I sometimes use macro statements such as this.

 

#7021=-30.3738(WRITE G54 P2 X ZERO)

#7022=-17.9974(WRITE G54 P2 Y ZERO)

#7023=-19.7293(WRITE G54 P2 Z ZERO)

 

No operator error.

[Josh Kinney -Elite Engineering]

I have 3 Fadal VMC's (I know....) and I was thinking I could make a subplate with a location in the bottom right coner to pick up Fixture Offset #1. Then have pins in my Kurt vises to locate them. I would then have in MasterCam the subplates that are in each mahine with a vise installed. I can then toggle on and off different size jaw stock (2"3"4" tall) and cut my fixtures out of them. Setting my Origin at whatever point on the part I want to reference, this would be fixture offset #2. Now that my jaws are machined I can insert the part and proceed with the machining operations.

 

All the operator would do is have Fixture offset #1 permanetly set to the location on the subplate. When posting I could pull the difference between Fixture off set #1 and #2 and use that in a macro to set #2.

Operator throws the vise on the subplate, bolts on the specified jaw stock and runs the program.

 

My question is this:

 

This may work the first time you run that op but is it repeatable, and if so is it repeatable between machines using the same Jaws/subplate?

[Guest CNC Apps Guy 1]

The repeatability will be the difference between the two machines plus the difference between the subplates and fixtures added together... worst case.

[Josh Kinney -Elite Engineering]

So I guess this is something I should explore? How would I go about getting this information in my post?

 

I know what the code needs to look like but unsure how to get the data to fill:

 

N4#FX2=FX1+12.

N5#FY2=FY1+12.

N6#FZ2=FZ1+2.