Job Shop guys, do you have any logic to your tool numbers?

As I begin to outfit my VMC I'm wondering if I should start with a tool numbering system rather than just haphazardly loading them.

I was thinking a system of 4 digit numbers like so- first digit tool type, second digit holder type, 3&4 would be tool descriptors like size and flute length?

Tool 1104 might be an edge finder in a solid holder, or 2206 might be a 3/8" end mill in a collet.

Is this worth a hoot, or am I over-thinking it?

The way we do it, (not the best and not really organized) is any special tools that would need ordered just for that job go into a job box for that part (all out parts are numbered so it’s easy to find). Sometimes it’s just a metric drill, others, a handful of special endmills.


Sent from my iPhone using Tapatalk

I tried to do some kind of organization when I first setup my VMC but found it to be very difficult to be consistent across different setups.

Now, I simply reserve certain tool numbers for tools that I typically use on every job. I.e., edge finder is T15; 1.25" face mill is T1; center drill is T2..etc.

The rest are just swapped out as needed.
gm

I find it pretty tough to have any standardization WRT pocket #'s if that's what you mean. Other than 3D taster in #21 and facemill in #1, it's all over the place. Most jobs start with a rougher in #2 then the first finisher in #3, but sometimes I need to predrill for corners so it's spot drill in #2 then drill in #3.

Regards.

Mike

I’m not as experienced as most, but I have my probe in 1, face mill in 2, 3/8” EM in 3, 1/2” EM in 4. Then my spot drill is 9, drill 10, tap 11, chamfer 12. The others get swapped as needed. The tools in 2-4 get swapped between AL and steel tools as needed, but same sizes. This basic numbering helps make programming easier on me.

Not sure I would bother with any "system" per say, as like others have said, it's hard to carry through from job to job, year after year etc. What you might consider is being consistent when programming a "family" of parts.

Say you make an assembly of sorts for a customer which has many different parts that all end up together and are produced and delivered at the same time. It will be worthwhile to keep for example (T1 3/8 SPOT DRILL) the same for all programs of the series. In short meaning, load the tool changer up with all the tools used on the entire job (if you have room) and make a list of those tools and share that list with the part programmer if that's someone other then yourself. (Actually that scenario would likely be programmer to setup person.) That way you can move from part to part without worry about tools being called by the same number as you've taken care of that earlier. You can even go as far as setting all your tool height offsets. Then all you'll need to do is alter your master Z height for each different part you work on.

All this can still get tricky, but a little steadfastness to the idea will make it work.

Dave

Any system you come up with in which the numbers mean anything will eventually run out of slots in some area. You could end up with 12 different 1/4" endmills, some that differ only by corner radius, or flute count, or shank length, or coating. The only sustainable system is sequential, unless you have enough digits to encode a complete description of the tool. And then it isn't really a numbering system, it's a description encoded in numbers.

We're a job shop, 1-2pc jobs usually.
ALL of my programs, the tools are sequential. 1,2,3,4,5,etc...
It keeps things simple.

We have a lot of tools that stay set up for certain parts and families of parts. We're attempting to create a shopwide numbering system that will designate where those tools are stored in their vidmar drawers, such as 1A7 meaning drawer 1 lateral row A in/out row 7 so we can find them and return them quickly. Then we need a way of tagging the tools with that ID that stands up to use in the machine. We're currently using wire tags with job and tool info handwritten on them. Some of the tags are getting pretty deteriorated and are out of room to add data - there's never enough time to fix this...

As far as in the machine, we just group the tools together according to how they are called in the program to make tool changes quicker. That means moving tools around a lot and resetting lengths, but having an auto TLI makes that OK.

yes most larger shops use a tool numbering system. if tool 200027 (which can go in any pocket but some prefer a particular pocket for each tool)
.
so tool 200027 has a setup drawing with tolerances on length of stickout, length of flutes, dia, etc. obviously for collision or crash prevention the tool spec especially stickout length is important and obviously excess stickout length causes excess vibration. a 26% increase in stickout increases deflection 200%, it follows the cube rule 2x2x2 or 8x more deflection with 2x longer stickout length
.
so main reason for tolerances of tool setup is too short or long can cause a crash problem or sudden tool failures (from excess vibration). even a drill bit if flutes not long enough even if shank is sticking out if flutes totally buried in a hole the chips will pack and cause binding and severe drilling problems
.
obviously cutting parameters can vary widely with different tool setup. not unusual to increase cutting parameters 200% with what seem like a very small change in tool setup

Cole2534 said:

As I begin to outfit my VMC I'm wondering if I should start with a tool numbering system rather than just haphazardly loading them.

I was thinking a system of 4 digit numbers like so- first digit tool type, second digit holder type, 3&4 would be tool descriptors like size and flute length?

Tool 1104 might be an edge finder in a solid holder, or 2206 might be a 3/8" end mill in a collet.


Is this worth a hoot, or am I over-thinking it?

Click to expand...

Dooing this with a VMC may be daffycult?
If you have a horizontal with 80+ pockets, then yeah, but with a vertical, you prolly just need to doo like others and keep your everyday tools up front and change out the oddballs at T20 or whatnot.


---------------------------

Think Snow Eh!
Ox

ok i give another example. say you rough mill with a 1" dia end mill and some jobs need the tool length so you stick it out 3" for the occasional jobs needing the 3" stickout
.
say 3/4 of your work you could get by with 2" stickout instead of 3". so math says
2/3 x 2/3 x 2/3 = roughly 0.3 deflection or you can increase cutting rate about 333%. so the majority of jobs you can rough mill 333% faster by using a specific tool setup rather than leave tool sticking out extra for occasional jobs
.
specific tool setup not only can you save many hours per day but your tool life can actually go up too if you dont max out the 333% cutting parameter increase.
.
you got guys trying high speed machining or increasing cutting parameters when you rarely hear them talk about tool setup optimization for 200 to 400% increase in cutting parameters
.
the math says a 26% increase in tool length stickout increases deflection 200%. the extra 1/4" to 1" of tool stickout can have a big effect
.
math is the most powerful tool in the shop and often it cost nothing but the time for the basic calculations. i use excel to help with math. it can also calculate hp and cutting forces. useful if you dont want to stall the motor or have piece come loose in the machine

This is the sort of problem that barcode systems were invented for.

An overly simplified idea of how such things can work :-

The barcode is just a unique identifier. The identifier cascades into the database pulling up the tool description, 1" Ø long series endmill for example which in turn cascades into the tool call out file for the part to be made which finally cascades into the particular location of that tool in the machine for that job.

No idea whether or no things are actually done just like that but, hopefully, it gives you some idea.

You have to de-couple at each stage.

Any static numbering system eventually falls over itself either by becoming too complicated to use or by running out of number slots and designations. Usually long before that you hit the point at which its easier to just use the proper tool designation eg 1" long series end mill than faff about with a numeric system.

There is a reason why most folks simply reserve a few slots for always in tooling, probes et al and load the rest on an ad hoc basis. Much better to spend time sorting an effective tooling list with set-up parameters, as in Toms post above, for each job than trying to devise a universal numbering system. Having been on both the receiving and devising end of, at best, semi functional systems of this time I can assure you that there are much more pleasurable ways of getting a major league headache.

Clive

Cole2534 said:

.... or am I over-thinking it?

Click to expand...

I think yes to that.
What does your number system do for you and where does it save time or money?
KISS. Despite the human need to organize, never add things that don't provide value added.
Bob

No rhyme or reason, unless you have a LOT of pockets. We have one machine, first 60 tools on a 132 tool magazine are "standard", but I can only remember a dozen of them. They are sorta sorted by type and size, but it isn't perfectly sorted.

T1 is a spot drill. T2 is a huge spot drill i never use. T6 is my go-to face. T12-14 1/4" endmills, 15-17 3/8, T18 1/2 rough, T19 1/2 variable, T20 1/2 sharp corner.

Various bigger endmills up from there that I refer to, then drills and their corresponding taps, then standard size drills, then it is all over the place above T60

many tools above 60 are reserved for jobs that I know will come back next year, or simply didn't have the time to remove when the job was done - I kinda know whats in there, I might have to walk around to make sure if it is or which pot.




On the verticals, which most don't have more than 24 tools? No rhyme or reason, and we don't keep standard tools in a specific pot. If I have to face before milling/drilling, a facemill will be T1. Next job doesn't need a facemill, just a spot and drill? Spot drill is T1. and so it goes.

Definite KISS here.

Take advantage of location in your toolchanger, don't just follow numerical order. For example, my length standard is T32 in a 32 tool magazine, and the probe is T31. That keeps them close to pocket #1 for fast access, yet the probe is out of danger from flying crap. Other tools are arranged on either side of T1, the last couple tools in a job of less than 20 tools might be in pockets 27 through 30 just so the magazine is close to T1 when it's time to start the next part. We have our code generators set to reload the first tool when the program is finished, that way the spindle is not open to swarf while the part is being changed and you don't have to wait for the toolchanger to run when you push the green button.

CarbideBob said:

I think yes to that.
What does your number system do for you and where does it save time or money?
KISS. Despite the human need to organize, never add things that don't provide value added.
Bob

Click to expand...

Thanks Bob, practical as always.

You too, Ox and the others.

I'll keep a few of the typicals set as the first few and exchange the rest as needed.

Sent from my SM-G930R4 using Tapatalk

I make a tool list for each machine. I start with spotdrills as T1 then leave a few empty numbers then start with drills at T10. Then taps start at something like T100. Then Rolls at T110. Specialsl tools like T120. Endmills T150. Face Mills T180. Probes, tasters, test bars start at T190. Those numbers are just guesses.

Most of the time tools, especially drills are not in order of size. I add them to the list as needed.

I keep track of this list in excel and I print it and clip it to the side of the machine. I also have a tool library setup in my cam system with the same tools and numbers. Sometimes the cam system gets confused and I have to reference my excel file.

This helps because all my programs are written based on this list. For example T175 is always gonna be a 1/2" sgs scarb endmill. If there are tools in the machine and a repeat job comes in that uses some of thoes tools the number and offset will good.

This only works if you have a random pot tool changer, or if you can assign different T numbers to different stations in a umbrella changer. My old Fadal couldn't do this and I would have to repost programs for every job because tool stations would change based on what jobs were running at the time. Or after each job tools would have to be jockeyed around to match the programs.

My brother can do this but only up to 100 tools so its list is different than my okuma mills.

Some tools I use alot have dedicated toolholders some get broken down after use. On the tools with dedicated holders the offsets stay in the machine unless the tool is dull and we break it down. Otherwise I stick it back in a pot and tell the machine T175 is in pot 10. Very easy and saves lots of time and confusion.

This is where the Siemens control is superior as you can use names to call tools
T="Al_EM_.500_1.250_1.750"
ALUMINUM SPECIFIC 1/2 Endmill finisher 1.250 flute 1.750 projection
T="SD_.500-90-2.00"
1/2" X 90 SPOT DRILL 2" Projection

T="AL-SM_.250_.375_1.125"
aluminum specific 1/4" ball endmill 3/8 flute 1.125 projection

You don't have to manage what pot tool 1004 is in... and what 1004 is actually...

been doing this for a very long time, still cant come up with a good way.
I guess the best way for me the last 2 years is all odd numbers were endmills 1/2=1 3/8 =3 etc etc. drilling stuff taps and c drills and counter sinks are even numbers.
taps and odd balls I put on the back end(highest numbers) probe is always either 21 or 24 depending which machine it is.
anymore all my tap and drill tools as well as my counter sink tools 60º - 120º and everything inbetween are all mounted permanently in there own collet holders got them from 0-80 to 4-40 sti. this way I dont have to find collets to change the common stuff. just take tool off tool cart and pop in the machines. all set up and ready to go.
always have extra tools in the tool cart for example I have 2 tools that are 1/2" x 1.250 3 flute alumastar Gar . one in machine one on the tool rack. same for about every endmill I run. I have 2 mills and over 120 holders and thats not near enough. mainly due to drills and taps and tooling for stainless.

I keep a white board on the mills with a tool list. cause every time you think you have a tool system figured out its gets messed up