how do you setup??

[Elad]

I'm trying to find the optimal way to setup the machines.

we setup in the machine.we have vertical machines,and after finding the x,y we call every tool,and we take the tool to the material and we write the tool offset (length)

This is not a very good way.it takes us about 1.5 hours to setup a simple job (with 5-8 tools) and about 2.5 hours to setup more then 10 tools.

We have about 7 vertical cnc machines and we have about 8-10 setups in a day.so we spend about 15-20 hours on setup every day (and we work only 10-12 hours )

Is there a faster way??

What do i need to do it faster??

[Mick]

One way would be to get a tool presetter (like a height gauge)

They are expensive, but tool length offsets can be set away from the machine, while the machine is cutting. I used to use one of these at one of my last employers, and they were certainly productive. Basically, while the machine is running, you set all the length offsets, write them down, and when ready, load the tools, and load the offsets into the control.

Works great. If I was buying a machine, I'd buy a presetter at the same time.

[Kenneth Potter]

I like using a shadow graph for presetting TLO,s

 

Nothing touches the tool {tips/edges}!

[limitless creativity]

Invest in a tool presetter in the machine...

 

Once the distance from the presetter zero and your program zero is known, all you have to do is call a g code, then the H number in a line and the machine will set the height offset for you. or you can load all your tools in the magazine and run a small program to set all your tools for you.

 

Talk to your local Distributor or the machine tool builder

 

The money spent on the investment will pay for itself within 2 months.

 

Mike

 

[ 06-16-2002, 11:50 PM: Message edited by: limitless creativity ]

[beav700]

I do setups all the time.It takes less than 5 minutes to set fifteen tools on Hurco Machine. All I do is put all my tools in the magazine, change the tool, jog it down to my work piece, touch the tip of the tool to my 2" gage which lites up, then type 2 enter and go to next tool.Most of my jobs have at least ten tools and I never spent more than five minutes. And that's standard in every shop I've been in. If did 10 tools in 1.5 hour, I would get fired on the first setup. Got to move to Israel.

[Fig sign]

HI , Elad!

The cup of coffee and a cigarette is the must.

Speaking serious if you are not making a lot of parts , like in mould production, it is a good idea not to take offsets all the time.

I have smthn like 10 tools always in the magazine

(central drill,rough mill12,end mill 12,insert mill20,insert mill25,end mill 6,drill5.8, drill23,ball mill 6,ball mill 8).

whose offsets are tacking according to first constant tool like rough mill 12.

So if my new setup will need them they are always by hand ready to go.

I never take off any tool before I make new setup there is always a chance that I will need it.

So without any presetter my tool setup is not more then 5-10 minutes.

It consist of adding a couple of tools and changing the tools numbers according to magazine.

Thus I can make 5-10 operations a day(including programming ) alone.

And I like to work alone .You are the boss, nobody

is fooling you ,you have a good time quickly making parts the way you like ,beeng sure in YOUR program,setup and tools.

The setup speaking generally is very specific matter, always try to find the simplest way.

I want to say a couple of words to Beav700 .

Hey , man !

Come to Israel I will invite you to my place and plz show to us pure creatures how to work.But sorry without any presetter without any clever things you have and I will show you the speed of my setup and my results.

[chris m]

Ouch! Setup can be a killer; many ways to reduce it though:

 

1) Beav's 2" presetter is a good quick way (MSC sales flyer this month, very short money).

 

2) Dedicated tools are good if you can use them (touch it off once and you'll know the length for ever), we use these a lot on our Okumas as you can set it up so that the tool length offset is the same number regardless of which machine the tool is in (love my Okumas).

 

3) Renishaw (and others, I'm sure) make tool measurement tools that will check the tool length and diameter and write to your offset register using a subprogram; probably pricey, though...

 

4) The lathe answer, of course is quick-change, quick-change, quick-change. Very expensive up front but a huge timesaver on repeat jobs.

 

Good luck

 

C

[McRae]

A Presetter is a quick solution. For an economical alternative I would suggest to use a Spindle Adapter (basically a spindle taper to hold the tool) and a hight gauge. Measure the distance from the face of the adapter to the tip of the tool, record this, enter it into the machine offset register, and set a z value into the fixture offset. This way all the offsets will be calculated from home and job to job tool setting can be eliminated (The hazzard is with critical depths - may need to run the tool twice, or record the deviation between measured length and actual, then correct the offset amount.)

 

This emulates what a "presetter" - in todays Functions - a "premeasurer" will do for you. (A presetter is the rusty hunk of crap the boss bought at auction because he thought he got a good deal even though he has no idea what he bought. Unfortunatly you can buy Crap for 5 cents a pound but then you are still left with 32 pounds of Crap!)

[Jack K]

I use a presetter to check my tools and once they are in, they are set for any job that is common. At another shop I used a height gage. I made a fixure to hold the tool on my surface plate and set my gage to zero out at the same level on the holder where the spindle face would be. Then I used a 8 inch bar and touched the it between the spindle face and the workpeice. Set Zero and add 8 inches... right on the money. Just as good as the presetter and about 10 to 15 grand cheaper! I can set a new job with 20 to 30 tools in 30 minutes or less.

 

jk

[mbuster]

I use 10-15 tool also and I call the table zero. so all I have to do is call tool up and touch it off with a gage block. And I run the tool at the speed it will be running at for like 30 seconds or so. before setting it off the gage block. I do this because I find the tool holder gets sucked up a couple tenths when running at high rpm's

[Matthew]

I set all my tools to the table, then determine a height from the table to the top of the workpiece, either with an indicator (rare) or one of the tools (most common). I find this works great if I have a bunch of part for one customer that have most of the same features, then all the tools are already set. Also, when I program my first part in mastercam and save it, I erase all the geometry and toolpaths, then import the second part into the file, and I have all the tools already defined. If I need another tool, I just add one to it. I could start with 5 tools for the first part, but by the time the last part is finished I might have 15 different tools in the magazine.

[PE @ IHS]

Amen to Matthew's suggestion. It makes far more sense to measure your tools from a permanent datum like the table than touching the top of your workpiece. This way all you need to adjust is your work offset Z value and you can use many of the same tools on a completely different part without having to re-measure your tools.

 

A lot of good milling machinists measure their tools from the top of the workpiece every time, but this is not the most logical approach.

 

Peter Eigler

[jeff]

I work for a job shop so setups are endless.

i usually try to keep a few dedicated tools in the machine and just change my work shift Z value accordingly.

typically i use about 5 tools for each job and i can set-up,program and be operational in less than 1/2 hour.

give or take a few depending on the job difficulty of course.

but i always touch off my tools from the workpiece.

a tool presetter seems like way too much coin to spend on something that can be done in 5-10 minutes by hand.

it could just be the way that you or your setup man goes about doing it.

i have a guy that takes 2 hours to gather and touch off tools for the simplest of jobs. (a single keyway or bolt circle)

that is going to end shortly believe me.

lol

it's nice being the boss sometimes

[heeler]

We have an 3" high dial indicator that we set in the mill and use a setup tool to establish our reference z0 and the measure each tool from that point. If you break a tool you reload the setup tool, reset reference z0 and the measure the new tool with the machine. You then use the setup tool and the indicatior to set your part G54 ect z0 as required. This way you can use any of theese tools in any setup. We use Fanuc 18 and 21 controls. Our 21 controls have a measure function on them and the 18 you have to manually type in the offset in the offset screen.

 

This works great for us and is very fast.

[Elad]

Nobody here do his tool offsets outside the machine??

I think it can be the best way to get the tool offsets while the machine is cutting.

i would like to know more about that.does anyone here work that way??

 

Thanks

[chris m]

Heeler

 

Your Fanuc 18 doesn't have a measure function? Ours does; could it be an option?

 

C

[iowajim62]

Yes we do it that way.

We use Parlec Presetter and Hoffman Balancer Machine to balance after setting up Tools.

We buy balanced holders only (Heatshrink,Collet,Millchucks) to eliminate the holder from the balance equation. This is all for Horizontal Cells, thus we change tools while the machines are running. We also load parts while the machine is running. Once you have your cell up and running you can theoretically achieve 90-100% Spindle Efficiency.(70-75% Realistically)

This is all for High-Production Machining not your 5-40 pc jobs, but you could use these tools

to help on any work. The cost is not small, but once you commit to the extra holders and equipment you'll see the difference as the method pays for itself in increased spindle time.

 

HTH

Jim

Chips hittin the floor,give me more!

[heeler]

quote:

---

Your Fanuc 18 doesn't have a measure function? Ours does; could it be an option?

---

I believe that it is an option. But it really doen't take long to type in 6 digits and a decimal point.

[rottncf]

I use a ground block(jo-block, 1-2-3 block) on top of any fixed surface on the table--I have a ground block that I can bolt to the tee slot, or I just use the back of the fixed jaw of a vise. I set all of my tools once (the same 7-15 tools that I use on almost every job), and whenever I am using my edgefinder(also a dedicated tool) to pickup my work fixture x and y, I slap a .0005" dial indicator and measure the distance from the top of my pickup block to the top of my work surface and wallah--G54,G55, etc. Z offset. This works great--I can have several jobs setup in the machine at the same time, even with the same vise, and never have to change my TLO (except to compensate for tool wear).

[Tony]

Renishaw Tool probe TS27R (I only use it for Z offset)

Sure when things really have to be there I make that tool a Non probe tool, and sneak up.

But drills and hog mills etc, Ten tools in 60 seconds.

Were at 50 hrs a week as of Mon. and are farming out complete molds I can't make by there due date!

[mikhael gutman]

Hi gues !

Elad, look like you using chip control. Fanuc-0, or some thing like that. Your machine look like

Leedwell or something like that.

Cheep stuff that the problem. Good machine as Okuma ,for example, you can set in one touch .

So it not metter what are you country from. Metter what equipment are you using.

[Elad]

Mikhael,

 

Didn't understand your point.

How me time do i neeed to touch in a cheap old control??

I'm using the newest Mitsubishi and Fanuc controls

[Fig sign]

Elad !

Mikhael meens that in enough sophisticated machine you can input ofset from the touch

(from your current position ) automatically.

I am not so lucky, but in my Deckel -Macho Dmc -63v with sinumeric 810 I see my current position in regard to my active home (G 54 for example)and active ofset and simply add this number to my current offset to the offset table with build-in calculator .

Takes a couple of seconds and after reset I see my new active height (0 for example).

Never had any problems.

[PE @ IHS]

Out of all the machines that I have run, I would have to say that the best tool length measurement method was on the Mazak mills. Pretty much any mazak mill with the Mazatrol control built since the late 1980's comes with a tool probe. Not only that, but you can measure all your tools with one command. In other words, you tell the control to measure all your tools while you are on coffee break. It even knows to alarm out when trying to measure a facemill or slitting saw with this method (since those tools cannot be measured on center). This control was far more advanced than any other for its' time.

 

This is thre reason there are so many Mazaks out there. I have still to see a control that is as easy to use. The newer Mazak mills will also measure tool diameter automatically!

 

Peter Eigler

[Hugh.Venables]

Peter's right, the Mazak system is quick and easy to use. The on-machine tool measurer measures the tool length from the end of the spindle. You can simulate this approach off the machine with a height gauge and a block with a tapered bore in it on a surface table. The block should have a reference surface on it to zero the height gauge. The height of the reference surface is not particularly important, it is just a consistent reference.

 

Once all your tool lengths are relative to each other, you only have to use one tool to find the z-zero on the job to set your G54 (WPC in Mazatrol).

 

Hugh Venables.