240 tool machines

[medaq]

We have a new hplus300 matsuura running 240 tools. I am noticing a little temperature variance in height offsets to the tools. I was wondering what do people do to make their machine more accurate. Do you have the machine pull in all the tools it needs for that job and reset the tools automaticaly with the tool probe?

 

I was thinking of monday mornings when the machine is nicely warmed up to have a program with every tool I have in the matrix. And have it pull in and measure em all on the same day and about the same time. So they have a better repeatability to one another. Our tools once placed in the matrix will probably be there forever till we sell the machine. So having one master program to reset all the tools will be no biggie.

 

But I ask this to know how people handle having so many tools for day to day accuracy. Being one tool set 30 days from the next tool has to have some growth or such.

 

Thanks Jim

[Psychomill]

How much of a variance are you seeing? We have many machines with 200+ tools (including a MAM cell) and don't seem to have this problem. The last couple of weeks have been pretty hot outside. Maybe the temperature of the shop is rising quite a bit?

 

Having to measure 240 tools with the tool eye is time consuming. Maybe instead, you could add a tool checking (measure) cycle before certain tools run in the programs (like tools that cut critical depths).

 

Check out the machine though too. Maybe the spindle is running alot warmer than usual (time to replace the oil?) for example.

 

HTH

[Mike Mattera - TFM]

I'm sure it's the head growing and not the tool.

 

Mike Mattera

[iowajim62]

You in a Climate-controlled facility ?

Huge variations without it.

Good Luck

[Psychomill]

quote:

---

I'm sure it's the head growing and not the tool.

---

Isn't that the same thing .....

 

Sorry,....

 

That's kind of where I was getting at. Check the conditions of the machine. Something with it has changed or is changing.

 

[medaq]

Yea temperature is a factor for us, We dont have the ability to air condition our shop. We have air conditioners, just they are not adequate to cool off the shop enough.

 

Just this morning, I wanted to reset the tool, since the part was out of tolerance, So I ran the tool offset program. And noticed the .5 endmill had a different offset by about .0025.

 

I dont think it is the holder slipping. This tool holder is the kasier big plus mill chuck. Thing seem to have a very good bite on the tool. But who knows.

 

Being it is a new machine, I am not sure it is a oil problem. I went around and checked all the levels and all looked good.

[medaq]

quote:

---

Having to measure 240 tools with the tool eye is time consuming.

---

Where here is what I was thinking to do. Themachine has the auto power on cycle. And with the power on cycle, has the auto warm up cycle. I was thinking of after the warm up cycles, the machine could sub into my program to go through and check all the tools. I think I would first do a h.005 check, and then do a tool set. One to make sure the tool was there. And 2 to reset them all up. And this can all get done 3 am on monday morning and be ready before the crew gets to the shop. So time should not be to much of a hassle.

 

I was just curious to peoples opinions on these type systems. It is my first one, and want to get the most out of the system as possible. Even right now, I modded the 9006 (m6) sub to confirm that the tool being called in has a tool offset value of more than pos 5.0" then I set only a select few tools to be checked at over 3" one this makes sure nothing bad happened to the offset and tries to run a height offset of 0. Positive offset 0 is bad

 

Am I just being to safe on certain things? or are others also having the machine alarm out when a tool comes in with a z0 offset? or if this is something someone would like on their machine, just say so, and I will post my mods to the 9006 sub. I personaly think it is a gfreat safety for the machine.

 

 

Jim

[LaszloK]

I'm not sure you will gain that much by probing the tools prior to using them, even on the same day. I have seen up to a .003 variation in height just from the heat generated fron the spindle even though the machining was done in a climate controlled room. If your variation is due to this, Then you would want to probe the tool just prior to inserting it into the spindle. This will only give a slightly better result since the spindle temperature may change with higher speeds and a long run time. If your programs are short or at speeds that will not generate a lot of spindle and bearing heat, than this advice will not apply.

[Psychomill]

I don't necessarily think its your tool holder either. What Mike, Jimmy and I are getting at is the heat in your shop is the likely culprit. Even if you set your tools on "Monday morning", as the heat rises in your shop, the machine moves, the spindle cartridge expands or elongates, ball screws elongate, etc. This causes your tools to "measure" differently. I'm willing to bet that if on Monday morning you check your tool, then at 5:00 that evening (after a full day of running) you check it again (on a hot day), you'll probably see a change in tool length.

 

quote:

---

I think I would first do a h.005 check, and then do a tool set.

---

I don't know how your probe programs are written, but usually this will cause your machine to stop if its out of tolerance thinking that the tool is broken. You may have to re-write or use a different sub so that the program will flag the tool, then skip to the next tool and continue. It would be a bummer if T1 alarmed out, and you get to the shop and still have 239 tools to measure.

 

Besides, if .0025 of difference is a problem for you, then a H.005 check won't do you much good. All of your tools could be +/- .0049 and you wouldn't know.

 

I think the approach is to attempt and combat the heat problems which is what I think is giving you grief.

 

[medaq]

Atm we are doing a job that requires a +/-.002 on the height of a cut to another plane. I would think I can hold this with ease. But this is not the case atm. I dialed in the machine friday afternoon. Had the .283+/-.002 call out running perfect. Come in this morning and the .283 has gone beyond .285. I have noticed this has been a continuous type problem with holding z offsets. Before I noticed this with some corner rounding cutting I was doing on a part. Where the corner rounding tool was going to deep into the surface. At the time I chalked it up to be my end and maybe the tool was not tight enough. But the problem came back.

 

And now I have a more critical problem where it is not a visual thing, but tolerance thing. So this morning I reset the tools and wrote down the original offset, and the new offset.

 

( ) FRIDAY SATURDAY DIFFERENCE

(T8 ) (5.1296)(5.1286)(0.001 )

(T13 ) (5.9466)(5.9457)(0.0009 )

(T15 ) (3.9306)(3.929 )(0.0016 )

(T19 ) (5.2847)(5.2844)(0.0003 )

(T39 ) (5.9268)(5.9259)(0.0009 )

(T48 ) (5.5715)(5.5687)(0.0028 )

(T168) (5.23 )(5.2311)(-0.0011)

(T196) (6.2138)(6.2134)(0.0004 )

(T197) (6.2414)(6.2401)(0.0013 )

 

 

From my highest number to my lowest number, I have a difference of .0039 .

 

I understand we will always have some thermal growth issues. But this is a little much for me to handle. So I thought I would ask the question. Is this a normal thing to have .0039 change from overnight. Now even with thermal growth happening. If I set all these tools yesterday at the same time. They would have been set at a certain amount of growth. Then again in the morning, should they not seem the same type of thermal growth or shrinkage? And even in the morning it might be cooler. But the machine never shut down all night. So alot of the areas would still keep the same amount of heat as the day before. (spindle, ways) Since at both times they have been checked under same type circumstances?

 

 

Should I expect better from a mam type machine? hplus300? on a poured foundation, And bolted down.

 

Or is this normal for people?

[medaq]

Btw we have 2 sides to our shop. The hplus is on the side where the shop stays cooler. Since we have more airflow (side doors).

 

Now I just went to what is the hotter shop. We have 2 es 450h's in there. I checked a tool that has been in there for a good 5 months. I checked its offset. And it came in within .0003 of the offset in the machine. So I am truly baffled if this is thermal growth. I am almost thinking being it is new, something is just not right on the machine yet. Being a japanese machinea dn somewhat high end. I would think this growth is a little excessive.

 

But again would love to hear people with a similiar type machine or same type quality machine.

 

I dont think I have this much growth from tool to tool on the fadals. :/

 

Jim

[Tom Szelag]

Got a 21 tool ATC Fadal and my tools stay dialed in

 

Can you give me the approximate length of one of your toolholders (from the flange down to the bottom of it, NOT including the tool length)? Maybe T197? From there you can extrapolate what kind of temperature change you'd need to cause that, see if it matches up with what the shop normally goes through.

 

The thing about the machine on your "hot" side of the shop...the issue of thermal expansion isn't really a question of the absolute value of how hot something gets, but the relative difference and cycling it goes through during the day. If it STAYS hot and close to the same temperature all the time, since there is no temperature difference, things won't change.

 

It would be nice if you could track a few tool's length offsets over the course of a typical day, or a couple typical days. Make a little chart. See if it's consistent over time (short in the morning and night when its cool and/or not running, long mid-day and mid operation), and from tool to tool (all tools growing and shrinking).

 

Then you could narrow things down to this being a heat problem or something else (ie, we've been barking up the wrong tree). Maybe its just a disgruntled employee messin with ya

[flatwoods]

Have you taken the tools out and checked them manually on a tool height measuring gauge?

[Tim Johnson]

Is there a chance you're loading dirty tools? If there are chips being clamped it will change the height. You could also check for variance in your drawbar pressure though you should notice that with bad finishes if it's not pulling correctly. Also, are the tools that are being pulled hot or cold? If the tools are in the spindle a lot they may be warm going into the spindle while a tool not used much will be cold going into the spindle. Just throwing out some ideas.

[Paul McGarr]

I've seen that before, and it's almost always due to machine head temperature. Dont forget to check some things the old way. Put a tenth indicator setup on the table and set it against the underside of the head. Watch the reading throughout the day. If nothing happens, do the dame thing with the spindle running at typical speeds for your shop. Maybe you see movement now.

 

Even a new spindle can have problems. Ask the machine manufacturer what temp the spindle should be running at. It it running at that temp?

 

No matter what, .004 deviation in Z is not "acceptable", and I don't think anybody would say it was.

 

Not to scare you, but I had to work on a machine that had the same problem, and it remained a mystery. I never knew what I was going to get. I would pull my hair out...it was no fun. I hope in your case, you can find it.

 

Don't forget that it's all relative. If you have a lot of "Z", you will get a lot of error. A warm spindle will cause a warm head, and that will cause a warm column, etc. Every inch of steel is going to be affected by this growth. You won't notice it as much on a smaller machine.

 

Good luck. Keep us posted.

 

Paul

[Tom Dorgan from American Precision]

I realize this is a machining center/mill question but in my shop floor days I ran a brand new 4 axis Warner Swasey that I could walk in and minus the X & Z offsets .002 and back them off .00025 every part until it was warmed up. I assumed this was normal warm up as it was consistent. Is you varience consistent where you could adjust and sneak up on it as it warms up or is it all over the place? If it is all over the place I would look at something other than head temp myself. But then, I am a Router guy now so close tolerance for me is 1/16" in wood nowadays even though we can hold +/- .001 .

[?Mark]

Jim, couple things to check.

You mentioned running big plus holder. Those types are VERY sensitive to dirt. With todays higher end machines big plus spindle is standard but in order to have it run fool-proof(clean) you still need some kind of attachement to keep the bottom of the spindle clean. Ours is prolly coming next week so I'll know exactly what it does and how it looks like.

 

quote:

---

So I ran the tool offset program. And noticed the .5 endmill had a different offset by about .0025.

---

Did you try setting the same tool twice after only a tool change? If there still was a diff. it would mean bad or loose probe...

 

If you run a spindle close to max rpm for several minutes it will grow no matter what (heat), so it might be a good thing to invest in a machine probe to check critical dim. without having to deal with scraped parts.

 

Since the machine is new call the service to check if everything is nice and tight

 

 

jm2c

Kind regards, Mark

[robk]

quote:

---

From my highest number to my lowest number, I have a difference of .0039 .

---

Boy that # looks familiar

Since you have a new machine under a warranty get the manufacturer of the machine, control, and the laser software in there ASAP and have them work out what the problem is. Might be a paramater problem. You could be swithching between inch & metric in the middle of the cycle.

[medaq]

quote:

---

Did you try setting the same tool twice after only a tool change? If there still was a diff. it would mean bad or loose probe...

---

First thing I checked was to recheck the tool to itsself. And normaly the offset will repeat to be the same number or a little difference of .0002

 

I have contacted one of the machine dealers head honchos and explained my problem through a email. IN fact I cut and pasted that letter and posted it here to see what others thought also.

 

As for tool cleanliness, it was one of the other thing I thought of, and evey tool I pull out to check, I use my hand to wipe the taper. And I never find any debri.

 

 

Jim

[?Mark]

quote:

---

I use my hand to wipe the taper. And I never find any debri.

---

Since you use big plus which is "dual contact" holder you need to pay attention to a bottom surface of a spindle also, but I bet you covered this as well.

 

Keep us posted, will be intereting to know what the couse of this is

 

Mark

[Psychomill]

I'm still stuck on it being a heat issue. I would assume you have a spindle chiller unit of some sort. Is this functioning properly? We had one that by all appearances, was working. It turned out that the pump was going south but not enough to trigger the alarms at the control. Check the condition and levels of the coolant (refrigerant) it uses.

 

Oil control is another thing and thats why I asked about it earlier. Not just levels, but good flow (clean filters and clean, not burned or old, oil) and pump pressure.

 

[iowajim62]

medaq,

 

I agree with Rob on the heat issue. Now that it has been brought to my attention about the dual contact holders it makes me think there might be issues with thermal coefficients being different between the spindle and holder. In other words the holder would heat and cool faster than the spindle itself. Another thought is that the machine casting itself is heating up as evidenced by the .0039 difference. I have seen .0035 throughout the day and got by it with using the probe to update offsets right before cutting critcal features. This allows the magazine to stay "matched" so to speak or relative to each other. Another thing to watch for is that biga$$ magazine full of tools causing the magazine to lean towards the machine.

This is more pronounced as time goes by. First indicator is the toolchanger grabbing the holders and leaving rub like marks on one side only. Which indicates that either the machine sagged or the magazine/toolchanger assembly has moved from the original position the techs set it up at. You can get by this with a change to your G30 toolchange position parameters.

There is also a tendency for machines to go out of square up there in Fremont. Most notably in the "Warm Springs" area.

Good Luck and hope it is a simple fix like thermal comp not working right.

[Matt Berube at Ferron Mold]

I wonder what would happen if you "idled" the spindle at about 40-50% of maximum overnight. Then see if the problem goes away... Our fadal idles 24/7 and that makes all the difference for us.

 

Also, we have a Johnford that had serious thermal problems. We added a cooling channel around the lower bearing housing and added a supplemental chiller (a second unit) and it got a lot better.