DEBATE: Gage cuts needed for boring on CNC horizontal machining centers?

[powerfulp]

There is an on-going debate at our shop on whether or not gage cuts SHOULD be used when finish boring on a CNC horizontal machining center on tolerances of about +/- .002 or less.

 

The shop floor personnel say "yes" because we have problems of getting chips in the spindle which will help to cause oversize bores. However, management disagrees. The main reason is because we have a sister company and the management there says they don't do it and don't have any over-sized bore problems. We both run the same parts on similar machines.

 

(We have about 15 horizontal CNC machining centers and boring mills. We machine part sizes that would fit on a 500mm x 500mm table to 2500mm x 1500mm table. Material is usually ductile iron castings)

 

I know we get chips in the spindle, in fact if you look at our pockets in the tool magazines there are impressions of where chips were, therefore I think that's proof that there would be this problem. What I don't understand is how the sister company "doesn't have any problems" when it comes to this.

 

Any feedback on this issue? It's driving me nuts hearing from management that we should take the gage cuts out when I know (at least I believe) it will cause over size bore problems. And don't want to scrap parts out to prove a point...

[jeff]

What do you mean by gage cuts?

I would call your sister shop and ask them how they prevent chips from getting into the tool pots.

[Guest]

Oh high value parts, castings and materials, I have always done gage cuts on fussy diameters.

 

On something I can pull off the stock rack and remake for negligible cost, I do not.

 

When you get 1 $100k casting to make a part, you don't take chances

[Newbeeee™]

Yep - 'phone a production engineer in your sister company and find out.

You should know never to believe management

Are the machines identical models.

Are you cutting like them, or faster and throwing chips everywhere?

If your management insist to take the cuts out after you guys have explained why you want to keep them in, get a manager to email/memo/put in writing to take them out.

On the next expensive scrap jobby you'll have a bit of arse protection then...

[BenK]

We do a lot of boring of tight diameters here without gage cuts. I think you need to figure out why you are getting all the chips in your spindle before anything else. We have 7 horizontal machining centers and we don't have a problem with chips in the spindle. Are the operators using an air hose in the machine when the tool is being changed?

[K2csq7]

Gage cuts..... You mean back the boring bar off, check size, then adjust for finish?

 

I would look at how much time it takes to make this extra cut & check the size. Lets say 4 min. (have no idea the size of your bore)

How many of these 4 min checks would it take to equal the cost of 1 scrapped part?

 

Even if there was not a problem with chips in the spindle, I would MAKE SURE, my operators were backing off, then checking, the going to finish....

[dforsythe]

Make sure your overhead coolant is spraying the tool and spindal. this will keep chips from making it into the tool changer. second use your tool probe in the machine to check the z offset. if there is a chip then the tool will check .001-.005 longer. this is what causes the run out.

 

damian

 

 

[chris m]

What you're doing now is a work-around; what the management would like you to do is fix the actual problems in the process to avoid unnecessary direct labor and machine time. If you can research 1) how many times the gage cuts are catching problems (1 in 100, 1 in 10, 1 in 2), 2) what the productivity increase would be if you eliminate this practice, 3) what the cost in scrap parts would be if your current problem rate continues, 4) what is the root cause of the problem, 5) what the cost would be to eliminate the problem, and present all of this information in a cogent manner, you will (hopefully) get an informed decision from your management regarding how they would like you to proceed.

 

my $.00002

[gcode]

you will (hopefully) get an informed decision from your management regarding how they would like you to proceed.

 

 

or he will pound his fist on the desk and scream "Just f'n do it!!"

[chris m]

This is also a possibility; BUT, if the boss' plan fails, following my prescription will enable you to pull our your report and smile as your a$$ is covered.

[Guest CNC Apps Guy 1]

IMHO, if you have to take a gage cut, your process is out of control and needs to be fixed. It's an unnecessary step and should be eliminated. If it can't be due to "issues", those issues need to be identified, documented and finally remedied.

 

JM2C

[MIL-TFP-41]

The only time you should be taking a "gage cut" is for the first article. If you find yourself having deviations after that, then likely you have other issues.....taper problems will rear their ugly head every time with inconsistent boring results. You noted that you have problems with chips in the spindles....this should never be an issue with good housekeeping. I have run bores from 1" in diameter to 32" in diameter (manual toolchange that one!) with no issues with repeatability.

[Zoober]

3 issues here.....

1: You are damaging good machines and holders due to chips. Fix that. Pronto.

2: when you say Gage cuts, do you mean boring .05 deep and checking, or backing off and adjusting? Either way is a problem. Get a sacrificial plate, and cut in identical conditions as the part so you don't have different amounts of cut material. There is little chance of gaging a cut .05-.100 deep accurately...

3: like James says, look at the process. Chris mentioned ways to control it better. I came frm a shop that specialized in $200k+ Ti castings, and trust me, having a sacraficial plate can save your bacon on tight bores and insert changes. And gages real word, where a shallow test cut does not.

[powerfulp]

What I mean by gage cuts is we do not back the diameter off, instead we just bore just deep enough to allow a measurement (in most cases this is 5% or less of the bore length) and we adjust the diameter (if necessary) from there.

 

I just find it hard to believe we are the only shop in the universe who has this problem. It is across the board on the horizontals in the shop. From the old to the new to the small and the large. Obviously on our 10K+ castings we are taking preventative measures no matter what. On the mid to smaller stuff, it would be "nice" not to take the gage cuts but I, in good conscience, can't just eliminate them across the board because of the potential scrap that will incur. Regardless of CYA.

 

Regarding the CYA, I know how to go about that with the emails/documentation and etc. And I will do this when the time comes to start eliminating the gage cuts. I want to have an idea of what is causing this oversize bore problem and make a change of some sort before removing the gage cuts, however. Which brings me to the root cause analysis...

 

...I'm at a loss as to the contamination and here's why: Our sister company uses the same equipment in a lot of cases, some are different, but similar across the board. When I ask the question (how do you keep chips from entering the spindle, etc) the reply is they don't do anything "special". So I ask specific questions hoping what they don't think is special is something we would think is special. Some ideas are that the chips are accumulating on the spindle housing/face and dropping on the tool taper when tool changing. So do you (my sister company) keep an eye on this or clean it every so often, etc. The answer is, "not particularly" & of course on special occasions. And to be honest, these are CNC automatic machines. I cannot imagine that shops that don't have this problem do (or can possibly) keep their spindle housings/faces clean of chips at all times. So that being said, at some point they would have to experience the same problem I'm having, IF that is the root cause. But I'm not hearing this. Another idea is the chips are coming from the tool magazine pots (but HOW do they get there to begin with?) and transferring to the spindle, etc. etc. Do they have PM that cleans these pots out regularly? Again though, how would the chips get there to begin with? And I'm talking when I look at these pots (plastic liners), they are embedded with indentations from where chips were. If they are getting there, they are getting in the spindle. HOW??

 

I agree I need to find the root cause. That's what I'm working on here with the help of you guys on this site. I need other ideas cause I'm out. I'm hoping we are doing something different than those that say they don't have this problem, and I can't think of anything. And btw - regarding the frequence: We can run 10 - 20 - 30 parts in a row with nothing but normal tool wear causing the size variance, but we will eventually get an oversize bore.

 

Thanks for taking the time to read this and giving me some ideas...

[Newbeeee™]

Are any other features oversize?

If they are not and it's only ever the boring tool, then by the logic swarf is only getting on this tool, every time???

Which may then lead to something else, because chips if they are getting on the taper, would surely get on other tools as well?

Just a thought.

[Joe788]

 

 

...I'm at a loss as to the contamination and here's why: Our sister company uses the same equipment in a lot of cases, some are different, but similar across the board. When I ask the question (how do you keep chips from entering the spindle, etc) the reply is they don't do anything "special".

 

Maybe they aren't doing a very thorough job of checking the bores.

[MotorCityMinion]

Backing off a boring bar then taking a cut, and adjusting afterwards was always common practice in the 3 larger shops that I worked at. Not every part, but definitely on the first piece or after indexing an insert edge. On tighter tolerance bores it was not unusual to clean the spindle taper and hand load the tool. Not every tool, just the fussy stuff.

 

I've run iron and aluminum castings exclusively for over 13 years, using systems with filtration on HMC's and Boring mills. IMO, regular cleaning of the tool magazine and tool changing components is a no brainer. Whether you use air or coolant, chips and residue get into everything, period. Same goes for the pallets and locating pins as well as the pads on the rotary unit in the machine. Yes, it sucks unloading the pockets one at a time and cleaning them on occasion buts it's necessary. Throughly cleaning out a multi-pallet system is no fun either. I will admit though that most shops doing quantities do neglect this and run continuously until there's a problem.

 

Your sister company either doesn't care, or they do not know better.

[HT]

You may need take a trip to your sister company, stand next to their machine for few hours and talk to no one but the operator of that machine then you may get a better view of picture. There are things that a "CARE OPERATOR" doing every day along with doing his job that became nothimg special to brag about .

[Rob @ Target Machine]

Maybe one on the simplest solutions to keep chips out of the spindle:

 

Keep all of your tool pockets clean and full!

The same goes for all moving parts within your tool changer.

Arm, door, etc.

 

Edit:

Usually the culprit is atomized coolant condensing in empty tool pots.

This dries and thickens and will let a stray chip stick in the pot.

Eventually the chip will get turned around and the dried coolant will help it stick to a tool holder,

That's usually how they get in the spindle taper.

 

Chips can't easliy get into an occupied tool pot, and neither can the coolant mist.

 

Been working for me for years.

 

As for test cuts, I'll use one for a first piece and at tool or insert changes/indexes.

[Sticky]

Why is your spindle air blow not working during the toolchange? Are the chips on your taper from buildup on the spindle nose, or from other parts like the tool change, door or magazine? Either way you need to get those chips off your tapers. I would not recommend shooting coolant at the face of your spindle, that is going to decrease the life of the seal on the spindle nose, even if it is equipped with air blow around the spindle nose during operation.

 

Gage cuts in any sort of production is a waste of time, get your process dialed in, get your machines cleaned up and functioning correctly and put out more pcs/hr!

[BenK]

Do your machines have a shower coolant? we use ours and it keeps the spindle free of chips.

[Rob @ Target Machine]

After giving your 2nd post another read, I'm inclined to think that your oversized bore problem is more likely an insert problem.

Sometimes what looks like normal wear on an insert is causing a "built up edge" causing an oversize cut,

or a rake angle change causing a change in the amount of and / or direction of deflection.

 

It's a more likely scenario if this is across the board as you say.

 

I'd rule out the chip problem in one machine first by cleaning and filling all the tool pockets.

 

Then throughout a full shift, have the operator monitor the bore sizes noting the degee of wear on the insert, finish achieved on the part, and the # of cuts the insert has made.

Give him a pen, pad of paper, and a profilometer to record the results.

M00 a tool check point after the bore is cut and try to catch the oversize bore right after it's been cut, but before the tool change.

Check for runout, look for that chip and pull the insert. Mark the edge that cut big and set it aside.

 

A pattern is bound to appear.

 

Assuming feeds and speeds are dialed in or close, more than likely, a change in insert geometry, grade, or frequency of insert change is all you need to change to solve your problem.

 

JM2C

[Justin Beebe at Folsom Tool]

I'm not sure what kind of boreing head your using but you should be able to easily hold +-.002 with a good boreing head with no gage cuts. We use Komet here and easily hold +-.00025 with no gage cuts.