quickest way to mach.large bores?

[stovepipesteve]

running a VF3.
got a job coming up that has (4) 5'' bores, 5'' deep.
i plan on using a 1.875 insertable drill to pilot.then a 1.5 Dapra insertable end mill to rough, then a 1'' finishing end mill to spiral interpolate the finish. Bores have a +/-.0015.
This is going to be very timely. Its a 25 pc run.
I also have to thread mill (3) M30 holes, which i have never thread milled before.dont even know where to start.
The parts wiegh bout 350 pounds,so thier not going to be easy to handle in and out of mach.
All i got is a fork truck to get em in and out, which worries me cause how am i gonna handle them to work stops and secure them once in mach?
i need to face the part , then flip over, face to print, bore (4) holes,thread mill (3) holes,drill (3) 12mm holes.
Then stand up on its side to drill 8'' deep, then slit saw a 6mm slot.
This job is weighing heavy on my mind,the economy is survival mode and this job will make or break the shop.
any suggestions would be great.

[HuFlungDung]

What kind of material? Are the large holes blind bores? While interpolating is fine for the roughing, I think I would bore it to finish. In a 5" hole, you can fit a medium sized boring head right down in the bore, so you can use the side holes in the head, or fabricate some sort of head extension to get the tool tip down that extra inch or so. Interpolating to finish with a 5" long endmill sounds like a recipe for a headache.

With heavy stuff like that, you can actually slide it around fairly easily once you've got it at table height. If there is any way to drill and tap some 1/2" NC holes in it to add lifting rings, that will help. I make regular use of a hydraulic stacker, which is like a manual forklift, to put stuff in and out of my VF3.

I like to use some 3/8" or 1/2" puckboard as a 'skate' to slide the piece around, off the forks and onto the table, to save the table if the part is rough, or save the part if the forks are rough

I would most likely take the part out clear of the machine and lower it near the floor, then flip it with prybars, or chains, or any other leverage. Then lift and slide it back inside the machine.

One modification I made to my VF3 table, which has proven handy innumerable times, is to drill and tap the backside of the table and bolt on a 3 by 3/8" ground flat stock, 36" long which can be bought from many tooling supply places. This serves as a fence. I have it sticking up about 1" above the table top. Yes, I crawled back in there on my hands and knees, and hand drilled those suckers, 3 of 'em 1/2" NC. I did this with the machine powered completely off. I'd hate to get crushed if the machine decides to runaway at that moment

With that facility, you can then use 1-2-3 blocks or any assortment of parallels and/or toe clamps to push the part against the fence and hold it down, etc. This can make for speedier setups, if you add a permanent stop block to the table to locate in the other direction.

So slide the part in on the puckboard, then rather than put the part right down on the table, slide in some 3/4" keystock for parallels beneath the part. You should be able to lever the part up easily, provided that you never let it drop right down flat on the table.

Edit: when roughing the holes, do your initial interpolation as if you were roughing a tapered hole, say 5 degree taper. This will keep the body of the tool away from the wall when the chips are flying hot and heavy. Once you get to full depth, then semifinish with straight down helical interpolation. Now the chips have somewhere to fall away.

[littlerob]

I wish you all luck

Maybe someone can explain to me how to do a multi or partial quote

[stovepipesteve]

thanks for the advice Mr. HuFlungDung.
The material is regular A36 steel(a good thing).
The 5'' bores are thru.
I know that using a borehead would be the way to go, but,,,,i have not got one nor is it in the quote for purchase.(bummer) I may have no choice but to get one when its all said and done.
You think that finishing with a 1'' or bigger finishing end mill and spiral interpolating is a bad idea?(+/-.0015). I dont like it much,but its plan A at this point.
As far as moving pc. around.
Drilling pc. for eye hooks is not an option.
The puck board idea is good but..faces must be parallal. So ground parallals are good under pc.
I plan on putting a sub plate on mach. bed, but i dont think i have travel in Z to skim sub plate for perfect flatness, but i could put stops on sub plate(the big boss would never let me drill/tap the mach.bed itself.
Any suggestions on securing the pc. seeing how i must machine surfaces parallal? Or thread milling M30 2''DEEP.
The pc is bout 24''wide,it has a large radius nose with side tapers to a 10''square bottom.(rough descrip.)5''thick.
this job is gonna kick my butt.

[HuFlungDung]

You use the puck board just as a skate, not as a precision spacer. You can flop the part around on top of the plastic, then use a prybar to lift the stock and slide the precision parallel beneath it. Remove the puckboard from the machining zone altogether while you do the cutting. Then, put it back under, remove the parallels and flop the part around some more.

You can purchase inexpensive boring heads from Shars tool for less than $100. You don't need anything fancy for that. A cheap boring head is just that, a cheap boring head, but with care and attention, and use of a dial indicator, you can split tenths with it easily. Once set, the boring head should be good to finish many holes in one go.

[stovepipesteve]

Thanks agian Mr. HungFlung.
i wasnt planning on keeping puck board in machine, i errored my typing (not good for at mach.programming).
i will check into Shars boreheads,i can afford to drop a couple hundred on a cheap head.
Im worried about chatter in a lrg. deep bore. What about those issues?
Any word on thread milling?
thanks in advance.

[HuFlungDung]

Re: boring head
I'm suspicious of the use of small diameter shank adapters for boring heads. If this connection to the spindle is inadequate, then you've essentially increased the probability of vibration occuring.

In personal experience, I had some old CAT40 ER16
collet holders that were cracked and useless. So, I took one of those and cut it back a little, and then threaded it to suit the Shars boring head. It took a bit of playing around to get the head oriented in line with the drive keys, because you need to do this so that you can use one of the boring cycles to orient the head to get it out of the hole without creating a score mark up the side of the hole.

Anyways, this makes a good solid connection between the boring head and the spindle. I'm amazed in fact, by how good it works. I use a set of 3/4" Shars boring bars, and with 4" of bar sticking out of the head, that thing will bore steel as quietly as a church mouse sneaking around

In your case, you only need a stubby bar sticking out the side of the boring head. So perhaps one of their larger diameter shanks will serve you well, as you'll want the whole head to be extended downwards enough to obtain 5" of depth below the spindle.

As for thread milling, well get yourself a thread mill, and practice on something cheap Do you use cadcam? Or I have seen some guys referring to some online calculators that will create a threadmill path. These are found at the sites put up by the thread mill manufacturers. Myself, I would prefer to do the whole thing in the cadcam, so that I know the position of the thread is correct within the model's orientation. You can, of course, do this manually by programming G13's on your Haas.

[extanker59]

stovepipesteve said "I plan on putting a sub plate on mach. bed, but i dont think i have travel in Z to skim sub plate for perfect flatness, but i could put stops on sub plate(the big boss would never let me drill/tap the mach.bed itself."
I ran a Matsuura years ago that I put a subplate on. I couldn't reach it with my face mill so I put a cheap flycutter in a longer reach endmill holder and that did the trick. Just slower. Could that work for you?

[dertsap]

what works best with large parts like that is to make some riser blocks and bolt them to the table , this way you will have less chance of a single chip under your part making your life miserable also if there is any variation in flastness you will have far better control than trying to lay it flat on a subplate , you can add dowel pins to the blocks for stops , its a fairly simple and standard jobbing proceedure ,
as far as your bore goes , if you weigh the price of a decent 1" carbide endmill and a decent boring head you would be best off gettiing a boring head , at least at the end of the job you will still have the boring head and chances you could be turfing the endmill .
if you insist on using the endmill then i would suggest ramping the cut and relieving the flutes so the only cutting edge touching the work peice is the one you want to do the cutting , or you will be dealing with a tapered bore because the cutter will keep recutting the upper portion of the bore as the cutter interpolates downward

emuge makes some good threadmills

[lerman]

You asked about ideas for securing the piece while machining. I usually use a vise.

For something that large, I would use my table vise. It consists of two parts. One has a fixed jaw. The other has a movable jaw. Both parts bolt to the table using the T-slots.

Depending on the shape of your part, you might need to make custom jaws for your vise.

Ken

[ktm666]

i use a solid carbide 1" dijet mirror bull for finishing holes and it does a fine job. no headaches. im sure sure on the cost, although i know its much more than 100. very versaitle though, and extremely rigid and good for finishing holes