[Shane1234]

My brother was telling me that their shop uses Komet insert drills and their finish comes out great, and the cat 40 & 50 holders are adjustable to a 32nd. Problem I am having using Mitsubishi TAFM line insert drills are #1 the finish is steppy from tiny deflections and #2 not adjustable to the hole size I need and #3 wont hold the +.005 -.000 dimensions. He believes the Komet insert drills are my answer, and would shave about 5 minutes off my process. one hole dimension is 1.270 +.005/-.000, the other is 1.585 +.005/.000 . surface finish isnt too critical since a bronze bushing is pressed into these holes.

Also, Komet makes special size insert drills as well, so I am torn between an adjustable or special sized drill.......

Your thoughts?

[fizzissist]

How deep is the hole?

Have you considered doing a rough drill, then finishing with an endmill doing a helical boring cycle for a finish cut to size?

[Shane1234]

yes, we rough drill & clean up with endmills currently. thats a 6 minute cycle time. the part thickness is 1.375", the holes are thru. with the right tooling, i know we can get it under 2 minutes easily with the right tooling.

[RICHARD ZASTROW]

Is there enough clearance behind (or under) the part to drill thru with an indexable drill then finish bore with a boring cartridge on the side of the drill shank? I did that in the past and held bearing bore tolerances and finish for 100mm OD bearings.

Dick Z

[Shane1234]

Hey Richard, yeah, there is clearance. I have some simple hard jaws made for my kurt vises. The part is actually about 2 inches above the rails of the kurt vises. Never heard of those attachable boring cartridges before, might have to look em up....

[jamesu229]

I do not know where you are located, but you should call our mits rep. He is the district manager for the southeast. Their drills have worked perfect for us using his recommendations. number is (256)431-2804. Byron Haney is his name. He was a machinist for many years before taking this position.

[RICHARD ZASTROW]

Shane123, Just for ** & giggles, try "googling" Mapal ISO tooling. They have an ISO tooling catalog that has the cartridges in them.

Dick Z

[Shane1234]

Shane123, Just for ** & giggles, try "googling" Mapal ISO tooling. They have an ISO tooling catalog that has the cartridges in them.

Dick Z

Thanks Dick, I will check them out. I am still fairly new to the flat world, only 5 years of self taught experience. I was raised up on lathes, so I have missed out on tips & tricks of the mills, mainly because I had no one to follow in the flat world, just sink or swim (get it done and get it done fast). I find myself looking back at when I first started programming mills and laugh at the lack of future planning I had. Its getting better, but still wish I had learned some of the fundamentals before jumping in head first....

I do not know where you are located, but you should call our mits rep. He is the district manager for the southeast. Their drills have worked perfect for us using his recommendations. number is (256)431-2804. Byron Haney is his name. He was a machinist for many years before taking this position.

Our rep was a machinist for years at Prince hydraulics, pretty decent guy and knows his shyt about cylinder work, etc. I haven't contacted him about this issue since we dont currently have any holders that will offset, like the Komet kub series line do. Also with my experience with the mitsubishi line, sure they hog out material and I can trust it enough to walk away from the machine, but I haven't had the best surface finish using their insert drills. Seems that i get steps in the walls, and its enough that I wouldn't try to send it thru without cleaning it up with a bore bar or endmill. I am riding the middle of their recommendations for feed/speed for mild steel. My chips are not coming out curly, they are coming out long and stringy, have to keep an eye on them or they will clog the chip conveyor in my hurco vmx42. I will give him a call tho tomorrow and see what he has to say about this.

[Shane1234]

That Mapal stuff is pretty sweet, I love the facemills and stainless steel drills. Not much information on their site about the cartridges, like how they are attached. Will try to search for more info....

[Shane1234]

Ok, Dick, can I say HOLY SHYT? Man oh man....... found a catalog, some extreme overkill for what i need, but it sure does light up the old lightbulb upstairs about how to tackle the situation. The owners would easily justify spending a couple thousand dollars to shave 5 minutes off the 6 minute part time, and the Mapal stuff is really giving me ideas.... like doing without a tool change what-so-ever with a custom insert drill that had cartridge expansions to expand to the next hole size. My head is going to be running wild at work tomorrow, hahah.

I already sold them on custom made draps (drill tap combos) for the set screws that intersect these holes from the side. 9mm split point drill about 7/8" long, the next 7/8" of the tool is 10mm tap, and then undercut shank for another 7/8". We had to show them the ergonomic issues that will arise from constantly loosening & tightening the jacob chucks in the 2 bridgeports for those set screw holes. Without the draps, the side work takes about 6 minutes, with 2 different part rotations for the fixturing (50 lb awkward part that looks like an arm for a loader). I am having troubles selling them on ingersoll rand pneumatic self feed tappers for the draps, without bringing the total cycle time down. Even suggesting the ergonomics of twisting that heavy part for the side operations hasn't sold them completely. However if I can get it so the machine time is far less than the side work, they will want to definately go the ingersoll rand route, and then side work will be a dream. And yeah, we have discussed 90 degree tooling, but our hurco wont spindle lock except during tool changes, so thats out the window.

Our projected work load of these parts is 80 per week, with 6:34 cycle time, approximately 2 minutes load/unload time, it ends up hogging up our machine for 2 days almost. Keep in mind these parts are just job shop stuff, about 2% of our total business, where as another 2% of our business is emergency work for packing plants/food production plants, and the other 96% is our own conveyor system/meat packing plant products, which is not slowing down anytime soon. So yeah, I need to get these parts done faster if I want to start seeing weekends off again.... lol.

And yeah, I have thought about a 5th axis gantry style cnc with a huge table for multiple parts, or even a larger 5th axis cnc with possibly a pallet changer, but I dont foresee them buying a machine just to accommodate job shop parts. And I really dont see them telling the customer NO to these parts in the future since our bid was 26 minutes per part, and we are already smoking that time since we are doing the set screw holes as sidework.

[Delw]

Shand as far as insert drills Kormets kick ass In 1" and up with the trigon style inserts.
we do 9310 gear steel in our lathes and run a few hundred holes 2.4 inches deep between insert rotations and we also use that same drill for boring after drilling( which you cant do on a mill).

on a mill I have run the sanviks 1/2" and 5/8" insert drills and WOW

then after a hole close use a adjust indexable inserted boring head like dick was saying. They work great very accuracte and with inserts always repeatable.

on the small bore with a 1.250 drill then a boring head to take out remainder in one pass
Thats 2 down shots are what 5-15 IPM? depending on insert and rpm. ( Your familiar with lathes so its pretty much the same in drilling a boring on a mill and you know what inserts can do.) Ceramics, ceritips, etc etc


then the big bore well leave that one alone or buy another drill and 2 boring heads,( one finish one rough) unless you can get a drill close enough to the size.

One thing to remember if your running a job like that on a mill treat it the same way as a lathe always use a rougher and a finisher( boring head) this way you only have to change the rougher insert and the finish will be left alone.

Delw

[Shane1234]

Thanks Delw, that was the original plan before i heard of the surface finish capabilities of the Komet Kub series. I was planning on using a 1.25" insert drill for the 1.27" hole, and a 1.5625" insert drill for the 1.585 hole, and use a boring head for each hole. Deco Tool Supply quoted me a couple Seco finish bore heads with cartidges for 1200 & 1100 for these holes, just thought I might be able to get by for cheaper...... Now to get ahold of Mitsubishi and see if i can get their insert drills from scoring the holes so badly that I wont be afraid to jump up to that .02 under hole size for the insert drills....

[jamesu229]

Please call Byron again, he apologizes, but he accidentally deleted your number. He can control the hole diameter within .001

[Shane1234]

will do james. I had my local mitsu rep on the phone, as well as the deco tool supply rep in person, trying to get the galling out. we got her real close, and the next step might be to switch over to the gt inserts. currently we are using the mt (pressed, not ground) inserts, with the u2 chip breaker. we got it close enough that i could trust it with repeatability.

part of the issues we are thinking is a) its 1045 material (stress proof), so it doesn't chip out well, it strings out and maybe tends to cause loading up. slowing down the IPM and turning up the rpm to try to thin the chip didnt really affect it much. b) its flame cut, with induced warp near the larger hole (yeah, 1.4" material warped is freaky). c) possibly induced vibration from not enough support on the jaws. the flame cut part we receive from the customer has slight taper on the side walls, with slight variations from part to part on the contours. We ended up having to ditch the contoured jaws i made out of 3x3 a2 because the more contact I had with the part, the more it would throw it out of whack for location wise (36" long part, with 1 hole pretty much at the very end of each side). Seems less is more to control the part. So now in the hard jaws is only 3 touch spots for the part, on the far right vise i have the x & y touch off that the part must rest against, and the other vise on the far left only only clamps on the y. I have thought about adding toggle clamps to help the situation, but first i might try C clamps to see if actually does anything to solve the issue.

[Shane1234]

the part aint hard by no means, its just that any slight variations by the flame cut mess with this part, whether thats in warp, contour on how i jig the part, or the taper on the side, making it less area to clamp on...... and since the part is so long, variation on the angle can throw the laft hole way out of tolerance if I clamped more based on what the contour should be....

[Shane1234]

well, i ordered a 1.5625" & a 1.25" insert drills from mitsu, and using a finish bore for one hole, got it down to 1 minute, 45 seconds, and I think i sold my boss on getting another boring head to do the other hole instead of using an endmill, which will save me another 20 seconds......

[Delw]

Shane nice job. thanks for the update

[Shane1234]

no problem. using 2 kurt vises to hold it, trying to think of a faster way to load/unload without throwing too much money into it. plus we are doing plug gauging in the machine before the part gets unclamped, so that eats time right there.

[Shane1234]

http://i488.photobucket.com/albums/r...CAfan/mvs1.jpg
http://i488.photobucket.com/albums/r...CAfan/mvs2.jpg
http://i488.photobucket.com/albums/r...CAfan/mvs3.jpg

the part is 36 inches long, 1.4" thick, and 49 lbs. got machining under 2 minutes now! next thing is to get load/unload times down without having to throw a huge chunk of change on a pallet changer....... any ideas?

[Delw]

Shane you have a probe on that machine right? can you use that to check the parts instead of a pin? I wouldnt use the standard bore program because that checks x plus and minus y plus and minus which is the same spot your ball screws change directions( which could cause a bad reading if you have loose ballscrews), but checking it maye at a 45 degree angle would work. renishaw would more than likely help you write a simple marco to do the job, if not some of those guys in the haas forums are smarter than ****.