T.I.R. probs drilling

[jhauschild]

I'm haveing problems drilling concentric to the O.D. The work is being done in a Hydromat Indexing machine in which the tooling is rotated and moved into the material. I have tried gundrills and reaming and fluted drill to size, with or with out a previous hole, and we always end up with a fairly good entrance hole, but the exit is off around .003 to .005 or more. The machine is squared up and lined up as well. The part is compacted metal, cuts like a gray cast iron. Also the feeds and speeds have been brought up and down with little to no difference. Does anyone have any ideas?

 

[gbent]

You havn't given any relative information about sizes. Since it's a hydromat, I assume it is a small part. I would allow between .0001 and .001 runout per diameter of drill depth. Whenever I had to make fussy parts with long holes, I always finished the OD off the hole, as I could never get better than about .0001 TIR runout per diameter of depth. Trying to hold 6 sigma, I would want about .001.
As for gundrilling, it seemed we got better accuracy by spinning the part and not the drill.

 

[jhauschild]

The dia. of the part is .562, the hole size is .303, the distance is 4.004 long. The drills are rather long, 9inch. Tried one flute and two both having the same results. The entrance is usually .001 to .004 and the exit is .003 to .008. This even happens when there is a precast hole in the part, Which I find a bit strange. Starting to wonder if it's the machine that is causing the prob. the specs on the part is .0045 and we need to keep it as low as possible. Has anyone ever used the TX drill by Kennametal? It seems, thou, that what ever drill or reamer I used I allways ended up with the same results. It's getting to be a pain in the back side.

 

[Viktor]

Unfortunately, there is not way to solve the problem with rotating drill, reamer etc. No matter, you have pre-drilled hole, pore-cast etc., not matter what type of drill you use –the results is the same (only the magnitude of deviation of the axis of the drilled hole changes). Unfortunately, the tolerance you are looking for is a way too tight for trying to solve the problem by altering drill design. In my opinion, if you even succeed on one drill, the next one would not guarantee the same result.

The proper way to solve the problem is to rotate the work or rotate both, the work and the drill.
Viktor

http://viktorastakhov.tripod.com

 

[gbent]

If your .0045 is TIR on the back of the part, I don't think you can make the part without 100% inspection and a large amount of scrap. That is true position accuracy of .0022, and will be hard enough to hold on the front, let alone the back. If I had to give it my best shot, I would drill about .88" deep at .296" diameter. I would jig bore ream (thru drill bushing against face of part) to final size .75" deep. I would then drill thru. (I know it's an ugly process with 3 stations) I wouldn't want to have to guarantee 6 sigma better than .010. Will engineering change tolerances?

Good luck, and let us know if anything works.

 

[jhauschild]

We do use a carbide bushing to guide the gun drills. The bushing cradles the front of the part. I have been getting a consistant .0004 to .001 on the entrance with a solid carbide gun drill. I am drilling from both ends, meeting in the middle. then reaming. The center of the part ends up with about .003 TIR. But yet it seems when i try to continously run it all fails. I personally think it won't ever work out. We are looking to run about a million parts a year on this thing. I have to say that I've become less and less of a Hydromat fan. Considering what we just paid for the thing and what my managment expects from the machine I see nothing but grief. And because Hydromat told them it can be done on the machine they think it can be done easily. A person would take into consideration that they told us that as a sales ploy, nahhhh. I like my turret lathes much more now. I do have a meeting today to present my case on the machine and the tooling I have used and would like to use. So on and so forth......

 

[Viktor]

Dear jhauschild

I believe I can help you out. Being a specialist in deep-hole drilling

http://gundrilling.tripod.com

, I can tell you that the problem can be solved if a proper approach is taken. According to your last message, you have a solid carbide bushing. The next step is to get proper gundrill to assure minimum possible runout and hole deviation. Gundrilling is a system which includes many parameters and components
(if you have a chance, look at my article published in Cutting Tool Engineering, December 2001: GUNDRILLING KNOW HOW).
Only when these components are coherent, the desirable result can be achieved. One missed link and you out. The prime concerns in your case are: gundrill design and geometry; alignment “starting bushing-drill holder”, accuracy of the feed motion in terms of it straightness (the drill path just copies this motion so the hole straightness cannot be better that the accuracy of this motion), clearance in the starting bushing (the difference between the drill and bushing diameters), the distance between the faces of the bushing and the part, type and pressure of the coolant.

Regards
Viktor

http://viktorastakhov.tripod.com

 

[jhauschild]

Here's another question for you folks. With what we have to work with, what would be a good feed and speed for a two flute gun drill, "Drill Masters", in inches per rev. and a suficient RPM? Again the material being a compacted powder metal that cuts like grey cast iron, drill size at .303" traveling up to 4". The drill has a guide bushing. And the machine speed at up to 300 rpms.

 

[Viktor]

Although the regime to start with can be follows:
3000 rpm, 5ipm (it could then be increased up to 4000 rpm, 7 ipm)
the two-flute gundrills are not suitable for your application at all. The problem is that they are not self-centered (self-pilot, as we call this feature) so you cannot, even in principle, to get straight hole (I mean, as straight as with a self-piloting drill). Therefore, I would not recommend using these drills for your application unless you enjoy troubles.
Viktor

http://viktorastakhov.tripod.com

 

If you are feeding bar stock into the machine, mark the stock and see if there ia a relationship between the runout and the mark. Is the hi point of runout always in the same place? If it is your problem may be alignment. If no realtionship is found then the problem is more than likley in the process. Try an undersize drill and a Shefcut reamer. This reamer has a large carbide wear pad that helps to straighten out a hole. Be sure to keep all tools as short as possible. Let me know.

Fulton Tool Co.
Peter Russell

http://WWW.Fultontool.com

 

[jhauschild]

Well, since the last time I left a reply things have changed. We are going to drop the gun drills all together and go to a TX style drill or even a margine drill, like Kenametal's. And it seemed before that our reamer size to hole size may have been a bit of a factor. There was only about .006 material left for the reamer to clean out, and since there was up to .005 runout the reamer was free to do what ever it wanted at times. The drills we were using where not suited for what we are doing. They were Drill Masters gun drills at a .303 size carbide head and a crimped tube shaft that made the drill very weak. You could bend it in your hands without any effort. Spinning it at 2000 to 3000 RPMs, even with a carbide guide bushing, it would whip. Can't cut a high tolerance hole with that and the cutting times needed to make the 8 second cutting time we are expected to get from the machine. I would like more info on that reamer, the Shefcut one. I have smaller lathes of which dilling probs
resulted in the use of 3/16 bore bars. The parts are pressed with a hole in them already and those holes aren't very straight. Could this reamer do the trick, straightening the hole out as it cuts.?

 

[gbent]

Yes, a Shefcut style reamer could probably straighten out the hole if it has good starting conditions such as a short bored hole. I used to use a solid carbide head, steel shank, thru the tool coolant version of those reamers to finish valve guides on AMC prototype cylinder heads (.3125). It is only a single lip cutting tool, so feeds can't be very agressive if there is much stock. I don't know where to buy them, however. I had a sample, and had a speciality tool shop duplicate them. I have heard some people refer to them as a gun reamer, and others say they were not.

 

[Viktor]

It should be very clear that any reamer, including gun reamers, cannot, in principle improve much the position of the drilled hole axis. It can improve diametric accuracy and surface finish (surface integrity as we call it which is a bit wider term). It a hole is drilled crooked, not much can be done to improve it.

About “whipping” of gundrills. This is a myth. If a gundrill designed properly and has proper support including a whipguide, it should not whip at all. We use gundrill for automotive applications which we run at 8,000-12,000 rpm and whipping is not an issue when the drilling system is right.

The apparent low stiffness (or as we call it, bending rigidity) has nothing to do with whipping. It does not affect the performance of such drills. Gundrill MUST BE MADE for the application as well as the drilling system.
Viktor

http://viktorastakhov.tripod.com

 

I would put in a REAL GOOD bitch with hydromat, and tell them to tweak it in, seeing as how they said it could be done in the first place. If you're looking for 8 seconds (how many stations is this machine?), and they sold it to you under that pretense, they had better put their engineering where their mouth is and come up with a solution for you. Sounds like a very tight tolerance to hold on that length. gbent made a good point about finishing the od off of the hole, but now you're talking about another machine. You could cell the hydro and a finish grinder next to each other, and have one babysitter for both. How concentric can your pm producer make a hole for you in the blank part? If they would core it to within a couple thousandths of finish, it could then be finish honed or reamed, but it sounds like you may have tried this already. Dunno, just throwing out ideas. Good luck!

 

[jhauschild]

We have three stations doing the drilling each doing a third of the part. The first third is being done with a .303 gundrill, the second is a .302, the last is again a .303 from the other side. The first and last drills are guided by bushings that cradle the face of the part, the second is using the first drills hole to start it off. The part is then faced, chamfered and O.D. features from both sides at the same time. Finishing up with the reamer at .3125. The machine is a trunion style not horizontal. We used this set-up today with Star cutters drills and our CPK's were fairly good, but not good enough. I feel that we aren't leaving enough material for the reamer to clean up. Each stage of the drilling starts with a good hole but the end of it is larger and out of round. Also did some testing and found out that the drills start to walk once the carbide portion gets past the bushings at the start. Lots of little variables that seem to be playing their part in the works.

 

Have you had your toolgrinder try a different nosegrind on the gundrill? Your feed may also be too high. Have you tried pushing the first gundrill a little more than halfway through, and then use a second gundrill to come from the other side? Seems to me you may be getting your runout when you use that second unsupported drill to extend the hole on the first side. You could section a part and measure runout at the start and finish of that second drill to verify or deny this theory.

 

[gbent]

If your holes start clean, and are oversize and oor at the bottom, I think you have chip disposal problems. Do you have enough pressure and volume of coolant? As for material left for the reamer, the less the better. As long as the drilled finish is cleaned up in the hole, you are leaving enough stock.

 

[Viktor]

I would not agree with the statement “less is better” – this is the problem. Your stock for reaming is too small so the force generated in reaming is not sufficient for self-piloting at all. So, you supporting pads (or supporting area in case of Star Cutter reamers) cannot guide the reamer properly. Moreover, if you use Star Cutter gundrills with their “famous” stepped-slash point grind this is inherently the cause for hole axis deviation (the standard calls it “position error”). Use normal gundrills. Viktor

http://viktorastakhov.tripod.com

 

JHAUSCHILD---When I started reading your post---I thought small start hole and add a second operation "wire burning".---Then I noticed the large quanity you need to do, and I bet that would be way to slow for you.---since any drill that dia and cutting that far will prob drift more then acceptable, I would try a undersize drill (about .025 or .03" undersize and drill through (try .004"/rev feed and .075 peck to start).---then follow with a two flute (soild carbide for rigidity) end mill about .01" undersize (It will act like a boring bar, this should fix the drill drifting problem and should put a crooked hole on location)--I bet you will not be able to reach all the way through with the End Mill but if you can go at least 2" deep you can flip the part over, End mill (use .1" pecks on the end mill and .006" feed/rev to start with) the other end of the hole to meet in the center then run a reamer through.---If this works, I am looking for a job---lol.

 

[jhauschild]

We have tried different grinds from a b;unt angle to a sharp one. Getting the run out to settle down is hard enough as it is, but we have to maintain an 8 second run time. We have to push the drills pretty hard, in fact had a drill loose its head at the weld. Go figure. We have had a Star cutter rep. working with us for two days now and he has been pretty helpfull, but they just don't seem to get it that we are pushing the drills too hard. 3600 Rpm's at .004. The drills are Drill masters with the Star cutters cut on them. Star cutters factory burnt down so we ended up with the Drill Masters drill, but we had them work their cut into them. As far as testing the parts cutting them, sectioning them.....etc. Have been doing that since day one. Most of our tweeking has been done as a result of those tests. We are sitting fairly good as of today. after reaming we are at .001/.002 to .002/.0035., with a few fliers mixed in. I figure that we will be getting smaller drills and take more out with the reamer. It's pretty certain that the reamer is bouncing around the inside. And the uncuncentric holes that it is following gives it room, at times, to not do much of any "reaming" at all. This whole gundrilling thing has been a learning ordeal for me. I have been programing, tooling, and setting up Mazak's, Hitachi's, tsugami's, Miyano's, and CMS's for eight years now and never have I had to deal with gundrills. Always found a way around them, until now. This time the tooling was choosen by someone else. someone with very little machining back ground. And as stuburn as a mule! It's has taken me three weeks to get them to listen to me about the reamer size to hole size prob. I've started smoking again.LOL.