PDA

View Full Version : Problem drilling holes on the centre line of items



loose nut
04-06-2018, 11:02 AM
1 - put block in vice
2 - pick up edges on sides and use divide by 2 function of DRO
3 - OK it should be right on the center line of the block

But some times it is off.

I pick up the edge with an edge finder and even a 3D Taster. I use a center drill or if it is a bigger drill a spotting drill to start the hole so the bit should be in the correct location but it seems to deflect or jump to the wrong spot. Frequently I will double check the location, with a caliper after putting a tiny mark with the spotting drill and it will appear to be in the correct location. I know twist drills are not the best for accurate work but getting a .005 or even .010" error in position seems to much. I know others with the same problem.

Any ideas or solutions.

RB211
04-06-2018, 11:16 AM
Center drills are for lathe work, use a spotting drill. If a round object, mill a flat.
I think the error is in your use of the edge finder and DRO. Are the dimensions of your block accurate? Divide 2 by what exactly? You can measure the workpiece with the DRO, then divide by two. Edge finders are simple, but can be off by .002 to .003. If the round types deflect out, that’s beyond center, need to bring them back a tiny bit. Unless you are NYCCNC, and spend money to make up for lack of manual machining skills, spend extra time on metrology skills and use a liberal amount of DTI’s and Noga holders and actually verify things are what you think. Also, if your DRO isn’t glass scales or something better, get glass scales or something better.

danlb
04-06-2018, 11:23 AM
The only thing that comes to mind is the tramming problem combined with parallax that one of the threads talked about a few weeks ago.

In his case, the head was not in proper tram, so when he used used a short center finder and a longer drill the hole moved over. Are you using two tools with the same extension?

Is the error always in one direction? That would point to the parallax problem as mentioned above.

Dan

Mcgyver
04-06-2018, 11:30 AM
If you are using spot drill or end of centre drill to start, my first suspicion is that you're not really where you think you are vs the drill somehow going off 10 thou from there. The short stiff nature of a spot drill shouldn't let move about. I would usually pick up one edge and move in 1/2 the part dimension, but I doubt that matters. Not sure what it could be....if you pick up the two edges of something of a known length, does the DRO tell you to go to the predicted middle? i.e. 1/2 part, the DRO tells you go in .500"?. Are the machine tools ways tight - no overt movement of an indicator needle if you try and manual move them about? how about the quill? These may or may not be likely suspects but you have to start with elimination.

edit - yes of course, tram as Dan suggests, curious how that checks out

David Powell
04-06-2018, 11:37 AM
Sticky or worn edge finders , old eyesight and, maybe DROs that do not tell quite the truth can all add up to put you off by a few thous. I usually find both edges with the centre finder, divide by 2 then zero the readout and carry on.( I build steam engines not rocket parts) However, if I REALLY want the middle I go again to the edges. Quite often I find a thou or so difference, so I rezero as appropriate and go again until both readings are equal. IF possible use the centre finders against the part and not the vice jaws , tilted vice jaws may throw you off a bit. Hope this helps. Regards David Powell.

rklopp
04-06-2018, 11:42 AM
Check your edge finder technique by putting a test indicator in the spindle and seeing if you get the same reading picking up the high point on each side of the part or the faces of the opposing vise jaws (if the part is sunk below the top of the jaws). If that turns out <<0.010, then that rules out edge finder and DRO issues, and points more to drill wandering, and possibly tram depending on whether Z changes a lot between edge finder, indicator, and drill. Your tram would have to be very far out of whack to accumulate 0.010 lateral movement in a few inches Z move. Also try drilling the hole and then sweeping it with an indicator and see whether the hole is on the spindle axis.

danlb
04-06-2018, 11:53 AM
For those without a DRO with the "1/2" function, it's almost foolproof. Assume a 4 x4 inch block in the properly aligned vise. Assume you just want the center of the X axis.

You pick up one edge using the handwheel for the Y axis. Zero the X axis there. You don't even care what the diameter of the tool is. Then you move the table to find the far edge. The DRO should then be reading 4.000 plus the diameter of your edge finder. Press the 1/2 button and it shows you the coordinates for the center of the block.

In theory, it even cancels the small offset that edge finders tend to have, where they 'kick' a few thousandths after contact. As long as it kicks the same on both edges the DRO takes care of it.

After using it for years I finally realized it works for symetric holes too. Even if you start by being offset to one side or the other, you end up with the center of that axis. Then you repeat on the other axis and you end up with 0,0 at the center of the hole. It's quicker than using a wiggler, although a wiggler does work too.

Dan

JoeLee
04-06-2018, 11:57 AM
When you zero the back of your vise you should always clamp something in it to put force against the back (fixed) jaw before entering zero into your DRO.
If that's how your zeroing your DRO.

Loose spindle bearing or drill walk could also be coming into play. There are a whole lot of things that could be causing your error.
An off center chuck arbor or chuck jaw could also cause this.

Other possible contributing factor..... is your work square??? Is your vise tipping the work when you tighten it??

If I'm going for real precision I always square up my work before milling or drilling. Flat bar, even ground flat bar is not perfectly square.

JL.............

J Tiers
04-06-2018, 12:15 PM
Some of your answers may need tweaking.... he has checked location with caliper, and verified it is where it should be.

It seems that the problem is not with locating the spot, but with having the drill follow the spot and accurately locate where the spot was (which was verified)

SO either the calipers are always "off" just enough to make the spot seem to be on center even though it is somewhere else (quite a co-incidence), OR the issue is with getting the drill to go down where the spot was.

Edwin Dirnbeck
04-06-2018, 12:39 PM
Center drills are for lathe work, use a spotting drill..
I respectfully diagree. I ran a Moore jig bore for years drilling and borring thousands of holes ON LOCATION. for interchangable stamping dies.I found the best location came from using a new 5/16 usa made center drill. Many times you could skip the borring operation . Just center drill, drill and ream..And of course siting at the Moore it was easy to go back over your finished work with the special Moore jigbore indicater holder and verify locations Especially in later years when they had digital readouts installed If the original poster puts a 5/16 good centerdrill in a 5/16 collet ,the hole WILL BE ON LOCATION THE TIP DIAMETER ON A GOOD CENTERDRILL ACTUALLY HAS RADIAL RELIEF AND CAN BE USED as a short stuby endmill I say this to ilustrate how small and ridgid it is and how well it resists the inevital forces trying to push it of center.Another illustration is trying to spot a hole on and angled surface ,say 45 degrees. A spotting drill will walk all over the place.Where a spotting drill exells is locating the hole prety good AND SIMULTANEOUSLY CHAMFERING THE HOLE ..Edwin Dirnbeck

rklopp
04-06-2018, 12:46 PM
it was easy to go back over your finished work with the special Moore jigbore indicater holder and verify locations Especially in later years when they had digital readouts installed.Edwin Dirnbeck

This is what Loose needs to do, but without a special Moore indicator holder.

J Tiers
04-06-2018, 12:58 PM
So....

Locking the table before drilling? It is not unknown for the drill to "kick" the table, especially with smaller mills. Or kick the work, if not securely clamped {"but all I am doing is drilling holes, not pushing the work into a cutter").

Not spotting in a way that actually is bigger than the center chisel edge part of the drill point. The chisel edge on a drill tends to make it "walk around", and it is best to make the "spot" larger than the chisel edge of the following drill, so that the drill will "locate" and not "walk around".

Mcgyver
04-06-2018, 01:00 PM
Center drills are for lathe work, use a spotting drill.

yes, but if you're just using the end point of a centre drill, it is essentially a very rigid spot drill. Otherwise, agreed.

Forestgnome
04-06-2018, 01:04 PM
I'm thinking most likely slop in the quill. When I want a real accurate hole, I scribe, prick punch, center punch, then run a flat file over the surface to knock down the metal displaced around the punched divot.

Edwin Dirnbeck
04-06-2018, 01:17 PM
Spotting drills didnt become widely known until everyboy bought vertical machineing centers. People started saying "why not chamfer the hole at the same time that we center drill them". Edwin Dirnbeck

DEVILHUNTER
04-06-2018, 01:22 PM
Had the drilling in place problem when I first started working with my mill. After a while I discovered that the column was tilted, so any time I changed the tool from a short spot drill to a long drill, the point of the tool was in other XY position.

JoeLee
04-06-2018, 01:56 PM
I'm thinking most likely slop in the quill. When I want a real accurate hole, I scribe, prick punch, center punch, then run a flat file over the surface to knock down the metal displaced around the punched divot. I've seen and had prick punches slide off the scribe line when the point sinks into the steel.

JL...............

ahidley
04-06-2018, 02:17 PM
Spotting drills are stiff but try a split point drill. They stay true.

If there is any play in the quill that can be an issue. Especially if the quill was LOCKED for using the edge finder and not slightly LOCKED for the drill to start the hole

The Artful Bodger
04-06-2018, 03:39 PM
Drills, and I assume similar tools, will wander off if the first contact is too heavy. My technique is to make contact with a light pressure then pause the feed so as to give the drill a chance to 'mill' a divot perfectly concentric with the machine spindle.

old mart
04-06-2018, 04:41 PM
Make sure that locking the table does not move something. Use stub drills if possible, solid carbide drills are better still and could be used as a starting pilot. If you have an optical device to go in the spindle, it can also be used to see if your quill moves when it is locked and unlocked.

MattiJ
04-06-2018, 05:23 PM
Drills, and I assume similar tools, will wander off if the first contact is too heavy. My technique is to make contact with a light pressure then pause the feed so as to give the drill a chance to 'mill' a divot perfectly concentric with the machine spindle.

And split-point is lot less likely to "walk off"

Some of the Split-point pop rivet drills have very short flutes and make nice spotting drill. And are dirt cheap compared to "real thing"

J Tiers
04-06-2018, 11:16 PM
There is a LOT of merit in the idea someone mentioned above about light pressure.

I have "drawn" holes back on-center, even with a loose quill, by light pressure and basically letting the drill act as a milling cutter to make a good starting cone before getting into serious drilling pressure.

heavier pressure does lead to more "walking" of the drill, and even more "wandering" after the drill is started. Some of that may be due to a bad grind, some just to random things like hard spots.

Paul Alciatore
04-07-2018, 12:28 AM
Gentlemen, TRAM your mills!




Had the drilling in place problem when I first started working with my mill. After a while I discovered that the column was tilted, so any time I changed the tool from a short spot drill to a long drill, the point of the tool was in other XY position.

tom_d
04-07-2018, 12:42 AM
What type, or style of mill is being used here?

The way I read the OP's problem is that he has started off with using both the center drill and spotting drill, confirmed his spot position location, and then sees the problem when switching to a twist drill to complete the drilling operation. This tool change most likely requires a move of the quill to accommodate a change in tool length. If the machine used is along the order of a traditional Bridgeport type mill then it would most likely be the Z axis of the head not trammed in. If that's the case then the error would be consistent in the same direction.

He says that sometimes the holes are off. The head tram could be the problem going from one set up to another set up. If the errors are from piece to piece with the same set up then it sounds like there is movement in the head, or table, that's causing a problem.

CCWKen
04-07-2018, 12:50 AM
heavier pressure does lead to more "walking" of the drill, and even more "wandering" after the drill is started. Some of that may be due to a bad grind, some just to random things like hard spots.
Tom Lipton (Oxtool) starts the hole then rams the bit through with considerable pressure. He demonstrated this while making a mini pallet. Perhaps it just takes good drills and the right speed.

Paul Alciatore
04-07-2018, 01:06 AM
Yes, nothing says the initial prick punch will be on center.

When I punch and drill I:

1. Scribe the cross hairs
2. Lightly prick punch USING A MAGNIFYING HOOD
3. Use a 10X magnifier to check the location of the prick punch
4. Lightly punch with a fine punch, tilting the punch to adjust the location of the punch
5. AGAIN use a 10X magnifier to check the location of the punch
6. Use a larger punch, again tilting it to adjust the location of the punch as needed
7. Repeat #5 and #6 as needed to get the punch centered on the cross hairs.

With that procedure I can usually guarantee +/- 0.002" or better accuracy for the punch mark.

Now even a jobbers length drill can "find" that punch mark and start on it. But, if I want the best accuracy I start with EITHER a center drill or a spotting drill. I find that the results are much the same with either one of them. I mount the part in a drill press vise and allow the vise to float on the table. The short center or spotting drill will center the punch mark under the tip of the drill. I suspect that a center drill will make a better hole for the next drill to follow due to the small diameter hole it drills at the tip. That small hole, made by the tip of the center drill, will be around the web thickness of your next drill which should follow it almost perfectly. So, center drill, pilot drill, and finally full sized drill.

Yes, it is a lot of steps, but it does work.

When I drill in the mill-drill, first, I have a well trammed mill. No errors due to the length of the drill or the position of the head on the column or of the table on it's vertical slide. Without that, you are just whistling Dixie.

Then I find two perpendicular edges with an edge finder. I find that technique is everything with an edge finder. First, I LOCK DOWN any slides that I am not presently using. Thus, while finding the X edge, the Y gibs are LOCKED and visa-versa. If you don't believe this is necessary, try this: put a DTI in a collet in the quill and bring it into contact with an edge. Now grab one end of the table and push it back and forth while watching the needle on the DTI. If it doesn't move 0.005" or more you have a very tight mill table. Locking the gibs on all unused slides will eliminate much of this movement.

Then I would find the edges TWICE. Once to get in the ball park and the second time with a lot finer motion on the axis to allow the best possible accuracy in the location of that edge.

I often scribe lines on parts that I am going to drill in the mill. This is a double check on the location of the holes, mostly to avoid the dreaded, "one turn" error (0.100"). When I do this, I often find that the holes are offset just a bit from the scribed positions, usually 0.005" or less. For many parts, this is acceptable as the relative locations of the internal features are more important than their relationship to the edges. Such errors are usually about the same for each and every hole or other feature. If not, then I will chase after it when I see that offset when I touch off the first hole. And I have found that this can have many different causes.




I've seen and had prick punches slide off the scribe line when the point sinks into the steel.

JL...............

J Tiers
04-07-2018, 01:16 AM
The tram issue will only come up if you have to move the table between using the spotting drill, and using the actual drill. If you are just using the quill, there will be no issue unless it is really sloppy.

Following a spotting drill (usually short) with a screw machine length drill, will be ideal.


Tom Lipton (Oxtool) starts the hole then rams the bit through with considerable pressure. He demonstrated this while making a mini pallet. Perhaps it just takes good drills and the right speed.

Whatever works.... The key is, both for him and for the situation described by the OP, that you are STARTING the hole with light pressure. After that, you can do as you wish, although "ramming the drill through" is not the best... usually you want to keep enough pressure on for it to cut, but not so much that you begin to split drills, or the like. A sharp drill has a rate of cutting and advance that suits it, and "ramming" with extra pressure is counter-productive at worst, and not helpful at best.

danlb
04-07-2018, 01:52 AM
The tram issue will only come up if you have to move the table between using the spotting drill, and using the actual drill. If you are just using the quill, there will be no issue unless it is really sloppy.



While that is often true, you almost never have a situation where the drills are all the same size and don't require moving either the head or knee to change the tools or to get the depth that you need for the hole.

It's bad practice to use your mill if you suspect it of being out of tram even one degree. As Paul said, Gentlemen, TRAM your mills!

Dan

Richard P Wilson
04-07-2018, 08:10 AM
Gentlemen, TRAM your mills!

This point was covered at some length recently in the CNC section in a thread called 'Albrecht chuck/CNC', and concluded that if the head is misaligned (and it need not be misaligned much) then changing from a short tooling set up, like a spotting drill, to a longer tooling set up can easily result in a misalignment of 30 thou or more.

loose nut
04-07-2018, 08:41 AM
O, to allay any fear of "out of tram" it is 0-0 in the Y axis and out about .0005 in the X axis, to close to mess with. I understand how out of tram works against accurate work.

I generally use the spotting drills for larger sizes but for the small ones (3/32 or less) I use center drills. Smallest spotting drill I have found is 1/8" and not much good for small drills.

The quill seems OK and the machine (RF-45 bench mill) is not that old at least as far as use is considered.

To explain how I pick up the center of a part. I pick up one side and then zero the DRO, pick up the other and then hit the divide by 2 function and dial back to center. Sometimes I use a wiggler, repeating 2 or 3 times with good repeatability and sometimes a 3D Taster (accurate to under a half thou), it doesn't seem to matter.The "spot" always seems to be in the right position. I can lay it out on the surface plate first and use that to verify the "spot" and it will line up OK. I use a small drill to start and then drill to size, sometimes I drill one size under and then finish to size.

The weird thing is sometimes I will very close to position (a couple of thou, this isn't a jig borer) and sometimes way out using the same techniques. I guess it is something I'm doing wrong.

P.S. I should add that I generally work with small parts, the current ones are 1/4" x 1/4" x 5/8" with a 3/32" hole through one of the 1/4" sides so off center holes stick out.

J Tiers
04-07-2018, 08:58 AM
Just for grins, try doing things asif you had backlash..... coming back past center and then going forward to the setting.

While I assume your DRO is reading the sliding motion,as any real one* will, if a bracket is too flexible, or screws are loose, or if the table gib is loose, etc, there can be wrong display that does not reflect the actual motion. Then reversing motion can "cross the effective backlash" due to the loosely-mounted DRO.



While that is often true, you almost never have a situation where the drills are all the same size and don't require moving either the head or knee to change the tools or to get the depth that you need for the hole.


Dan


Spotting drill, followed by screw machine length drill. Just as in the part (of my post) you failed to quote

danlb
04-07-2018, 02:15 PM
I trimmed out the stuff that does not matter. I won't bother addressing why.

Back to Loose Nut's latest post:

You are dealing with really small sizes. When you are off .010 on a 3/32 drill, that's a lot. It sounds like you are saying that the spot drill is always correct but that the drill is not making it's hole within the dimple left by the spotting drill.

The center drill is likely to have a 120 degree tip. Per https://www.destinytool.com/spot-drills.html you may need to change to a spot drill for a smaller angle or a twist drill with a 135 degree angle. Per the above link, if the spot drill angle is less than the twist drill will result it the flutes digging into the sides of the dimple.

Dan

J Tiers
04-07-2018, 04:25 PM
I trimmed out the stuff that does not matter. I won't bother addressing why.
....

Dan

Dan, it's a wonder your own spit does not burn your throat. You are the nastiest poster on the forum.

oh, yeah.... go ahead and report this post.

machinejack
04-07-2018, 09:00 PM
When I want a hole on location I get the boring head out. Changing work heights will get you off if the mill is not true the spindle may be parrellel to the work, but if the post is not you will be off. If everything is trammed in you should be spot on.

David Powell
04-07-2018, 09:48 PM
I spent the last 7 years or so of my working career running a " First " mill ( and a Clausing lathe). A large proportion of my work was checked, ( BY a Chinese lady named Ying with a vastly expensive co_ ordinate measuring machine )and reports of my work were filed so that any discrepancies could be followed through. What we found was simply that everything mattered. I was in the land of small items, generally from 1/32 holes up to about 1/4". Certainly, if the maintenance gang used "MY" mill on the weekend or night shift I checked the tram before starting my day. We knew of, and tried spotting drills but found equally good results with tiny centre drills. We bought good quality drills, mainly from McMaster Carr, and once they lost their initial sharpness replaced them rather than even trying to sharpen them .Drilling fibreglass pallets generally meant drilling only 10 or so holes before the drills began to dull. We normally worked from an imaginary centre point on flat items, and when allowable I marked that with a small centre drilled hole so that if later modifications were needed we knew that was how it had been made. We began to be concerned if any hole was more than 2 thous off position. I hope this is encouraging and helpful. Regards David Powell.

loose nut
04-08-2018, 09:37 AM
I trimmed out the stuff that does not matter. I won't bother addressing why.

Back to Loose Nut's latest post:

You are dealing with really small sizes. When you are off .010 on a 3/32 drill, that's a lot. It sounds like you are saying that the spot drill is always correct but that the drill is not making it's hole within the dimple left by the spotting drill.



That is how it appears to me. Yesterday I drilled a couple of 3/32" holes and they where OK. .000 run out one way and 2 or 3 thou the other which is acceptable to me for a drilled hole. The next time it could be way off and there is no change in the machine tram or any other set up IE: the vise isn't moved etc. ???


When I want a hole on location I get the boring head out. Changing work heights will get you off if the mill is not true the spindle may be parrellel to the work, but if the post is not you will be off. If everything is trammed in you should be spot on.

Boring a small hole (3/32 or 1/16) is a bit impossible for me.

Me thinks the drills must be jumping around some of the time??

J Tiers
04-08-2018, 09:49 AM
If you are sure the spot drill is in the right place, then please tell us if you are moving the head when you change drills, or if you are just retracting the quill.

On your mill, both the head and possibly the column might have a tram problem.

MattiJ
04-08-2018, 09:56 AM
For tiny holes and parts I would try spotting with PCB carbide drill. Very sharp, reasonably stiff and cheap.
No scribing or punch marks, clean surface and just mill DRO.