Order of operations

[Rotate]

Let say you have drill and counter sink 5 holes using a milling machine(non-production scenerio). Do you first drill all the holes and then change the tool to counter sink, or do you drill and counter sink each hole at a time. Because I don't have a DRO, I find that I do the latter so that I don't lose the position. It does mean that I have to change the tool 10 times but it's better than having a counter sink which isn't concentric. Is this the approach that most HSM use?

This may sound like a silly question, but when you don't have any formal training in the field and you're tinkering all by yourself in the garage, you start to wonder whether something you're doing is completely out of wack.

Albert

[t&cgrinder]

Hey Rotate.

I think you are doing the right thing. If you want to save some time and effort check out MSC. They have some adjustable countersinking bits that attach to the twist drill depending on the size you are using. They are called Cham-Bit, also Severence tool company makes a similar tool.

They slide up and down on the drill and lock into place with a set screw.

Paul

[John Stevenson]

Albert,
I do a lot of second op work for a local laser company. I drill and tap or drill and countersink literally 1,000's of holes.
I usually set the CNC up to drill the holes as it's automatic and I can flood cool.
I then swap over to a small mill drill to either tap or countersink.
I've tried loads of different types of countersinks, Some have lasted OK, most have chattered, some have been absolutely useless and some have left great burrs on.
From costly personal experiance I have found the best ones to be one sold by J&L but made by M.A. Ford in the USA.
They are TiN coated single flute and the J&L part number of the big one is MUT-89353H
All this series start MUT
Being single flute they don't chatter and line them selves up on the pre drilled hole.
One job I have to do is a 10mm hole [ 3/8" ] countersunk to a head diameter of 30mm [ 1.18" ] which is a big and deep countersink, far deeper that a 10mm screw.
These csk's do this with a thick continious cut coming off and keep doing it. I can get between 2,000 and 3,000 holes per tool.

I have just orderd an indexable countersink with three tips in it for doing some 13mm stainless countersinks but as yet it hasn't come. Be interesting to see how good this is against the Ford TiN one.

John S.

[rmatel]

Albert,
I'm also a newbee and do the same as you; change all tools without changing position.
Also change to a tap to start threading.

You should see the ritual I go through to line up each spot before machining ;-)
Bob

[Peter S]

Rotate,
I can't see anything wrong with the way you are doing it. If you don't have DRO, I think you are on the right track. It is the safest way. Even with DRO, I sometimes do it either way, depending... For example, if you are countersinking (or counterboring), and you want all the c/sinking to be the same depth, then it may pay to do all the c/sinks at the same time, so you can use the quill stop. You don't want to be adjusting the quill stop at every hole. Another way is to do your deburring, c/sinking or c/boring later on a drill press using depth stop, with the job "floating" on the table.
It also helps, on your mill, to have a free-turning drill chuck, ie one you can easily spin to adjust with your hand. Sometimes they are stiff and therefore slow to change tooling.
Generally, if I am using just a drill chuck, I will stop on each location, and finish that hole, eg centre drill, drill, tap etc. and then move on. However if I have to change to say a taper shank drill or a milling cutter, I would do it the "other way".

[C. Tate]

Severance and Sevcal also make a tool for spot drilling and chamfering/countersinking in one operation. The tools come in several sizes and several angles. They work very well on holes in the .375 range and seem to last a reasonable amount of time.

To set the depth on a tool such as drill or countersink you can make a collar to go around the tool and set screw in place. Simply drill till the collar touches your work piece and all of the holes will be the same depth. This is allows you to remove the tool from a drill chuck change to another tool and not have to set the stop each time.
Remember this may not work if you are trying to hold close tolerances on depth or if you have finish requirements on the surface you touch with the stop.

[This message has been edited by C. Tate (edited 05-27-2002).]

[Oso]

I have several countersinks, and a couple of them are piloted.
They have a place for a pilot stub just like a counterboring bit has. Then it is easy, you just use a pilot the same diameter as your hole, and you are right on automatically.

An aircraft countersink is both piloted AND settable for depth, so all the c'sinks are exactly correct. It has a housing sort of like a housed drywall screwdriver bit, but somewhat more adjustable.

[Thrud]

Albert
It is only "wrong" if you damage the tools, the work, or God forbid - yourself. Do what is easier for yourself and your conditions.
Like Peter I often use a piloted counterbore for Allen capscrews - it is not really critical in most cases and is no big deal. I revert to the same thing you are doing when I have to have a countersunk hole.

I use a Severence 6 flute Chatterless countersink - the Single flute was far more money here. These must be returned to Severence for resharpening or they chatter like crazy.

I buy cheap uniflute CS's when I need odd ones and get the Foredom and the points out and put a razor sharp edge on them for wood, plastic, Aluminum, and Copper. They are never used in steel or fingers - to damn sharp! They whiz through wood and Aluminum really well.

John,
Have you tried the Weldon Zero flute CS's? They are not available locally, and I wondered if they suck or not. Good luck with the insert CS - let us know how it works out.

[metal mite]

Guys,

An old jigbore operator told me years ago "Spot drill all your holes first with just a dot (not full depth centerdrill)"

Everyone has an error frequency, mine is one hole in fifty. Transposed digits usually.

The chance of screwing up the same hole twice (dot/centerdrill operation) is 1 in 2500, considerably better than the 1 in 50 I average.

If you dot all your holes, than come back and centerdrill, an error will stand out like a sore thumb.
If you have just a little "dot" off location, usually an inspector will pass it.

If you are doing a casting and a hole in a boss is off, you can readjust the whole pattern to equalize, if they are just dotted.

On critical work that is what I do.

Sometimes I lay out the holes with marker or grease pencil first.

It is quicker like someone above said to dot/ centerdrill on the mill, and drill/tap/ream etc, on the drillpress.

mite

[Paul Alciatore]

Rotate, I do a lot of one of a kind jobs that are just like what you describe. I always do all the holes with a given tool/drill at once and rely on the handwheel calibrations to return to the same spot.

I use layout dye and scribe cross hairs at each location first. Then I use the center drill-spotting technique that metal mite describes to insure I am in the right place. I find it's easy to see even a small error under 5X maginfication. Haven't clocked my percentage of misses but It's probably even higher than his. This allows instant correction.

Then I center drill until I have a small cone to start the next drill. When all the holes are "center drilled", I try to drill a pilot hole with a small bit about the size of the web of the final drill. On many jobs this amounts to 1/16 or 3/32s for all the holes. Only then do I mount the final size drill and finish all the holes.

I return to the location of each hole using the handwheel scales. With a properly adjusted machine and proper attention to backlash I find I can return to the original location +/- a few tenths.

I find this a lot faster than changing bits several times for each hole and it allows me to use the quill stop to set depths.

[Rotate]

I have been told not to start the hole with center drill because the angle on the center drill is smaller than the normal drill so the drill can still wonder. I have noticed this myself, and I now use either 118 or 120 degree spotting drill to start the hole. I only drill deep enough so that the opening is slighly larger than the web of the twist drill. Any comments?

I do layout my work but I never center punch as I've found that I can position the work much more accurately than where I center punched. More often than not, I've seen the spotting drill touch down just on the edge of the center punch. Needless to say, I only do this when I need to position the hole very accurately. Other times I do center punch and come staight down with the drill. Am I correct in that if you spot drill, center punching is unnecessary?

All this operations makes me think that vertical mills should have turret style spindle attachment.

Albert

[halfnut]

When you have to crank out the locations you hate to move from that spot. I love a keyless chuck for this sort of thing. The countersink will go back to same spot as far as depth goes with a keyless. Set the depth for the countersink, I cut off long center drills so they are a bit longer than countersink, and the drill will be longer. I do this when I can, even with a DRO.

Metal Mite, or should I say Kap, brings up the point of doing some layout, lead pencil or marker is good enough. This helps to avoid mistakes, and often those mistakes are .100 or .200 errors, easily avoided by some simple layout. Same thing goes when using a DRO, sometimes dirt appears and the scales are wrong, hate it when that happens. The DRO always messes up at the worst time, something to do with Murphy's law I reckon.

[L_Miller]

I look at the time it takes to change a tool VS. moving location Vs. changing part.

If the holes are real far apart wich = lots of cranking and counting of turns. I change tools.

If the holes are near one another. I move to each location before changing tools.

If the part can be put in a vise with a stop.
You can center drill all the parts on that location. Move then go through all the parts again. Move and go through them again.
This works great if you can swap the parts faster then you can swap tools. If the parts are bulky and big... not so good.


You can also use a marking pen and put marks on the machine that go with locations that are a few inches apart.

Move to your first location. Put a big mark on the side of the table's part that slides and right on into the part that doesn't slide for X and Y. Then move carefully to next position. Mark this one too, using the same mark on the part that don't slide as a guide as to where to place it on moving slide. Add #2 and any little dial numbers to it in ink. Like if you have .200 dials and you need to move 5.375" then it will land on .175. So I'd mark .175 along with hole #2.

All this is doing is making a cheap scale that lets you zip to the ballpark location, but still using the hand dials bring it home. Rember to always keep back lash in mind. Bring up to numbers in the same direction. If you over shoot back up a turn then try again.

This also works great on the knee if you need to run it up and down a bunch times for longer drills and stuff.

Acitone works great at removing pen marks when finished.

Later

Larry Miller



[This message has been edited by L_Miller (edited 05-29-2002).]

[John Stevenson]

Well I got the insert CS today from J&L plus 5 spare tips. I was a bit dubious when I saw the design but I tried it. What a total and utter waste of money. It's a single inset tool and the tip sticks out about 30 thou from the body. This means that the tool isn't suported but just has this one tip cutting.
It's probably made for fixed machine drilling where the work is bolted down.
Trying to use it in a drill press is a waste of time. All that happens is that the insert digs in and just bounces around the hole.
I fully expected the insert to be level with the body so the opposite side of the body supported it.
It doesn't look nothing like the one in the cataloge. J&L no TDX 19000H shows one with a square tip at the edge. Compare this to
http://homepage.ntlworld.com/machines/csk.JPG

Well I don't see how anyone can charge $76.50 for this thing. It's on it's way back tomorrow.

John S.

[Peter S]

Rotate,
I don't have any trouble with using centre drills. Can't really see where that idea comes from...they work well. If your drills are not following the centre drill location, they may not be ground evenly.
You shouldn't be centre punching locations that you want to pick up on the mill. It is much easier to locate on scribed lines. You can't locate accurately using a centre drill either, what you need is a sharp spinning point. I use the type that comes in the "wiggler" or edge locator sets.
Another well known method of picking up on scribe lines is to use a "sticky pin", a lump of plasticine with a pin stuck in it. These can be found stuck to the side of most Bridgeports heads in this part of the world. These are used when you have a milling cutter, or some other cutter in the collet, and you don't want to remove it. You stick the plasticine to the end of the cutter, and start her up. Use your finger to get the sharp end of the pin running true, then wind your handles to pick up the scribed location.
When using any sharp point like this, you can use a simple magnifier (the eye type), and bright light, to get pretty accurate location.
The other method, which I always prefer, is to avoid any form of marking out, and work from a datum of some sort, and place all the holes, slots or whatever just by indexing the tables. Which brings up the different methods of edge finding...
I guess most of us have valid ways of doing the same thing, some of the differences just relate to how accurate the location needs to be.