I think I know what you are going to say, but just in case, here goes.
I need to make a "large run" of mounting plates - for me that means more
than five :) These will be 0.065" Al, about 6.5x11 in with four or five
sets of related holes. This sounds like a great opportunity to clamp a
stack on my mill, with one catch: several of the holes require some
counter sinking. The design is more set than it sounds. I have one
working prototype, but plan to add some hole sets on the theory that
they will end up being useful.
Would you stack, clean up the edges, drill the holes (they need to be
reasonably precise, at least relatively in the different groups), and
then separately do the counter sinking on a drill press? Next up would
to be position stops to allow me to individually re-clamp the plates to
sink each plate on the mill. The only other alterative that I see is to
make the plates separately; I enjoy milling, but have better things to
do, unless that is really the only viable choice.
If you get serious about making parts, one of the investments you should
make is a micro-stop for countersinks. They control size very well, and
don't need precision locating, due to the use of a pilot. They can be used
in an inexpensive drill press with excellent results. You can stack drill
your parts, then go back with a second operation and do the countersinks.
You can do the same thing by establishing some simple stops on your mill
table, then countersink the same holes in each plate by going to proper
location. You need not clamp the parts, just bank them well against the two
stops. This setup requires that your parts are all drilled accurately from
common datum points----so try to make your plates identical in size, and
insure that they all locate properly when you make your setup. By
countersinking this way, you can set a spindle stop to control the diameter
(or depth) or the countersink.
Regards part size, I've always made it a practice to hold dimensions
closely, and the parts square. That way you can bank from opposite edges
when necessary, and still hold tight tolerances in hole spacing when all the
holes aren't drilled in the same setup. .
That sounds useful, all the more so because I have a Ryobi drill press
that has been largely collecting dust since my mill arrived.
I follow most of that. What do the stops look like, and how do you
ensure the part aligns with the axes of the mill?
I suppose one could mill the plates and use them, still clamped in
place, as stops to position the stops; if that works it would keep the
numbers from the milling of the plates. It seems safer to make the
plates, remove them, position (probably indicate??) stops, and then find
edges/zero based on a square or a squared plate clamped against the stops.
What am I missing?
The more I follow that advice, the more I agree with it. With a stop at
the correct height, it can be very helpful in milling things that need
to be approached from multiple sides. I took advantage of it just today
to alter a part that holds something that a manufacturer changed
"without notice". I was able to seat the affected part on parallels,
find its left edge (the transverse dial was already zeroed on the on the
back jaw), and put an additional hole in it to accomdate their design
change - fit like a glove :)
Thanks for your substantial role in teaching me how to do this stuff.
There's a couple ways you can go about this setup. One, you can use a
couple of parallels that are the same thickness as the slots in your mill
table. The slots are usually fairly close to size, and will have a minor
burr on the bottom corner that will hold the parallels in place when you tap
them in with a soft hammer. Use two of them spaced such that your part
is located on each corner. For the third stop, the side, use something
that doesn't present a large area, and make it anywhere from the center of
the part to the bottom edge. When you bank your pats, they should bank
along the two parallels, which should establish the part dead parallel with
the table, and the side stop will locate the parts consistently with one
another. Once you've made the setup, use an edge finder to orient the
spindle with the part edges, and mark the table and saddle according, plus
set your dials. If you use a DRO, you'd zero it according to how you'd
work. Once you've made this setup, you should be able to remove and replace
each part reliably. It's a good idea to not have any chip traps where
your parts locate. It's also a good idea to work with edges that have been
deburred, so nothing will prevent your parts from locating against the
If you follow the procedure I outlined you should have good luck. Let me
know if you're either confused, or find something I left out. I've used
this procedure for years with good luck.
I think I get it now. An alternative would be to make a fence that can
be indicated parallel to the table and then use a round side stop. Is
that reasonable? If I understand about the parallels, I don't have
anything that thick (though perhaps I should), but I do have a few
candidates for a fence. One tricky part is that the plates are designed
with my cross travel limits in mind, so there isn't much wiggle room.
However, the fence could be an L section that is bolted underneath the
top edge of the plate.
Understood re the edge finder and dials. I do not have a DRO, and am
really not burning to get one. If I can get a scale to sit flat on a
part (clamps sometimes get in the way) or can at least reach an edge and
a point of interest with a dial caliper, then all I seem to need is a
course (+/- 0.1 to get the correct revolution) after which the dial
takes over. I have not yet zeroed based on an internal hole; that might
get me to change my tune, but for now, I'd rather keep the cost of the
DRO toward other things.
Yes, it is---the one advantage of using parallels is that you eliminate a
large area of contact. That's a good thing. It's too easy to get a chip
or other bit of crud between your part and fence, but if you use good work
practice (and an air hose), plus deburr your parts before you start the
second operation, it shouldn't be much of an issue. I'm not sure I was
clear on the "chip trap" I spoke of, but that's what I meant. You have to
be alert to not get things between the part and the stops.
If I understand about the parallels, I don't have
The L section would work entirely, assuming you didn't try to use both full
length edges. It's fairly important that you don't do that. Parts, or
stops, are rarely perfect. You want your parts to locate the same way each
time, thus the small side stop and double stop at the top. Or, you could
reverse it, just make sure you use three point stops, and always bank
against the two to square the part. If you use the L configuration,
relieving the short edge might be a good idea, or you could just make it
very short. The corner should be relieved, too, so it doesn't interfere
That's a tough way to learn to drill, but once mastered, you don't really
need a DRO unless the screws aren't worth a damn. I've always taken great
pride in working without one------and did work that was subject to tight
scrutiny (defense work). I comment you for learning the system----you
can always use the cheat devices, but if you lack the fundamentals, you'll
always struggle with these things. Learning to use the screws is the core
of all the work.
I have not yet zeroed based on an internal hole; that might
Only if your holes relate to one another would I suggest that. As long as
you use the edges as a datum point, you can check your movements with a
scale---which will pick up even small mistakes (transposing numbers, for
example) if you pay attention. It works very well for picking up an added
turn of the dial, or one that has been dropped. That is also one of the
things you must master when you work by this method. Keep your scale handy
at all times. I never run a machine without one within arms reach.
There may be times when you must work from a hole. When that occurs, make
the hole the 0-0 point, then you can crank off directly. Checking with a
scale or caliper isn't all that hard, especially if the hole is a fractional
size, such as 1/8"----you just measure to the edge and add the radius.
Easy enough, and can be done in your head.
Much of this makes sense, but I might still be off re your use of
parallels. Are you standing them on end, like below (looking down from
above the table at one t-slot)?
| | ||
| | ||
| | ||
| | ||
Then I probably do have parallels that would fit, but might not trust
them to stay put or to align all that well. I would also have trouble
clearing them, at least with the parallels I have now (6 inch length).
It does give two nice points of contact, and a round stop at the side
would do the rest.
Either way, this suggests a simple change to the fence idea, something
+--------\ /----------------------------\ /----------+
| - - |
| O <--- mounting holes ---> O |
One would drill holes, bolt a plate to the table, and mill the fence
with a couple of bumps that become the stops. Then indicate off of the
fence to align it for use. In fact, with a large enough plate, one
could put the side stop on the plate, though that is probably not
necessary or even a good idea.
There might be better ways to make it. It would be easiest to do with
Al, but that might not be a good choice for something that takes any
kind of pounding. I probably could make it from steel, but it would be
painful. Is there a reliable way to combine a couple of sections that
might simply need to be faced vs. carving an L out of large plate? It
wouldn't be much good if the pieces slipped.
Mine appear to be in good shape. In fairness, most of the work I do is
making parts that align with other parts made on my mill, so I could be
missing some errors. However, I have matched holes from the outside w/o
problems. Well, there was the one time that a major manufacturer's
drawing was in error on one hole ;)
> I've always taken great
It's really not that hard. I made a simple spreadsheet to help with
windows; given the desired edge locations, it handles the tool radius
and leaving some extra metal.
One thing that still bugs me a little is finding the reverse-direction
dial reading. I pretty much know the amount of backlash, but still
suspect I should do it by feel. What I do is move forward to the
desired reading, then back up until "the screw hits" and note the
reading. Then I go forward again, trying to get the same reading as
before (again w/o moving anything). If it doesn't work, I alter the
reverse direction reading and repeat it. I usually get it on the first
or second try. Please let me know if there is a better way.
I bought a scale as soon as you first suggested it to me, and
immediately saw the value of it. Do you do anything special to position
the scale at the edge of the part? I tend to use my finger as a stop
for it, but there is probably a better way.
Another trick would be to put relevant distances on the drawing. I am
shameless about over dimensioning when it helps. There is a tradeoff
between having the needed distances in view and having so damn many of
then that it's easy to read the wrong one, so some discretion is
required. Certainly a reference to edge distance belongs on a
shamelessly dimensioned drawing :)
For anything that gets difficult to read, I frequently use multiple
dimension layers, and print the drawing one time for each layer. One of
my uglier examples is a plate with 11 slots, 3 windows and 40 holes; I
used three separate dimension layers. More frequently, I use a layer
for milling and another for drilling, and for really simple stuff, I
create just one dim layer.
Back to holes as reference, my primary interest in the idea comes from
using internal holes for clamping. For my upcoming stacked plates, I
can simply add holes and not worry much about their location; they need
to be reasonably close transversely (to align with the slots) and not
hit any "working" holes - there is plenty of room. However, not all
parts can be punctured at will. Perhaps the answer is to still
reference the edges, but not bother milling all the way around at first,
so there would be little if any reason to move clamps. With a clean
left and back edge, the references are set; then one could position
internal holes with precision. If there happens to be a t-slot under a
few of the holes (courtesy of a favorable transverse location on the
table), they could then be used for clamping, after which the external
clamps could be removed.
Does that make sense? Please comment freely.
Only work from one side of the screw. Let's say you have zeroed the dial
turning the crank clockwise. If you need to work backwards from that point
turn counter clockwise to beyond where your desired point is and then come
back turning the crank clockwise. This doesn't account for wear in the
screw itself, but usually the wear is in the brass half nuts so this is
usually not an issue.
If you are milling a pocket, you of course can't over shoot without taking
the cutter out of the work.
Taking the time to square your stops with an indicator and making sure
everything is good and snug is good practice that leads to precision
Another thing that helps avoid the brain fart errors is to layout the part
with scribe lines and that way you can see if you have not counted your
crank turns real easy.
About the time I had mastered getting the toothpaste back in the tube, then
Take a piece of angle iron. Drill two hole in it to receive short
carriage bolts. Nut on each side of one leg of the angle iron. Tighten
the bolts up evenly. Place your raw part on table, bring bolt heads up
to touch edge of plate. clamp othe leg of angle iron down without
moving. Every new piece you put in there will only touch those two
points of the rounded bolt heads.
That's correct. Years ago, when I was in training, we had pretty much
full shop capabilities, at least within reason. While I never ended up
with a set, the journeymen made small sets of locating jaws, more or less
short parallels, but stepped. They were heat treated and ground. They
could be used for two different T slot sizes, and stood above the table a
small amount, maybe 3/4".
Yep! I agree. They do get in the way, depeding on the job at hand. You
might find you can use parallels installed the short way. You can use only
a short portion of each one, with the balance beyond each end of the parts.
Reason? If you have a minor deviation in either of them, it can't be much,
due to the slot size. By spacing them, neither of them can steer the
part----and you'll have minimized the inherent error, should you have any.
As I said before, because T nuts tend to swage the T slot tight, if you
make them nominal slot size, they are a light tap fit with a soft hammer.
Not deadly accurate, but when you use a pair of them, you can expect
alignment within a thou----which is pretty decent if you space them as far
apart as is possible. Typical shop tolerance is .001"/inch, so you'd be
well within tolerance on all but the most demanding of jobs. When it must
be closer, you, of course, resort to a DTI.
Make your plate of aluminum, and thick enough, so it becomes a great work
platform for multiple jobs. If it's thick enough, you can drill into it for
through holes as an added benefit.
I tend to work off parallels all the time, to avoid every touching the
table. My mill was purchased new in '77 and has no pecker tracks on the
Regards the third stop, the side one----it does no harm to not have it on
the base plate-----that way you won't be limited to the size the plate can
accommodate. You may find yourself working with a long plate with a hole
pattern in the center. You can set a stop real easy by using a hold down
bolt and a few thick washers, and place it accordingly. All you really
need is an elevated platform that is straight cut, but if you do lots of
small stuff the L shape could prove pretty useful----with a stop on the left
Regards milling the L shape----no real need. Use a thick plate, then drill
and ream for dowel pins. Do all this after milling an edge, so you have a
reference point for setup. Dial in the machined edge and your dowels are
parallel to table travel. Dowel pins are heat treated and ground, and
cheap! Again, you can even use one for the side stop. They present
almost no surface area for chips to prevent proper banking.
For starters, the only way you can reliably work with the screw in both
directions is to measure. Even when you know the amount of backlash you
have, there's no guarantee it's uniform. Backlash occurs because of wear,
which we all know. Thing is, the wear doesn't occur strictly on the nut.
As a machine ages, the screw will develop wear, too, so the amount of lash
you have will be different, depending on location. Probably not a serious
problem, but it can be if you have a narrow tolerance. I make simple
pencil sketch on a piece of paper and trust the dials in the two directions
that are proper, then cut and measure when I reverse the screw----marking
the dial, or recording the reading for finish size on all edges. The
sketch I mentioned consists of a cross, with the appropriate dial reading at
the end of each of the arms. I do all my finish cuts by climb milling, and
backing off the corners about the amount of the backlash as I enter them.
You can cut windows without a trace of undercut that way. The little
sketch will keep you out of trouble when you have more than one part to do.
I use a finger or thumb nail, but if in doubt, I'll often use anything
rigid. A small parallel, or even another scale. You'll be pleasantly
surprised to find you can see as little as .003" error, although not
I didn't have the luxury of generating my own drawings, I sub-contracted
from outside sources. That didn't prevent me from re-dimensioning prints
with a pencil, however. I did that routinely. Unless the draftsman has
worked on the machines, and works the same you do, he's not likely to
present information in a useful way. I've rarely found prints dimensioned
such that you can build parts without penciling in dimensions that are
functional for the guy twisting the handles. . Often I'll re-dimension from
a different edge, but I work such that it changes nothing, it just allows me
to read my dials in the same direction all the time. I avoid reading them
backwards if possible. It's all in the work habits you form.
By the way, from what I'm reading, you have really taken to this stuff. You
don't really need much help---your thinking is quite good.
Heh! Where I came from, anything that wasn't on the print equated to making
scrap. You learned to make setups that didn't harm parts in any way,
including clamping marks. The idea of drilling holes for manufacturing
purposes wasn't a consideration, but if you can do that and not create
problems, go for it.
Perhaps the answer is to still
My procedure rarely provided for partial milling, then drilling and final
milling---but that doesn't mean it isn't a good idea. One part I made had
such a tight tolerance that I actually did work from a hole, using a pin.
All dimensions were generated from the hole as the part progressed. 26
operations in all-------and when the job was finished, all 209 of them fit
in the palm of one hand.
Circumstances can dictate what works best-----and often do. Regards
plates, my personal method was to always take them to final size----again,
if for no other reason, I may need the opposite edge as a datum point. I
not only took parts to size, but I held them close-----a target of /- .001"
always. I still have one that I made for Univac, years ago. It's a chassis
made from 1/4" thick aluminum with holes drilled and tapped in various
locations, plus counterbores for transistors. I mention this part because
it's a classic example of having to turn parts over and pick up existing
work for a second operation, which justified holding lengths and widths
close. Tough job, all done without the use of a DRO. If you're curios
about these parts (the tiny one, quantity of 209, or the chassis), I can
send a pic by email if you're interested.
If you work as I did, you'll get more than a few arguments from young
machinists that are production oriented, at the expense of quality and
personal satisfaction, but the most successful machinists I used to know all
worked that way----and acquired the respect and acknowledgement of their
peers. That's how it was before CNC---at least in the defense industry I
Sounds good. I think for the stacked plates, I will start with the
assumption that the sinking can be done on a drill press. They do not
need to be pretty, just enough to "hide" the machine screw heads without
being too deep as to weaken the connection.
No troubles so far.
> then cut and measure when I reverse the screw----marking
I guess my question is really how to know where to take the first cut.
I typically start a window by locating the (inset 0.010" or so) corners,
plunging about 0.020" (in truth, I stop when I think it's enough to see
it later). All four corners can be marked by moving with the dials, but
eventually I have to start moving against the dials, and I find it
helpful to have located the reverse dial reading by my feel/check
method. When cutting the window, the holes at the corners allow me to
see when I am on the last revolution, after which I look at the dial; if
I have a good guess at the backlash, I usually don't get into too much
Ideally, one would expect to find 0.010" (or whatever was left for
cleanup) all around. I usually find that the reverse directions require
different corrections. I think that is what you are saying should
happen, but let me know if I'm in error.
Do you mean something like below?
22 --+-- 75
I'll have to try it to be certain, but that looks it would be very
helpful and simpler than my drawings. I have been drawing a window and
placing the numbers around the box. I do no always use my spreadsheet,
but it adds absolute locations; they could always be written under the
dial readings on your diagram.
That's high praise from a respected source. However, my thinking is
good enough to know that I need a LOT of help :)
Any advice for avoiding marks?
> The idea of drilling holes for manufacturing
For the plates in question, a couple extra holes won't hurt anything.
BTW, said holes _are_ on the print ;) I design with my shop in mind,
and in this case, I am pushing my mill nearly to its cross travel
limits, making the internal holes an attractive idea.
That reminds me that I would like to get your thoughts on my 8-24 Cross
travel thread. I am in no hurry to buy a new machine, but I want to
have thought about it in case a used one appears [*]. I also want to
form some guidelines for what I would buy if I were to buy new. The
conscensous here seems to be that old American beats new Chinese. I
have no problem with that (I drive a 16 year old car by choice), but
wonder whether I would be happy with a heavily worn machine.
[*] If you have not done so, I highly recommend reading "Failure is not
an Option" by Gene Kranz.
Does that mean a reamed hole and indicating on the outside of a pin
inserted into it?
I can see the time=money argument agaist it, but I completely agree with
you any time something needs to be approached from different directions.
For now, I try to hold close tolerances on everything just to get the
> Tough job, all done without the use of a DRO. If you're curios
I am indeed interested. Please feel free to send the pictures.
The good news is that there is nobody around to argue with me - the bad
news is there is nobody around to help with the work. While not true
globally, I am pretty much a corporation of one with respect to machining.
Yep! Exactly. The two dial settings come directly from the dial (with the
dial, which in almost all cases, is RH rotation for me), allowing for cutter
size, naturally. The other two come from measuring from a datum point.
It can be the opposite side of the window, just as long as you know where it
is. I often take the window to size, minus five thou on each side, then use
that surface for measurements to establish final marks.
Problem with a spread sheet is it assumes some things-----this method works
perfectly because you cut to known stops, determined by measurements. All
depends on the job, and the tolerance at your disposal. Nothing wrong with
what you're doing if you find it works for you, and you're making good
parts. When the work is critical, all four sides should be measured to
establish the stop points, the dial, nor a spread sheet, should not be
trusted. I'd say for anything with less than .005" tolerance. I would
never trust a schedule for tight tolerance. It has a way of biting you on
It's a good idea to keep a small amount of 1/8" soft aluminum around--kept
clean, naturally. A small piece under the clamp works great. If a job is
really critical, paper under the aluminum shim is also useful. You can
usually handle parts without a sign if you use your head. One of the
problems with a mill is denting the parts when your clamp is low at the
heel. I make it a policy to have the heel slightly higher at all times,
then use a soft shim under the point of the clamp. Parallel clamping is
also a good method because it spreads the load over a large area, but I've
found I often damaged parts that way due to minor irregularities. Best
to use clean shims, at least in my opinion.
That's the best of all worlds. Holding work can be challenging. When
you run a lathe, I can't think of anything that serves you better than soft
I'll give you something to ponder----but I don't think I should be making
decisions for you. I don't have a problem speaking my mind, for me,
Machine tools cost a lot of money because we pay for precision. Iron in
and of itself isn't very desirable, I'm sure you'd agree. I've heard all
the arguments about buying old American iron, but, frankly, I just don't
agree. I've run enough machines to know that when the useful life is gone,
it doesn't matter how good it once was, or how great the builder's
reputation may be, or have been. What really matters is can the machine
serve your needs? My money says an old worn out American machine has
another name----and it's sure to anger some guys. SCRAP. Just because a
machine can move metal doesn't mean it's a good machine.
I won't ever forget running an old #4 K&T horizontal, which had the vertical
head accessory. I was trained at Sperry Utah Engineering Laboratories, in
the late 50's. They were under contract to build the Sergeant guided
missile, so they could acquire used government machine tools for the shop.
One of them was the K&T I speak of. I was cutting some slots in a length
of stainless angle, a corner for a cabinet, and trusting the dial (big
mistake). I had little experience on machines at this point, but I was
giving it all I had. When time came to inspect my work, nothing was as it
should have been. The screw on that mill was so badly worn that it was
gaining or losing no less than .015" in a few inches. The machine had
obviously seen a lot of action during WW II. Could a new import machine
be any worse?
I don't do a lot of reading, mostly because I don't have a lot of spare
time. I read the paper daily, and the Smithsonian magazine-----then things
that interest me. I'd like to explore your recommendation, but I'd
appreciate a clue regards the contents of the book. The title is
intriguing, at least to me. It very much describes my attitude about the
things I do on a daily basis. I ran my shop that way, and the precious
metal refining business that replaced it as well. I've always done things
the very best way I could--and don't have a lot of patience for folks that
gloss over everything.
By now, you should have received the picture I spoke of. The pin was a part
of the holding fixture---simply---a drill blank. The parts were too small
to handle by most any other method, so I made what was soft jaws for the
mill vise, then milled the jaw away as the part took shape, leaving only the
profile of the part intact. The pin was in the jaw, and located the part
for all dimensions. It was one of the first features on the part, once the
blanks were squared. I trusted my dials for dimensions once they were
properly marked in relation to the locating pin Holding the parts in a
vise was a serious challenge. Tighten it too tight and you lost
location----and crushed the parts. I ended up using a small parallel clamp
(1-1/2") as the vise handle. Worked great. Used the same two fingers to
tighten the vise each time for consistency. Sometimes you have to think
out of the box.
I highly commend you for that. If you learn to work closely, in the end it
takes almost no more time, and you save what little you may spend by not
having to screw around with the parts for succeeding operations. Pay
attention to "hackers", guys that think that you need not work closely,
except on rare occasions. These guys never master the art of close work,
so when it comes along, they can't do it worth a damn. Fine work is
different from hack stuff----and you must know how to do it if you want to
succeed. You can't do it occasionally and ever get there. It must become a
way of life. Many don't have the balls for it-------and many don't care,
even if they do. I'm not one of them.
But------you have at your disposal some good people to provide guidance, and
it's only a few clicks away. The only problem I can see is it's hard to
separate those that "can" from those that *think* they can----but it slowly
comes out if you read long enough. There's NO substitute for experience
when it comes to running machines. You can have all the knowledge in the
world in your head, but if it doesn't come out of your hands, it doesn't
matter. When you watch people that know what they're doing, they look
different. I mentioned this recently---hope I'm not repeating myself here.
It's not so much what a guy or gal does that knows the ropes----it's how
they go about doing it. That comes from experience.
Thanks for mentioning it. I will give it a try.
> The two dial settings come directly from the dial (with the
Let's see if I follow. You are saying that you take the desired
location of the cut, back off a measured cutter radius plus five thou,
and use that dial reading. That is what I do, except I leave ten thou,
and I generally don't measure the cutter, except to check new ones to
ensure they won't double cross me (if they are over sized, I clearly
want to know). If I had more faith in my ability to measure from edge
to edge, I would probably take the time. Any tricks of the trade for
> The other two come from measuring from a datum point.
Are you saying that you turn the dial backwards until the edge of the
cutter is where you want it by measurement? What do you use to make the
I have always made a cut that I have good reason to think leaves some
excess metal, and measure the part (with a dial caliper) to find
Agreed. The spreadsheet always spits out numbers that leave some metal
(ten thou by default), after which I measure and alter the readings. I
end up crossing out numbers writing new reading beside them.
Sounds good. Is there any concern about the shims helping the part to slip?
You won't be making decisions, but I do value your opinion. If I buy
something too big or too small, that's my problem, not yours, so I have
to make the decisions. There are no immediate plans to buy.
INTERESTING. My opinion on this has been swinging from the ultimate
being a used/rebuilt BP to preferring a new machine that a future
version of me inspected, trammed, etc. prior to purchase. This is based
in part on posts such as "yeah, the screws are shot, but with a DRO who
cares?" and my experience with my own mill, which is a hell of a good
machine. If I ever reach the point of going out of my way to buy a knee
mill, a six hour drive to Atlanta or other hub location would not be out
of the question.
That machine probably saw more use in a few years than I could
realistically give a machine in decades of prototyping and tinkering.
Perhaps all the more reason to buy new.
Again, I am not in a hurry. The BP, owned by a little old lady who used
it only to square a block once a year, has not appeared, and I am not at
all certain what I would buy. If I were willing to kick my car out of
my garage, I could get a 10x54 with no space worries. But, the car
deserves better. An 8x36 seems a bit small cross travel wise (not much
of a jump over what I have now), and a 9x42 is a big jump in weight.
Benchtop knees are nice enough, but the travels are typcially worse than
what I have now. So far, I'm hindered more by travel than by mill-drill
Gene Kranz is a living legend. He began as a military jet jock and then
joined NASA fairly early in the space program, becoming a flight
director. The book is littered with history of Mercury, Gemini and Apollo.
> The title is
If the insights into NASA don't interest you, the insights into Gene
Kranz will. Get a paperback copy and a bookmark; you won't regret it.
I haven't seen it. Sometimes that is my fault. Spam dominates my
incoming mail (as it does for most people), and I know I occaisionally
delete things in error. Our server will bounce some messages, such as
those with a .zip attachment (but you can rename a zip file to have .z
extension and it will come though - the system will even offer to
I apologize for any inconvenience. A good starting point would be to
send a quick test message to make sure we are using the correct
accounts, and can coordinate it further offline. I would very much like
to see the photos. Also, I just sent a message to the address that
appears to be yours; you can simply reply if you see it, and we can work
up from there.
> The pin was a part
Considering I used to have my end mills re-ground, measuring them was always
important. Further, new end mills tend to not run true to size. On many
occasions I found four flute end mills to run slightly oversized, but two
flute on size, usually within a half thou. When working to a tight
tolerance, it can spell the difference between success and failure.
It shouldn't really be much of a challenge, considering most cutting tools
have opposing faces. Not true in all cases, naturally---such as a three
flute end mill.
It requires a light touch, and I highly recommend carbide faces for the
micrometer. It is also a good practice to measure the portion that you
actually use, not well up the cutter. That may not matter with end mills
unless the end is badly worn, but drills are not straight. Particularly
when measuring number drills, where size from one to the preceding drill may
be only a thou different, measuring near the shank will provide a useless
measurement. It helps to look at the tool as you measure----I simply spin
the tool slightly as I bring the spindle against the lip--and stop turning
the spindle when I feel contact. A little fussing tells you when you're in
proper contact. You should be able to measure drills or end mills within a
couple tenths----far more precisely than you can work manually.
If you've read my posted ravings, you'll know that I am NOT a fan of
calipers. They lie to you way too much to be reliable. That's not to say
I don't use them---I do---but I try to never trust the readings----and I'm
usually well rewarded for not having done so. I use micrometers----relying
on calipers only when nothing else will work. If you have a broad
tolerance and don't care if you miss dimensions by a few thou, hey, no
problem. Frankly, I'd trust my ability to measure with a scale before I'd
trust calipers. I've consistently measured the lengths of shoulders within
.003" with a decent scale-----although I will admit that was when I was
young and had good vision. I doubt I could do it today.
Cool! A man after my own heart. A perfectionist. Based on that, your
spreadsheet is a great idea. It's always nice to have something that gets
you close, so you don't spend unwarranted time getting there. The time
spent making corrections for the actual location is what makes the
difference, and I commend you for your technique.
The available tonnage appears to be the ruling factor. As long as you use
more than one clamp, slipping has never been a problem for me-----and I am
not a ham fisted operator. Having run grinding machines for a few years,
you learn to tighten bolts adequately, without over-tightening. That's
important if you expect good performance from a grinder. Placement of the
hold down bolt as it relates to the stand-off makes a huge difference, too.
By keeping the bolt near the part, away from the stand-off, you apply the
vast majority of pressure on the part----where it's needed.
That's a good thing. Keep your eyes open----and don't discount the clones of
BP mills. Some of them are huge improvements over the BP----more robust,
with heat treated ways.
I've owned two BP mills, both purchased new. I have no problem speaking the
truth, some of which isn't complimentary. I made the choice for one
reason, maybe two. One was the incredible flexibility. They offer easy
operation---and a head that can be tilted or rotated anywhere you desire.
The turret on a BP is one of the features that endears the machine to use.
You can work off the side, with long objects, or swivel the head to continue
a cut without resetting your work. Still, they are far from a great
machine, and are highly over rated. Were it not for the price (the
other reason I bought), which at one time was very reasonable, they wouldn't
have achieved the status they enjoyed. I've operated mills that make them
look bad-----Gorton, for one. Problem is, unless you buy the BP pattern,
none of them offer much flexibility. A Gorton 9-J, for example, is ten
times the machine, but you can't move the head in any direction. Great
machine, but only for straight away milling and drilling. No trick stuff.
If the screws are worn to the point where it's a problem, why would anyone
expect the balance of the machine to be any better? Slides wear away,
too. The issues with a badly worn machine are a serious
consideration-----and can't be solved without spending huge amounts of
money--even when you do the "restoration" yourself, assuming you want to
dedicate the time. Nothing wrong with doing it----I recall with great
pleasure an old 8-D Gorton that was nothing short of an anchor----that was
fully rebuilt by one of our machine tool repairmen at Sperry. New screws
and nuts, and all surfaces re-scraped, including the knee ways and table
surface. When it was finished, it was the nicest machine in the shop.
BUT-----it took time------lots of it. Having worked as a machinist and
toolmaker, not a machine repairman, I'm not sure I want to spend my time
making a machine work----that's not what I did, nor what I desire to do.
From the sound of things, you are involved in a project of sorts----and
maybe should not be dedicating your time to making a machine perform
properly. Rebuilding a machine probably isn't a good idea---but I may be
wrong. A new Jet mill surely would serve one better than a clapped out BP.
My first BP had the 36" table. Big mistake. I needed the extra travel on
many occasions. I agree---buy the largest machine you can accommodate,
keeping within the drop spindle design. Again, it all depends on the
work you do. That old 8-D Gorton I spoke of was a wonderful machine, but
very limited due to size. I made a nice 8 cavity 9/32" lead ball mold on
it, trusting the screws. Turned out beautifully---but the machine was
limited to small stuff. Not a solution if you do large work.
Thanks. There's a used book store in the "big city". . I'll check it out
the next time we go there. We live out in the country---nothing available
Done! Let me know if you don't receive it by posting here, or another
email. See below.
Not really, though it certainly would work. In terms of my time and
given the small number of parts needed, it would be quicker to just mill
them, and I need the practice anyway. If I were making many (by
real-world standards) of them, then it would be a natural choice.
Here is a quick way. Mill a template out of Plexiglas, about 1/2 inch
thick. blank out your aluminum sheets a little larger than your finished
Attach a sheet of aluminum to the Plexiglas with some double stick masking
tape and using a flush trim router bit cut the blank to finished size. Now
before dismounting the sheet drill your holes. Now all you said was that
the run was more than 5, but let's say that it is 20. With only 20, if you
were to have your holes drilled in the Plexiglas you could use those holes
to guide a drill bit before they degraded beyond tolerance.
If you had to do more than 20 you could use the holes in the Plexiglas to
guide a transfer punch. Alternatively you could set drill guide bushings in
On countersinking, the counter sink will allow the plate to self center so
setting the depth on the drill press you can knock these out quick.
You should be able to hold +- .003 with no problem.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.