Flipping the stock

[mrscheider]

Hi all,
Folks, I'm not getting it!
What's the secret to properly getting your stock lined up after you've flipped it on the Y axis?
I've ruined literally DOZENS of projects trying to get the same parts completed. Basically, it's a two inch long stock, 1X1 on H&W.
My zero position is highest Z point, center and my part is centered within the stock itself. I cut the top, looks good. I flip the stock, take the same measurements as before, and find center. Zero and run the job. The two halves almost consistently are a 32nd of an inch misaligned. I have used a number of methods to find center.. the latest being the use of a digital caliper. I'm confused about this because it's a two inch stock. If you take an inch, there's only 1 inch left... and even a half ass measuring job with a 32nds ruler should get me closer than I am getting now, while painstakingly trying to make it exact!! The tool shank is 3/16ths. So I am allowing 3/32nds on either side of center of the X axis (length) to compensate for the tool. Then using the caliper, I confirm there is 29/32nds of an inch of stock from the edge of the shank, to the edge of the stock. Now, that to me is center. I do the same thing on the Y axis but the usual misalignment happens only the X. Even though I flip the stock, if I use the same procedure to find the stocks center, shouldn't I be aligned when the two halves meet? At the least, ;less than a 32nd of an inch? The machine is doing exactly what I am asking it to do... So therefore, I am causing this error. Can anyone please tell me? What I am overlooking?
Thanks!

Michael

[Geof]

You say 2 inch stock but how precise is this? 2 inches plus or minus what? What could be happening is that in your two center finding operations you are inadvertently doubling the inaccuracy in the stock length.

Take the case where the stock is actually 2.015":

You find center from the left hand end by measuring 1.000 plus or minus a few thou then do your machining. The part you have partially machined into the stock is not exactly on the center of the stock; it is displaced about 0.0075" toward the left. To get it on center you would have to measure 1.0075".

Now you flip the partially machined stock so what was your left end becomes the right end and you re-find center as before. And this is often where the inadvertent error comes in....you find the center again from the left end and move across 1.000 plus or minus a few thou then do your second machining.

This second machining is also displaced 0.0075" toward the left from stock center, BUT your first machining, because the stock is flipped is now displaced to the right so the two machined parts are displaced 0.015" relative to each other.

NOTE I am being a bit sloppy writing numbers like 0.0075" because you can never measure to that precision with calipers; this is just for example.

To avoid these kind of errors sometimes it is handy to machine a reference flat on the end of the stock; or totally face off one end and always use the faced end for the reference.

[mrscheider]

Geof,
I totally get that and agree with you... I cut the stock on a miter and it appears very square on both ends. This inconsistency became more clear when I was zeroing the stock at High Z, front, left. I started to turn my attention to how I was centering based on the squareness of the stock edges. I then I decided to zero at the center of the stock. Centering by measuring from the tool to the end of the stock proved to be more accurate. The cut stock ends appear very square and using a ruler with 1/32 increments, each opposite corner is exactly on the 2 inch mark.
Of course, I am not trying to even out that .0075, I wouldn't think that's reasonable to ask... but certainly even off by 20 times amount that would still be less than 1/64th. No. In my case, I would have to have a stock 2.03125 which is much more evident and possible to compensate for. I could even deal with 1/64. No problem. But a 32nd is obvious and not going to work.
Starting with an accurate stock was my first step in trying to resolve this and I feel confident that the tolerance of the stock exceeds acceptable squareness to get an accurate part.
Thank you for your reply!

M.

[Geof]

There is an alternate way to find center without using rulers or calipers which sometimes give you a parallax error.

Grip a piece of round stock in a collet in the spindle as a probe and jog the machine to carefully bring this up to the end of the stock; use a piece of ordinary printer paper as a little feeler gauge moving it back and forth and you will feel it get pinched. Paper is remarkably constant at about 0.003" thick. To get from the point of contact to center you now move half the probe diameter plus half your stock.

[MrWild]

Another way is to machine the stock to a specific blank size. If the stock starts at exactly 2.000 inches, then you know where each edge is. Machining your stock to a specific blank size will also square it up. Sometimes the face can be at an angle when saw cut, anfd what is zero at the start can be off a lot when flipped.

You can also use a hole drilled and reamed through the stock as a 0 datum point. When flipped, you know the 0 point will be the same. You need more precise instruments than a vernier when machinging a flipped part. Time for indicators. and wiggle edge finders, but mostof all, time for squared up a precise stock sizes to start with.

I'm assuming your head is trammed square with the table. If your head is not trammed, all bets are off with just about all tooling as 0 will wander all over as you raise and lower your table.

[neilw20]

Method 1: Where excess material available at ends or dowel holes don't matter.
1). Given that the job is clamped down on a flat piece of (CLEAN, FLAT) scrap unless you really want to drill holes in the bed/table drill 2 holes through into the scrap, one at each end of job that you can fit spring roll pins in step 3. I use 7/64" tubular spring pins and drill 2.7mm holes.
Use extra clamps on the scrap so it doesn't move when you flip the job.

2). Do all the machining and drilling for side 1.

3). Remove job, turn over and insert roll pins.

4). Clamp down side 2 with the pins going into the holes in the scrap. Make sure it is clean underneath otherwise the job will be tilted and alignment errors will become evident just when you have finished the job.

Note: ANY alignment errors along the flip axis are doubled, so do it carefully, at least twice as good as your smallest tolerance.
-------------------------------------------------

Method 2:
1). Clamp down job: Set machine X and Y zeros to a known square corner of job using an edge finder and setup along the length, at least twice as good as the tolerance required.

2). Do all the machining and drilling for side 1.

3). Remove job, turn over and Set machine X and Y zeros to the same known square corner of job using an edge finder and clock along the length, at least twice as good as the tolerance required.

-----------------------------------------
Method 3:
1). Clamp down job: Using an edge finder, setup along the length, at least twice as good as the tolerance required.

2). Drill 2 holes, one at each end, say 1/8" diiameter through the job over a tee slot (to save the table from damage) at locations, say X0,Y0 and X100,Y0.

3). Do all the machining and drilling for side 1.

4). Remove job, turn over and move machine to X0,Y0. Put a 1/8" dowel pin in the chuck, making sure it is running true in the chuck.

5). Lower the pin into hole X0,Y0 and gently clamp that end of the job.

6). Move machine to X100,Y0 and lower the pin into the second hole, gently aligning the job.

7). Repeat steps 5 and 6 until alignment is at least twice as good as the tolerance required.

--- Didn't even need a ruler, so eyeball limitations go away. ----
I use method three on various jigs so that they can be easily reused at a given location without have to rezero everything, or just put the jig anywhere and zero the X and Y axis on the first hole.

[mrscheider]

Oooh... Machining the stock square IS an excellent idea! I tried edge finding with the tool, but not with paper. Another excellent idea. I actually have not trammed the headstock. And never considered that to be a problem. I did use a very accurate solid 12" aluminum triangle square but I didn't tram the spindle to the table. Would that be nessesary? Maybe the head is out but wouldn't I see that on a 12 inch square? Like I said, a 32 of an inch is obvious on benchtop mills. (a taig 3000, btw)
EZ-Tram sells a nice one specifically designed for the taig. Screws right onto the spindle. $60 though. Is it that much more accurate than the square tool?
Thanks for the excellent suggestions all!

M.

[mrscheider]

neilw20,
I think any one of these methods will get me better results than I am getting now! All very excellent. I am going to try number 3 tonight as this sounds like the most reliable.
Wonderful suggestions! Thanks a bunch!

M

[One of Many]

Generally, if you need to flip a part or for that matter make any subsequent setups for other operations. Tooling the part should be done off the previously machined surfaces known to be true to the original geometry. If the second operation is zero'd out on a known location, then it will remain relative to the opposite side. The outside excess material is no longer reliable to use as a locator.

Yes, indicator traming the head will make a difference. Not only in flipping the part right to left or front to back, but from a short cutter to a long drill will not be the same position at the part surface. Using the quill can compound that even further.

Having a good setup on the machine alignment is first and foremost in order to trust it to cut where you expect it to. Eliminating nesting error in the part is the next factor to minimise. Pushing the button will still produce an accurate path in the wrong location. It could care less if the integrity listed above in the setup has or has not been accomplished by the operator.

DC

[mrscheider]

Hi DC....
I am smiling and nodding politely.. which is what I usually do when completely confused. Explain "Tooling the part"? I'm new and don't know all the slang expressions yet. Does this refer to using an edge finder?
At least for the first (top) side of the part, there is no previously machined surfaces. I'm going off the edge of the raw stock. Then you mention, the outside excess is no longer reliable as a locator. I didn't understand this either. If you mean the outside excess which is part of the second operation, that IS what I've been using as a locator however, it should still be valid as this is the dimensions of the original stock. 2 inches.
Imagine a 2 inch long, 1 inch high stock. I cut down 0.51 inches on the first cut. Now I have my "north" part sicking out of a 2 inch long 0.49 high block of stock.
When I flip the part, that stock edge is what I use to recenter the zero point.
The rest of your reply, I go along with. So I will get that tram tool and make the table and headstock adjustments.. BUT... I still don't think these particular things are giving me this much of an alignment error.
Thats still human induced.
I just need a little more experiece. I will try some of the other suggestions as well as all seem sensible and better than my "scotch tape" idea.
joking
Thanks!

M

[One of Many]

Originally Posted by mrscheider Hi DC.... I am smiling and nodding politely.. which is what I usually do when completely confused. Explain "Tooling the part"? I'm new and don't know all the slang expressions yet. Does this refer to using an edge finder?

Sorry for being so vague in my response.

Fundamentally, My terms of "tooling the part" applies to work holding, encompasing fixturing or nesting. Which includes referencing, orientation or indexing and re-orientation of the stock for the next operation. The key is to minimise nesting errors. It is nearly impossible to eliminiate them.

Originally Posted by mrscheider At least for the first (top) side of the part, there is no previously machined surfaces. I'm going off the edge of the raw stock. Then you mention, the outside excess is no longer reliable as a locator. I didn't understand this either. If you mean the outside excess which is part of the second operation, that IS what I've been using as a locator however, it should still be valid as this is the dimensions of the original stock. 2 inches. Imagine a 2 inch long, 1 inch high stock. I cut down 0.51 inches on the first cut. Now I have my "north" part sicking out of a 2 inch long 0.49 high block of stock. When I flip the part, that stock edge is what I use to recenter the zero point. The rest of your reply, I go along with. So I will get that tram tool and make the table and headstock adjustments.. BUT... I still don't think these particular things are giving me this much of an alignment error. Thats still human induced. I just need a little more experiece. I will try some of the other suggestions as well as all seem sensible and better than my "scotch tape" idea. joking Thanks! M

So your first side profile is cut .51 deep.

For the first side, referencing (part dependant) is of less importance as long as the part ends up within the boundaries of the stock. Everything else can be considered excess to be removed or left unmachined as the part requires in relation to the original indexing surfaces and X0,Y0, Z0.

As good repeatable milling practice goes, the second side should utilize the most reliable references available in at least 3 machined planes when possible. Be that the previous top plane(now the bottom) and 2 machined edges, or the bottom and one edge and a hole, or the bottom and 2 holes. Or create a nest, which is to say, a pocket with the same outer part profile geometery cut into vise soft jaws or jig plate that captures the part for solid orientation in all three planes. It makes no sense to use the rough edge at this point when you have better options there.

This practice is common since a sawn edge is rarely square in 2 planes.

Sure, you can mill the ends square to 2 other surface and/or to exact length, but why do it if they will be removed or recut later? Just because you can use a rough edge in one operation to begin the part, the chances are poor the exact same stop point and edge point will be referenced in another setup, let alone part to part. Put another way; Using the existing geometry machined into the part in the first operation to relocate it, will ensure a much closer match than using a rough cut edge that has greater chances of inducing a mismatch. The amount of offset can change if you are flipping the part front to back or right to left. You are correct, if you keep your reference with the same end, it shouldn't be .03 out IF and that is a BIG IF the reference end is square.

If this were introduced by tram. One degree is roughly equal to .0175/inch. If by chance your mill head was out of tram, that one degree will change X,Y reference point along the Z and business end of an edge finder verses actual point of a cutter if they are not the same length. Setting X0 to the left side in one operation and the right side in another although the same end could multiply an error. There can also be some parallax error in reading a fraction scale along with rough cut ends not square. It sure is sounding accumulated. I'd need to get a better visual perspective of the part, your methods and machine integrity to get a feel for what all may contribute to it.

The good news is....it may not be all you. Being one with the machine, is a mutual "taming of the shrewd"

[mrscheider]

DC,
Boy, that was great! Thank you for taking the time to help me get that. You make very good points. Actually, I tried a pretty neat thing last night that was suggested here...
I did it a little bit different... I added 1/4" on each end of the stock. Measured the center of the top, As you mentioned, on the top half, it's not important as long as the part is still in the stock limits. I then told the machine to goto x -1.1300 and y -0.0300 drilled a 1/8th" hole, and did the same on the poisitive side of the axis. Then machined the parts. I was pretty excited about this! I knew all I needed to do was flip the stock, put the drill bit into that hole and tell the x and y to be those coordinates and I could jusy X0 Y0 and I would be on the same center as I was on the first side.
Then, the x motor stalled on me and drilled a gorge right through the parts! SOB! I hate when that happens! lol
Anyway, I'm going to try that method again tonight as I think that has real potential for success.
Thoughts?

M.