PDA

View Full Version : Symmetrical parts from a mill



RKW
12-16-2009, 11:44 PM
What is the accepted practice when creating symmetrical parts in a mill? Say, something like a t-nut.

Is it best to:

1. Locate one edge, offset, machine, then repeat with the other side/edge.
2. Use a work stop, locate edge, machine, and rotate the part against the work stop and machine.

I have done it both ways with acceptable results, just curious what the pros might do.

Keith

wierdscience
12-17-2009, 12:06 AM
On a tee nut type part I find the face of the fixed vise jaw,offset to the opposite side of the workpiece and climb mill that feature,then flip the part and climb mill the other feature.

David Powell
12-17-2009, 12:09 AM
My designer, in the last job I had, introduced me to a way of working which I had not previously considered. Since beginning to use it I have seldom worked any other way. The scheme is best done on machines with digital readouts. The first thing done is to find the centre of the blanked out squared up piece you will be machining and then zero out the readouts at that position. Assuming you can use your edgefinder reasonably well then that position will be within about 2 thous or less of the true centre. Next a quick look at the drawing will show if you can easily work from that position, or whether you had better work from a " false centre position" which relates to matching the part to some other part. If the part is symmetrical, like a Tee nut, you can begin by drilling and tapping the hole on the centre point, then you can work out the offsets on the cutter to give the size needed, for example if the part to fit in the narrow bit of the tee slot is to be5/8 wide and 1" long and you use a 1/2" cutter you can confidently machine down to . 562 for each side and .750 for the length. Using this method, works well for me, it is tolerant of slight mistakes and It does not suffer fromtolerance stack up problems which sometimes occur when working from one corner. Hope this is of interest David Powell.

darryl
12-17-2009, 03:33 AM
I like to use a jig whenever I can. Often times it's so quick and easy to make that I just do it. Mdf and pvc are my workhorse materials. Cut an L shape, clamp it to the mill table, then adjust positions for the workpiece. One after the other, tuck the piece into the L, clamp, drill or mill, etc.

Many times the jig consists of a piece of mdf pilot drilled for some screws, then aligned on the mill table with a workpiece tucked into the corner formed by the screws. The mdf is consumable, so you can drill or mill into it without fear of marking up your mill table.

Another way to quickly align several pieces one by one for machining that I use is a home made mountable square. I took a piece of channel, cleaned up three sides, then drilled five holes in a pattern at one end. A piece of angle cleaned up on two sides and squared is drilled with one hole on one face, and two holes to match the groove on the side of the mill table on the other face. With one bolt holding the two pieces together, it is set on the mill table and the angle part secured with hardware to the side of the mill table. From there, the channel piece is carefully aligned to be square across the table and secured using two bolts and t-slot nuts. Then the rest of the holes are drilled through, all of them getting spring pins pressed in before the jig is removed from the table. Now I can mount that anytime, knowing it's square, then clamp a block to it at an appropriate point and I have my corner to locate a workpiece into. When there's several to drill or mill, it makes shorter work of aligning each piece.

BobWarfield
12-17-2009, 11:31 AM
Workstops of all kinds seem like they save a lot of time. I got to the point where if I didn't start with a work stop, I often slap one on the vise before removing the part just in case I want to put it back.

BTW, a small Kant-Twist is a useful stop for many circumstances.

Cheers,

BW

Carld
12-17-2009, 03:47 PM
A T nut or several of them? For several a bar the width for the base and a little longer than the vise jaws. Mount in vise on parallels so you can mill the sides and locate center. Working from center cut each side the required depth Z and Y on both sides. Drill and tap bolt holes. Saw them the length you want and deburr them.

RKW
12-17-2009, 04:10 PM
Carl,

The t-nut was only a hypothetical, so it wasn't really a question of how to make anything specifically so much as it was keeping anything (t-nut or not) symmetrical and the preferred method.

But I do agree with your method in this case ...

Keith


A T nut or several of them? For several a bar the width for the base and a little longer than the vise jaws. Mount in vise on parallels so you can mill the sides and locate center. Working from center cut each side the required depth Z and Y on both sides. Drill and tap bolt holes. Saw them the length you want and deburr them.

dp
12-17-2009, 04:53 PM
I make t-nuts with a shaper and a hacksaw.

beanbag
12-17-2009, 05:17 PM
(do stuff as usual)
g52 x[...] y[...] (center of symmetry x2)
g51 x-1 y-1
(repeat: do stuff as usual)

Rich Carlstedt
12-17-2009, 06:58 PM
What is the accepted practice when creating symmetrical parts in a mill? Say, something like a t-nut.
I' ve done it both ways with acceptable results, just curious what the pros might do.

Keith

You ask a good question !

There is no correct answer.
The first question a pro asks, is "what are the tolerances ?"
The second is "how many"
The third is "what material will I be using"
The fourth is 'What machines do I have available"

This is not a smart aleck response, but shows the diversity of the answer.
Each Machinist has a certain skill level that he feels comfortable with, and that is the one where he makes the fewest mistakes.
The real question I think you are asking is :
"What method will produce the best results for me ?"

The fact that you ask that important question, tells me and others here, that you want to improve your skills.....hooray, that is great !
Keep all of this in mind, both when you read the answers of others , and try the various approaches yourself.
I confound some friends when I cut parts with a bandsaw, instead of milling,
or drill in the mill, instead of the drill press.
I look at the ultimate use/need and then ask the above questions.

Jigs/Fixtures are a waste of time for one off jobs, UNLESS, the tolerence required makes some dimensions critical, then it can become imperative to make one.
Digitals on any machine tool can and will double the output along with improved tolerence control and elimination of backlash error calculations.
W/O digitals, the job becomes more difficult

Now to answer your question
If "symmetry" is the critical designation ( and its a good one), I would drill the tapped hole first to dowel pin size, and use the dowel as a depth stop on the vise jaws to do both sides, OR,
I would mount a scrap piece in the jaws and drill a dowel hole which establishes my center lines, and then clamp the predrilled part on the dowel
and machine both sides at the same setting
Neither of these methods match the others, but is equally of value
Note, in the first method, I used the part as a fixture, and in the second method, we made a fixture to reach an objective.

The first is easier, but requires more clamp/unclamp time ( and ERROR entry)
The second requires more time, but gives an operation that not only will provide symmetry, but allow machining steps without resetting the part, and the ability to measure the part while still machining.
Think about this if the part were made from Gold....and no errors were allowed.
You would want to be able to sneek up on every dimension .

Good question Keith..and good luck.
Hope this helps you when you see the myriad of answers
Rich

RKW
12-17-2009, 08:43 PM
Again, not really making t-nuts here, just asking about symmetry ...


I make t-nuts with a shaper and a hacksaw.

RKW
12-17-2009, 08:44 PM
Thanks, but I never said anything about CNC ...


(do stuff as usual)
g52 x[...] y[...] (center of symmetry x2)
g51 x-1 y-1
(repeat: do stuff as usual)

RKW
12-17-2009, 09:05 PM
Ah, finally a detailed answer to the actual question! I'm certainly greatfull to have this community to bounce things off of and really just love to read this forum like a newspaper (since I really don't care about the real "news"). But geesh, sometimes folks need to read to OP a little more carefully. In this case I was looking for an answer to a question not a solution to a problem ... there is a difference!

Rich,

You are right, I'm always looking to improve my skills not just turn the cranks and produce any old junk (we have China for that ;-) The fact that you answered my question with several others just gives me more room for thought. I have not had to use any fixtures to date as the non-moveable vise jaw and work stops have worked quite well. But it probably only a matter of time before I do. Tooling plates have also piqued my interest. I do like your suggestion of dowel pins for items with holes.

Thanks,
Keith


You ask a good question !

There is no correct answer.
The first question a pro asks, is "what are the tolerances ?"
The second is "how many"
The third is "what material will I be using"
The fourth is 'What machines do I have available"

This is not a smart aleck response, but shows the diversity of the answer.
Each Machinist has a certain skill level that he feels comfortable with, and that is the one where he makes the fewest mistakes.
The real question I think you are asking is :
"What method will produce the best results for me ?"

The fact that you ask that important question, tells me and others here, that you want to improve your skills.....hooray, that is great !
Keep all of this in mind, both when you read the answers of others , and try the various approaches yourself.
I confound some friends when I cut parts with a bandsaw, instead of milling,
or drill in the mill, instead of the drill press.
I look at the ultimate use/need and then ask the above questions.

Jigs/Fixtures are a waste of time for one off jobs, UNLESS, the tolerence required makes some dimensions critical, then it can become imperative to make one.
Digitals on any machine tool can and will double the output along with improved tolerence control and elimination of backlash error calculations.
W/O digitals, the job becomes more difficult

Now to answer your question
If "symmetry" is the critical designation ( and its a good one), I would drill the tapped hole first to dowel pin size, and use the dowel as a depth stop on the vise jaws to do both sides, OR,
I would mount a scrap piece in the jaws and drill a dowel hole which establishes my center lines, and then clamp the predrilled part on the dowel
and machine both sides at the same setting
Neither of these methods match the others, but is equally of value
Note, in the first method, I used the part as a fixture, and in the second method, we made a fixture to reach an objective.

The first is easier, but requires more clamp/unclamp time ( and ERROR entry)
The second requires more time, but gives an operation that not only will provide symmetry, but allow machining steps without resetting the part, and the ability to measure the part while still machining.
Think about this if the part were made from Gold....and no errors were allowed.
You would want to be able to sneek up on every dimension .

Good question Keith..and good luck.
Hope this helps you when you see the myriad of answers
Rich

RKW
12-17-2009, 09:12 PM
Short and sweet ... That's the solution I like too.


On a tee nut type part I find the face of the fixed vise jaw,offset to the opposite side of the workpiece and climb mill that feature,then flip the part and climb mill the other feature.

Blueskys
12-17-2009, 09:43 PM
I like David Powell's idea about working from the center.
That's really the definition of symetry isn't it.
I know I do some parts that way sometimes because symetry
to the center facet is critical. But I never thought it
through to be a generalized system.

CCWKen
12-17-2009, 10:37 PM
You guys have way too much time on your hands if you're cuttin' T-nuts to a thousandths of an inch. :rolleyes: I've been known to cut 'em out with a hacksaw or drill and tap a flat bar. Cripes, nobody sees them! :D

Carld
12-18-2009, 08:55 AM
RKW, you did ask, "I have done it both ways with acceptable results, just curious what the pros might do." and that is what some of us did. I didn't think we were being tested, I understood you just wanted the various ways to do it.

Like Ken, I have cut them out on a band saw and drilled and tapped on a drill press but most the time I machine them with a tolerance of +/-.010". As Ken said, it's just a T nut for Gods sake.

For what it's worth, anytime I am taking equal metal off a part in the mill I almost always use the center line as "0" or home. It simplifies off sets to cut each side. It's the same offset on each side of 0, DUH :rolleyes:

Only a person killing time would work from one side on equal cuts on each side. The first part of doing machine work is to THINK and determine the fastest, best way to do a job unless your not interested in getting the job done fast and just want to spend some quality time bonding with your machines.

derekm
12-18-2009, 03:41 PM
What is the accepted practice when creating symmetrical parts in a mill? Say, something like a t-nut.

Is it best to:

1. Locate one edge, offset, machine, then repeat with the other side/edge.
2. Use a work stop, locate edge, machine, and rotate the part against the work stop and machine.

I have done it both ways with acceptable results, just curious what the pros might do.

Keith
Depends on the type of symmetry
mirror symmetry
rotational symmetery
- then we get in to the position of the symmetry axis.

beanbag
12-18-2009, 04:01 PM
Thanks, but I never said anything about CNC ...

Those instructions are what you would do manually as well, turning the cranks.

RKW
12-19-2009, 06:38 PM
IF you have prior knowledge of CNC ...


Those instructions are what you would do manually as well, turning the cranks.

doctor demo
12-19-2009, 08:50 PM
I make t-nuts with a shaper and a hacksaw.
I'll bet drilling and threading with those two items is a real pain.:D


steve

beanbag
12-20-2009, 06:55 AM
IF you have prior knowledge of CNC ...

If you had translated the codes, you'd see it was the same thing that David Powell said.

Doing it this way, you don't keep mounting and unmounting your piece. I realized after a while that this is the best way to make sure something is the right size when you cut at both sides of it.

David Powell
12-20-2009, 09:06 AM
Some of the fellows round here( Toronto Canada) who make model steam and gas engines begin by machining the bottom of the base, drilling the mounting holes and then firmly bolting the casting to an already squared up piece of aluminium plate.( say 1/2" thick) This makes life much easier in ensuring that the crank bearings really are square to the cylinder mountings and other items , you have the whole length or width of the plate to square up on instead of trying to square up relatively small features. If you square up a 6" length to a thou then a feature 1" long will be square to less than I can measure and worry about. Hope this isnt too far off topic. Regards David Powell.