Machining questions

[euphnut65]

Machining questions

I'm trying to get a handle on tolerancing and fits (I'm really an EE, not an ME) . I've been coddled in the past because our in house machine shops would figure out the tolerancing for me. However our in house shops have recently been scaled back so far that I am going to have to submit work outside.

Looking through my Machinery's Handbook, I see fits like LC1 through LC11. On a prevoius page it shows different types of machining processes such as broaching, milling, etc. None of those types of machining show anything below a grade 4 tolerance grade. This makes me wonder if anything below a grade 4 is practical.

The handbook verbally describes running fits from RC1 to RC9. It looks like I would choose an RC4 fit for my moving parts based on the verbal description, but am wondering if that would be practical.

Also, I'm going to be using mostly hard coat anodized aluminum parts. The shops I have worked with before would tell me this adds 0.001" to 0.002".

Any insight into any of this would be greatly appreciated (and needed).

Thank you,
Eric

 

[swertel]

Can you give me a page reference in your Machinery's Handbook, and version? I'm not familiar with LC or RC abbreviations, but know a fair bit about tolerancing.

Hard anodizing is typically per MIL-A-8625, currently revision F. Hard anodize is Type III and is typically Class 1 (colorless). But if you want to die it blue, black, or blond, you specify Class 2 and the color (preferably IAW FED-STD-595). Here's the tricky part. Unless otherwise specified in your drawing, the nominal thickness of the coating shall be .002 inches (2 mils) +/- 20% of the thickness. But, the thickness can range from .0005 to .0045 if you prefer more or less coating.

You can view the MIL spec here.
http://assist.daps.dla.mil

--Scott

 

[cclark440]

When sending parts to anodize I usually spec Type III Class I and also specify a thickness of .0005"

Are parts always come back with the thickness of .0005" +.0002"/-.0001".

Like Scott said you need to specify that thickness that you require.

 

[MilesH]

Eric,

I had some parts hard anodised a few years ago. I think it's up to you to specify the film thickness that you want. The normal range is 1 to 3 thou. but I think up to 5 thou. is possible. The important thing to remember is that half the thickness of the film is created within the existing surface (so a cylinder will increase in diameter by the film thickness that you specify). Also alloy selection is important. High copper content alloys are problematic, I think.

Hope I've remembered this correctly....

I'll stay away from the tolerancing thing........

Miles

 

[Anonymous]

You need to look at the table under the RC4 heading to find the recommended tolerance. The numbers are in thousandths of and inch. Down the left side of the table there should be a dimension range. What you do is you take the dimension (ie size of hole or shaft) on the left and then go across until you get to RC4. then add or subtract that number from your dimension. Leave room for the anodizing as the others have noted otherwise the fit might be a little tighter than desired.

 

[euphnut65]

Re:

Can you give me a page reference in your Machinery's Handbook, and version? I'm not familiar with LC or RC abbreviations, but know a fair bit about tolerancing.
--Scott

I have the 26th edition pages 630-633 have the information I was referring to.

Also, why would an LC4 fit have a larger tolerance zone than an LC5 fit? (Page 633 graph)

Thanks everybody,
Eric

 

[swertel]

For those with the 25th ed, it starts on page 645 and the graph is 647.

LC4 has a larger tolerance for the hole than LC5 because 4 is for a snug fit while 5 "resets" for a slip fit. If there was another category in addition to LC, LC4 and LC5 would be the divider between line-to-line fits and slip fits.

Now the questions comes into play -- what are you trying to assemble? Is this a machine design? A rotary shaft? A dowel pin fit? A clearance hole for a bolt or SHCS?

Reading the tolerance graphs is nice, but knowing the appilcation and the cost of achieving the tolerance in the graph is more important. For example, standard drill sizes for clearance holes (giving you .015 to .032 clearnce) is probably better than specifying a class fit that forces the machinist to ream the hole.

--Scott

 

[euphnut65]

Re:

LC4 has a larger tolerance for the hole than LC5 because 4 is for a snug fit while 5 "resets" for a slip fit. If there was another category in addition to LC, LC4 and LC5 would be the divider between line-to-line fits and slip fits.

..but in the ANSI standard tolerance table, there are higher tolerance numbers for a grade 5 vs a grade 4.

Now the questions comes into play -- what are you trying to assemble? Is this a machine design? A rotary shaft? A dowel pin fit? A clearance hole for a bolt or SHCS?

I have some dowel pin holes some press fit and some location fits (slip). I also have some sliding surfaces that I think would be described as running fits.

Reading the tolerance graphs is nice, but knowing the appilcation and the cost of achieving the tolerance in the graph is more important.

That's where things get a bit fuzzy for me.

For example, standard drill sizes for clearance holes (giving you .015 to .032 clearnce) is probably better than specifying a class fit that forces the machinist to ream the hole.

I wish you(we) could specify drill sizes in the hole tool!!

Thanks,
Eric

 

[swertel]

Dowel pins, that's a whole different ball game.
If you doing tooling with lots of locating features, I prefer locating pins from Carr-Lane as opposed to dowel pins. They allow for tolerance variation in a direction.

Here's my guide to dowel pins. I'm only going to post this once. This was developed after doing some comparison between fits, cost of machining, ability to press the dowels into place, and the standard size of a dowel pin.

Loose Fit (Dia)
.0629 +.0002/-.0000
.1254 +.0002/-.0000
.1879 +.0002/-.0000
.2504 +.0003/-.0000
.3129 +.0003/-.0000
.3754 +.0004/-.0000
.5004 +.0004/-.0000
.6254 +.0004/-.0000
.7504 +.0005/-.0000

Press Fit (Dia)
.0625 +.0000/-.0002
.1250 +.0000/-.0002
.1875 +.0000/-.0002
.2500 +.0000/-.0003
.3125 +.0000/-.0003
.3750 +.0000/-.0004
.5000 +.0000/-.0004
.6250 +.0000/-.0004
.7500 +.0000/-.0005

If you have a dowel pin larger than a 3/4 Dia, you don't have a pin, you have a shaft and REALLY REALLY need to consider using something else to locate with. As it is, .500 and above is more for strength of the joint than location.

--Scott

 

[cgriffin]

Eric,
Being an engineer, then a manufacturer who has used machine shops a lot, and now owning a machine shop, I can tell you that it's easier to actually call out the actual tolerances than to call out a tolerance spec. For instance, put down on the drawing:
All dimensions +/- .005 unless otherwise specified.
As a reference, that's one of the most common tolerances, although for many fields that are not critical, +/- .010" is also common. It all depends on how close your part needs to be to the actual drawing, and still work as well as you'd like. For instance, if you are making an enclosure that is a 24" cube, then +/-.010 might even be overkill. But if you are making parts that need to fit together, and they are very small, then in that case +/- .005 might not be good enough.

I have an assembly that contains about a dozen parts. Some of the parts have a tolerance of +/-.001 and some are at +/- .005. The bottom line is--the bigger the tolerance, the cheaper the part. The looser tolerance will reduce setup time and allow the machinist to move quicker, and it will reduce his scrap. Just make sure that if you spec out +/-.010 that it will work if one part is at the large end, and the other is at the small end.

 

[jemmej]

I've never been a big fan of tolerance tables myself as I feel they remove a layer of understanding of the design and their limitations are not clearly stated (i.e. it is assumed that one end can easily be determined to be the "fixed" part for practical purposes, or that you can work with nominal sizes).

As has been mentioned. It is far more pracitcal and reliable to use the tolerance tables to design your part, but to specify a specific tolerance for your dimension on the detail drawing. Anytime that you leave the math up to someone else, eventually the math will be calculated incorrectly.

Also, do you really need to worry about tolerance grades, etc. What is it, exactly that this is applying to?

For example, I don't use tolerance tables because I am usually mating up with some purchased part's hole that has a specified tolerance. Therfore I have to calculate "backwards" from that tolerance to determine my locational tolerances at the "fixed" end.

For most everything else, we use standard tolerancing (such as +/- .015) for clearance hole locations and such since this matches with the standard tolerancing of the shops that make our parts. We use +/- .005 for more accurate locating (such as tapped holes) since this is approaching the reasonable accuracy of the machine used (turret press usually). Of course, more accuracy can be obtained but at higher cost.

Of course, the question I have (w/o any offense meant) is why are you designing this in the first place? I've not known too many businesses that could afford to have their own shop and shop personnel and NOT employ an ME or similar to do the design. Just my curiousity at work I guess.

Jim

 

[euphnut65]

Re:

Anytime that you leave the math up to someone else, eventually the math will be calculated incorrectly.

I'd prefer to leave the tolerancing up to the machinist, but If they are not checking the work I would be afraid of getting a lot of parts back that don't fit with each other or align.

Also, do you really need to worry about tolerance grades, etc. What is it, exactly that this is applying to?

The tables seem to be a good guide for fits what I would verbally categorize as press, location, or running fits using dowel pins, running parts in slides. Basically they will be used for pneumatically actuated moving fixtures to handle glass tubes and vials.

For example, I don't use tolerance tables because I am usually mating up with some purchased part's hole that has a specified tolerance. Therfore I have to calculate "backwards" from that tolerance to determine my locational tolerances at the "fixed" end.

For most everything else, we use standard tolerancing (such as +/- .015) for clearance hole locations and such since this matches with the standard tolerancing of the shops that make our parts. We use +/- .005 for more accurate locating (such as tapped holes) since this is approaching the reasonable accuracy of the machine used (turret press usually). Of course, more accuracy can be obtained but at higher cost.

It seems as though tolerancing has been discussed so far, but maybe what's more important is picking the deviation from the basic size for what type of fit is what's not so clear or straightforward.. like the dowel pin holes sizing Scott (Gaspar) posted. I'm sure it took years of trial and error to develop the tables in the Machinery's Handbook.

Of course, the question I have (w/o any offense meant) is why are you designing this in the first place? I've not known too many businesses that could afford to have their own shop and shop personnel and NOT employ an ME or similar to do the design. Just my curiousity at work I guess.

Jim

I work at a large heath care products company in an NMR lab with equipment that I am trained to repair. However, sort of like the Maytag repairman that does not take up too much of my time, so our group comes up with automation challenges and I try to come up with solutions. I've already put two extensive systems together using robots and custom designed stations. I do all the work from the original design, drawings, assembly of the parts, as well as the programming and wiring of the controllers and associated circuitry. It may not be the most efficient model, since there are learning curves from CAD to mechanical design to controller programming, but it has worked out alright. After all- I am the one stuck fixing them if there are problems!! Admittedly it would be more time efficient for me to give the work over to more specialized people, but I think I understand the processes better than anyone I might outsource the work to. Besides it doesn't hurt to learn new skills.

I'm wondering if it would be too much to ask for Alibre to someday have automatic tolerancing capabilities based on fit types. Does Solidworks or other more expensive MCAD programs have this capability?

Thanks,Eric

 

[jemmej]

Ah...pneumatically arms and such....excellent. Well, unfortunately (or I suppose fortunatley ) I just got a large project at work to do, so I'll be light on the posting in the near future. G/l with your design work!

Jim

 

[euphnut65]

Re:

Here's my guide to dowel pins. I'm only going to post this once. This was developed after doing some comparison between fits, cost of machining, ability to press the dowels into place, and the standard size of a dowel pin.

Loose Fit (Dia)
.0629 +.0002/-.0000
.1254 +.0002/-.0000
.1879 +.0002/-.0000
.2504 +.0003/-.0000
.3129 +.0003/-.0000
...........
--Scott

Scott,

I'm confused about the numbers you use for your sizing +.0002 and -.0000 for a 0.1254" hole (for example), this is better than a grade 6 hole (I think it would be a grade 5). I'm looking at the LC1 fits in table 5 (p636) or Table 1 (p630) of my handbook (26th edition). According to table 22 (p630), a tolerance grade 6 hole is not achievable by drilling or even boring. I see reaming will just get into a grade 6.

Am I missing something?

Thanks again,
Eric