CNC positional tolerances 3

[Tunalover]

Folks-
I've been searching high and low for "typical" high-probability positional tolerances for CNC punched and machined clearance holes, machined threaded holes, and machined countersinks in 6061-T6 aluminum sheet and plate. If "Rolls Royces" are on the high dollar end of the scale and if "Ford Escorts" are on the other end of the scale, what can one expect from either? My question supposes that the machines are maintained per the manufacturers' recommended maintenance schedules.

I know this is a broad question. I use the fixed and floating fastener formulas (from ASME Y14.5M-1994) for designing hole patterns but I recently caught flack for designing holes and countersinks that are too big! Our fabricator says the best he can do without raising prices is +/-.005" in-pattern (or pattern-locating). I think that his CNC equipment is doing MUCH better than that. I also think that he simply doesn't KNOW what his equipment is providing him.

Does anyone have figures for positional tolerances of clearance holes, threaded holes, and countersinks deliverable by CNC equipment? Is there any industry standard that CNC machine manufacturers aspire to? I'm aware of ISO 230-97 which only gives the methodology of gaging the machine performance. Maybe much tighter in-pattern tolerances are possible than pattern-locating tolerances?

If anyone can give hard figures I'd be MUCH OBLIGED!





Tunalover

 

[mrainey]

CNC machining centers in good condition (I'm not experienced with punch presses) can position accurately within a few ten thousandths of an inch. Beyond that, the locational accuracy of machined holes is pretty much dictated by the fixturing, cutting tools, and machining methods used to make them.


Manufacturing Freeware and Shareware

http://mrainey.freeservers.com

 

[CMfgE1]

The problem with specifying tolerances is that the vendor must now hold to those all the time.

Its common knowledge that when you tighten the tolerance you will pay more. This is caused by increase machine time and such. So if your vendor is holding a .005" center line hole location, I would think this is sufficient for most applications.

If your trying to locate two pieces in an assembly than there could be a problem. Or lining up dowels for some reason. You can also cause more problems by specifying tighter tolerances due to tolerance stacking. The bolt or nut your using (threaded rod, stud, etc.) certainly is not that tight. SO less might not necessarily be better.

Just my .02

Quote: "Its not what you know, its who you know"
Everythings a learning experience-Everything

 

[BillPSU]

What tolerance you hold will depend on the type of machine, materials, tooling, and process.

Lets look at punching on a CNC machine. Say you are punching .250" thick material. The punch and die are aligned but not perfectly so the bottom of the hole is offset from the top of the hole and the bottom of the hole is larger than the top. You position the plate on roller balls and the plate is out of flat. Depending on the flatness of the plate will determine some of the positional error. Ball screw error comes into play such as reversing error and positional error. The clamping system holding the plate/sheet may have some movement along the moving axis. Head deflection while punching may also add error. +/-.005 within a hole pattern on a punch is a very good tolerance and I would prefer +/-.010. Positioning the pattern to the edge of a part can be very problematic if the edges are not punched/burned in the CNC program. Edges can be out of square and cause large errors. The thickness of the plate will also cause problems, the thicker and larger the plate the more problems you will have. Say you punch and plasma cut 60" x 60" x 10 Ga A36 on one machine and on another machine you cut 60" x 144" x 1/2" A36 plate. The 10 Ga weighs 138 lbs and the 1/2" wieghs 1229 lbs. The heavier plate will cause increased wear and tear on the roller balls supporting the plate, the clamps holding the plate and the ball screws driving the plate. The 10 Ga sheet material will also have a better surface and not contaminate the table rollers with scale as much as the 1/2" plate. Punching will not produce as good of locational tolerances as machining.

 

[ajack1]

The usual rule of thumb in Europe is 0.1 mm for locations, joining parts, jig locations, c/sink, extrusions for tapping etc, 0.25mm for clearance holes that screws or bolts go through and 0.5 for drainage, weld guns, holes for hanging for painting, coating or to lighten the part.

 

[Tunalover]

So far-
mrainey: +/-.0003"
CMfgE1: +/-.0050"
BillPSU: +/-.0050"
ajack1: +/-0.1mm=+/-.004"

Thanks guys for replying and sharing your thoughts!

However, these figures are "rule of thumb", "I would think"s or "should"s. Where out there is measured data including standard deviations and probabilities?






Tunalover

 

[ajack1]

Tunalover 0.1mm is standard in Europe for all “critical” hole positions for Audi/VW, BMW, Ford, Rolls Royce, Bentley, Jaguar, Land Rover and Renault. The Japanese manufactures that I have dealt with Honda and Toyota have completely different systems that I will not even try to explain on here.

Where they differ is “secondary” holes, usually clearance where some are 0.25mm and some are 0.3mm and on lightening holes and access holes some are 0.5 and some are 1mm.

The only place I know to get their standards from is the company themselves, they supply them to all first tier suppliers or find someone who works for a first tier supplier that is happy to give them to you.

 

[Tunalover]

Thanks ajack1! Are the tolerances you mention in-pattern, pattern-locating, or both?


Tunalover

 

[ajack1]

This is true for body panels, secondary panels, reinforcement struts, brackets and fascias that are stamped and or formed. Like I said generally the only things tied up to 0.1mm are either location holes for either inspection or as a tooling aid, weld jigs, weld nuts etc or fixings like screws or rivets.

Clearance for screws/ bolts tends to be 0.25/0.3 and the hole dimensions are also less tied up, however sometimes the holes are tied up but not the position for things like wiring clips where fit matters but position less so.

I hope that helps.

 

[RedPen]

All,
I would like to have a feature-based tolerance scheme for CNC machined parts similar to what sheet metal shops publish for their parts.

For instance, sheet metal suppliers will tell you they can hold ±.005 hole to hole (same flat), ±.010 hole to edge, ±.010 edge to edge, ±.010 per (90 deg) bend, etc. The tolerances they say they can hold are determined by the type and quantity of the feature(s). Large parts have larger tolerance ranges.

Are there any such tolerance tables or rules of thumb for CNC machined part features? Perhaps an error factor that is multiplied by the distance, similar to that used for injection molded parts?

Thanks for your time and consideration.

 

[Tunalover]

RedPen-
Are you commandeering my Thread?


Tunalover

 

[RRBD]

Here's the deal, most CNC are very accurate and repeatable to within tenths. The tolerances come when you start putting tools in the spindle. Take drilling for example, I find that I can generally hold a tolerance within .003" of nominal when drilling using a screw machine length drill. You can spot drill and get it closer but it all adds time. Most clearance and threaded holes dont need to be any closer than +/-.005 or (T.P. .015). Dont design around someones machine tool, design for what is absolutely essential. I regularly see prints that have a true position tolerance of .005 on 9/32" diameter clearance holes for 1/4-20 shcs. I tried to explain that a T.P. of .015" would be better suited for what they are trying to do, but, Engineering says this is what we need, so thats what they get, I just charge more. Detail and Dimension your drawings realistically and if your shop cant handle it, find a new one. Just my two-cents

 

[Tunalover]

RRBD-
Here's the type of trouble I've been getting into:

Note: +/-.005 is equivalent to .014TP and
+/-.010 is equivalent to .028TP

Suppose I have a small purchased enclosure (say an electrical component of some kind) with 2-56 threaded holes. Let's call this part No. 1. Next suppose I need to mount this component to the inside bottom surface of a large enclosure using 2-56 screws. Let's call this part No. 2. The enclosure surface needs clearance holes and countersinks because the outside bottom surface must be kept flush.

The following formula holds for the clearance hole:
H=F+T1+T2 where T1=the in-pattern TP of one part at MMC, T2=the in-pattern TP of the second part at MMC, F=the fastener major diameter at MMC (=.086), and H=the clearance hole diameter at MMC. Suppose the plate with the threaded holes is purchased from a supplier who is largely unknowing about his tolerance capabilities, and he says that he can provide only +/-.01 between the threaded holes. Thus T2=.028 (we have no control over what tolerance he says he can do!). Now if I use .014TP for the clearance holes, then the clearance hole at MMC must be .086+.018+.014=.086+.032=.118. Now the flathead screw is the 100degree kind with a .172 head diameter (across flats). If the countersink is independent of the clearance hole (and it is if the machine makes the hole + csk in two operations instead of one) then the required countersink diameter at MMC is .172+.032=.204.

Take a look at the clearance hole and countersink sizes. They are BIG. These are MMC values so the nominal values will be more like:
hole dia=.118+.001=.119 [using +.004/-.001 on the drill (or punch) diameter]
and csk dia=.204+.005=.209 [assuming +/-.005 on the csk diameter].

These numbers are TOO BIG for this design but the only thing we can control is T2! With thin sheet metal, the head of the screw will actually stick through the other side! Bottom line: +/-.005 is TOO COARSE in many fixed-fastener designs!

RRBD and ajack1: You SAY that CNCs can provide positional tolerances in the tenths of thousandths, but where does it say that in writing? I must have hard data before tightening our tolerances and changing our processes. HELP!





Tunalover

 

[mrainey]

A Google search turned this up. Some good info on punch press capabilities and design considerations.

http://www.makeitmetal.com/resources/CH5_CNC_A.asp

Manufacturing Freeware and Shareware

http://mrainey.freeservers.com

 

[RRBD]

First, I try to avoid putting the heads of fasteners in a place they cannot be reached for service in the field(ie: the mounting side of an enclosure)Second,when c'sinking holes in thin sheet metal, there is no sense drilling a hole and then opening it up again with a chamfer, find/grind a 100-deg spotdrill or something so its all in one operation. I cannot find any info on a 2-56 w/100-degree head in my MHB, but you say the head will actually stick through the material which leads me to believe the material is around .035 thick, which if unsupported during machining,you will likely have problems c'sinking it if its anything other than plastic. Considereing the criteria, Is glue a possibility. Lastly, if your component is laying flat against the enclosure and you are c'sinking so the head protrudes the inside you are going to bottom the head out in the component before the head even touches the enclosure.As far as milling machine specs/accuracy, go to thier web sites, many have them posted on their sites.
Anyway, I'd look into some mounting alternatives, you might save some money............

 

[BillPSU]

tunalover
The problem you have is accepting your vendor saying he can only hold +/-.010 locational tolerance on a .072 dia hole(tap drill for a 2-56). I've been a purchasing agent and I know suppliers can hold whatever tolerance you put on the print. If they cannot then source this part with a supplier who can. It may cost more money but having a part which works is what its all about.

Ideally when you specify locational tolerances, share the tolerance between the tapped hole and the clearance hole and if necessary increase the clearance hole diameter increasing the available tolerance.

When machining holes locational tolerances capabilities change due to mostly the tools used to manufacture the hole not the CNC used to make the hole. As drill length get longer tolerance zones get bigger. Say you drill a flat plate without spot drilling using a screw machine length drill, a jobber length drill, a taper length drill, an extended length drill. Now lets put the drills into an extension. Length does matter and in this case it is bad.

The accuracy of the drill effects the hole produced. The web centrality, the drill point, and the web thickness can effect the location of the drilled hole.

Good machining practices produce the best location holes. Spotdrill if possible before drilling. Use quality tools. Keep the tools short. Make sure they are properly sharpened and properly resharpened. Make sure your setup is rigid and doesn't impact the parts quality.

 

[Tunalover]

Folks-
Thanks guys but the Thread is not converging to hard data; everything remains empirical.

Historically, parts come in with the hole patterns "right on." That is, no matter how much I bend over backwards to accommodate the metalwork and component suppliers and regardless of whether the part has a robust design or not, the parts seem to arrive "dead nuts" no matter what the drawing specified. Then I have our Production and Quality folks who say "why worry about tolerances; designers in the past didn't worry about it and the parts always fit fine." It's hard to fight people who say why fix something when it aint broke! It's like people driving over a crumbling bridge; people are happy as long as they can get across, but once the bridge fails THEN they have a problem!

I encounter fixed fastener designs all the time from earlier designers who gave, say, a .090 diameter clearance hole for a No. 2 fastener, and the parts never fail to fit. The question is: do you want a design that CAN fit or do you want a design that WILL fit? Methinks the latter but top management believes that the holes designed for worst-case conditions are too big. Designers are being saved by the accuracy of the manufacturing processes but the manufacturers can never say what that accuracy is!

I'm one of these odd sorts that likes to generate sound designs that are based on real world data. It's just too bad that the fabricators want to charge us so much for tolerances that they end up giving us anyway!






Tunalover

 

[RedPen]

Tunalover,
Sorry. Not my intention to commandeer/hijack your thread. I was under the impression (mistaken?) you and I were asking for similar information even if it isn't formatted the same way.

 

[Tunalover]

Not to worry RedPen. Just try to glean what you can from this thread before starting another. Or start your own now!


Tunalover

 

[segges]

I think what you are asking is why do shops ask more for +/-.002 location vs. +/-.005, when the parts come out dead nuts anyway. The only thing I can say is that when you see a +/-.002, you will start planning accordingly, and depending on the material, feature, location etc, that may add additional machinig steps that you would otherwise not do. Example, You need a 4 clearance holes of .251 - .256 dia, TP .002 to each other. Well, in this case I would 1 - Center drill, 2 - drill (appr. .210-.220) 3 - Endmill (15/64) 4 - ream or profile to size.
Now if the same tolerance is .005 TP, You can do away with the endmill operation, or may be the center drill as well. If you now open the diameter tolerance to say .251 - .261, then it is possible to do nothing but drill. That is how you save 3 tool change worth right at quoting time. Yes, as someone pointed out machine repeatability is most likely not an issue until you start splitting tenth-s, but tools, even good ones vary somewhat ( in your case I would rather look at cutting tool and toolholder manufacturer's specs ) You can buy 10 drills from same mfg, same lot, most likely you'll have at least .001 difference in the finished hole, add to it the error by unchucking/re-chucking the same tool, the size difference can be easily at your +/-.002 limit.
Also, if the part does not meet the +/-.002 limit, it is scrap, go and make another one at your cost. With the .005 tolerance the scrap rate is probably an order of magnitude smaller, and so are your losses.
Now don't get me wrong, I am not against tighter tolerances, just tired of stupid ones. Example : I could not get an explanation from an engineer why he wanted +/-.0002 tolerance on a hole for a .125 spring pin. His reason (and only reason) was that it works and he will not change it.
And lastly, I once worked for a company that made film processors, welded frame, fairly heavy inside components, and covered with sheetmetal using 10/32 and 1/4-20 fasteners. After the installation, once the tanks been filled with chemistry and water the whole thing moved enough that virtually none of the covers were re-installable again without opening the holes. In the case of 10/32 we've drilled appr .210-220, 1/4-20 got .280-.290, and from then on the covers fit perfectly every time.