CNC positional tolerances
CNC positional tolerances
(OP)
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!
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





RE: CNC positional tolerances
Manufacturing Freeware and Shareware
http://mrainey.freeservers.com
RE: CNC positional tolerances
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
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
RE: CNC positional tolerances
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
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
Tunalover
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
Are you commandeering my Thread?
Tunalover
RE: CNC positional tolerances
RE: CNC positional tolerances
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
RE: CNC positional tolerances
http://www.makeitmetal.com/resources/CH5_CNC_A.asp
Manufacturing Freeware and Shareware
http://mrainey.freeservers.com
RE: CNC positional tolerances
Anyway, I'd look into some mounting alternatives, you might save some money............
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
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
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
Tunalover
RE: CNC positional tolerances
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.
RE: CNC positional tolerances
When you say .002 TP that's a far cry from +/-.002 RFS. Plus or minus .002 is equivalent to .0056 TP RFS. I'm not asking for the Moon! In my business, .060-80UNF tapped holes are common. With things getting smaller and smaller in the electronics business the tolerances often need to get smaller too. Why can't the machine shops study and publish the tolerances that they can hold with statistical certainty?
I spec almost all feature patterns on an MMC basis so as to take advantage of bonus tolerances. Also, I normally use composite tolerances to that the pattern-locating tolerances (that are so much affected by fixturing and setup) are loose (sometimes >DIA .100 at MMC). As for in-pattern tolerances, these are a lot tighter but even then these have bonus tolerances that grow with the hole diameter!
Typically, the spread on my drill and punch size tolerance starts at .005. So if a DIA .125 +.004/-.001 drill (.124-.129) has worn to effectively .129 (the LMC limit) then each hole will receive a bonus tolerance of DIA .005. Don't most machinists understand the MMC concept and the bonus tolerances that come with it?
Sorry if I'm venting on you!
Tunalover
RE: CNC positional tolerances
To get back to your initial question, "... "typical" high-probability positional tolerances for CNC...". As you already answered for yourself, it's "broad", the question and the answer. Can a CNC machine (mills and lathes and such) hold tenths? Yes, and even better under the right conditions. Can everybody hold tight tolerances? No. Several CNCs claim positioning down to .00005 and less. However, this is under the most ideal situations. Not all CNC's can do this. Even if I bought one that "could", my shop environment may not allow it. Some shops are hostile enough (environment) that they have trouble with couple thousandths or even more.
I'm glad you want to build me a "better bridge" (relieved actually being that I'm in CA), but I may not be able to supply you with the proper "materials". You're the engineer. If you're tolerancing a part because you feel "that's whats required", then do so. Just don't expect everybody to be able to do it. If you didn't like the answer you got from your fabricator, then go out and get it quoted somewhere else. That would make it his loss, not yours. Gather some data for yourself about job quoting and what dictates part prices. Right off the bat you made an assumption "that he simply doesn't KNOW what his equipment is providing him". For all you might know, his machine is a 40 yrs old G&L. Besides, he didn't say he couldn't do it, just had to raise the price. Well, if you don't like that, get another quote. You're not tied to him by rope are you?
Many things dictate the type of tolerances a machine can hold, even if you start with a "top of line, super precision" piece of equipment. Environment (temp and humidity maninly), type of machine footings, the floor it sits on, cooling capacity and capability, tooling, set up type, fixturing, heat generation, material type (of the part), size of part, shape of the part, climate control (at the machine, during machining, and then in QC or QA), part rigidity, quantity of work, lead time for parts (yes, think about it, if you need a part this afternoon, it might not be as nice as the same part in say a few weeks). This list goes on and on.....
So, if you want to tighten up tolerances, or you need a part thats super critical with TP .000 all over the place, so be it. I'll back you up if you can justify the need. I can draw/design just about anything like you. That doesn't mean I can make it though. I don't do any punches so I couldn't expain to you why +/- .005 would raise the price. For machined parts however, thats a fairly standard tolerance. I can hold it better than that, way better. Most of us will try and run parts "nominal" and maintain that. But when you tighten it to .002, this changes several things. Now I may need to adjust the current process, alter the program, add tooling, buy different tooling, add more inspection, buy inspection equipment, add more SPC, CPk may force a process change, slow down tool speeds,..... All of this, even if only some, costs money to the fabricator directly and up front.
So, whats the "standard tolerance" for CNC,.....
Anywhere from 0 to 7-1/2 miles. It just all depends......
Like you said, its a pretty broad question.
RE: CNC positional tolerances
I recognized that my question was broad from the get-go. Don't you realize that it's the pattern-locating tolerances that are so sensitive to the variables you mentioned? That's the beauty of composite tolerancing! Also, by Y14.5M-1994, dimensions and tolerances apply at 25C (room temp) so as long as fabrication and inspection are near 25C then temperature is not a factor. Also, I never said I wanted to hold .000 TP. It is my mission to make tolerances as LOOSE as possible! I'm one of those "rare bird" engineers who understands GD&T and TRIES to use it to keep costs down. Unfortunately, there are many fabricators who jack up the prices because "those fancy symbols" must mean the tolerances are "dead nuts." Only buyers and purchasing managers are empowered to source the parts. I get flack from buyers for calling out tolerances that are as loose as the design will permit (as loose as possible) because he says the GD&T causes the fabricator to raise prices! Also, I need to mount parts that often have a 2-56 mounting hole pattern held to +/-.015 betweem holes! The host part I am designing (the one the component is mounted to) consequently needs to have a HUGE clearance hole and TIGHT in-pattern tolerance just to make sure the parts will fit together. This sometimes causes the screw head or flat washer to fall into the hole (or I end up using a large diameter fender washer) because the hole has to be so big! Bottom line: the component supplier: A. Is giving me, probably, +/-.003 in-pattern but he doesn't know it, and B: Because he doesn't have a clue as to what tolerance he is giving, he puts a ridiculously rough tolerance on his drawing or data sheet.
Often in the electronics business it is the component supplier who specs the tolerances. He then outsources the machining to a fabricator who knows he can hold much tighter but is ecstatic to see that he can hold the specified tolerances even if he's using a drunk machinist on a 1930's vintage Bridgeport!
The biggest obstacle to cost savings using ASME Y14.5M-1994 are those people (engineers, designers, and fabricators alike) who don't spend the time to learn the method and get the wrong impression that "those fancy symbols" mean "dead nuts" tolerances. ARGGGG!
Tunalover
RE: CNC positional tolerances
Don't you realize that it's the pattern-locating tolerances that are so sensitive to the variables you mentioned?
Got news for you, feature tolerances are also affected by many of those variables as well, not just location or positioning.
Quote:
Also, by Y14.5M-1994, dimensions and tolerances apply at 25C (room temp) so as long as fabrication and inspection are near 25C then temperature is not a factor.
This is an ideal condition on order to attain a controlled condition. Many shops, if not most, do not conform to this and have to attain/maintain tolerance accordingly. Which includes but not limited to: cheating the machining condition, program or tolerance, creating seperate environments for at least one machine, not quoting a job with low tolerance, not machining particular materials, etc.
Quote:
Also, I never said I wanted to hold .000 TP. It is my mission to make tolerances as LOOSE as possible! I'm one of those "rare bird" engineers who understands GD&T and TRIES to use it to keep costs down. Unfortunately, there are many fabricators who jack up the prices because "those fancy symbols" must mean the tolerances are "dead nuts." Only buyers and purchasing managers are empowered to source the parts. I get flack from buyers for calling out tolerances that are as loose as the design will permit (as loose as possible) because he says the GD&T causes the fabricator to raise prices!
I jumped the gun a bit here on a couple of things and should have carefully read all of the posts. I got off on a tangent. You are a rare bird indeed that you have some cost understanding relating to GD&T. I know dozens of companies who could use someone like that.
As far as the excuse of GD&T causes the price to go up..... well thats just pure crap. There's no reason for it. If I made a part with +/-.005, and that changed to TP .014, I don't raise the price. Why? Just because you now have TP on it doesn't make the part any harder. Now if the callout changed to TP .005, that might have an effect. But its on a case by case decision. I cut TP .000 parts quite often (with MMC being the only tolerance). But thats because I have the capability of doing so. But that part does have some added cost because of it.
Quote:
Where out there is measured data including standard deviations and probabilities?
There isn't any. There are too many variables. The only reliable source for this is going to be the data your individual suppliers are willing to share with you. That's provided that they actually keep track of the data, compile it and scale it. Then continue to track and monitor. I'll say that most shops don't do this.
Sounds like you gave your part a fair tolerance that wasn't "tight". The GD&T gave him a scare. IMO, I'd start getting that part out in the field for other quotes. I believe his machine can hold what you need, he just doesn't understand how the callouts translate for him. Of course, I don't remember reading what you were actually calling out so I'm guessing here. Bottom line, there are thousands of shops out there, get it quoted till you get what you want. If you're not getting it, then there might be some more investigation required in finding out why, and what you can or can't do about it.
RE: CNC positional tolerances
To answer one of your previous question (and I know I will get hate-mail for it) Yes, there are lots of shops that either do not understand TP tolerances (let alone the difference between MMC and RFS), or choose to ignore them and err on the side of caution.
My case is unique as I am a small, up and coming operation, and try to learn everything there is to produce correct parts with the correct process and do whatever it takes, but in larger or older shops this is what I guess happens.
For short to medium runs, parts are mostly made by real machinists who don't know or care better, they just want to make the part right the first time, every time. This most likely results in additional steps and time since making it right is better than twice.
For larger volume though, the process is first developed by engineers or machinist, bearing in mind that the actual mfg. will be done either unattended or by "unskilled" operators, so anything that may go wrong has to be thought of first and steps must be taken to prevent it. The tighter the tolerance, the more "bomb-proofing) needed. They may even tighten tolerances in the mfg process as to eliminate certain inspection steps at the end. (good example would be to hold a diameter to +/-.001, if that will be a locating feature in a later operation)
Now to answer why there are no clear data on dimensional spread, as psychomill stated, there are way too many variables. Again same tool from same lot will most likely cut different, also tool wear will have to be calculated up front, which is very very very much dependent on the individual part itself (material, rigidity, feature size, shape etc.) In fact I would argue that machine tool positioning accuracy is almost immaterial for all but the tightest parts, as the actual positioning and contouring should be no more than .001 deviation if proper speeds and feeds are used.
Lastly, I would again refer to psychomill, and commend you for your effort in this balancing act. There should be lot more of you out there. Don't know what you've got out of this discussion so far, but send RFQ-s to more places, and you may also want to talk with individual companies about the process or possibilities. If they are interested in making the part, they certainly will have suggestions or recommendations, as well as questions on what is important for the application. Sometimes these discussions give you the best idea what is reasonable from a certain process.
I think psychomill and I have stated the pure machining possibilities, for stamping and forming someone else should jump in as my experience there is very limited.