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

 

[Tunalover]

segge-
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

 

[psychomill]

Tunalover,
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.

 

[Tunalover]

psychomill-
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

 

[psychomill]

Quote:
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.

 

[segges]

Wow, this thread got pretty buisy. I think psychomill has very well stated most of the points I was trying to make.
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.