How Is GD&T Manufactured?

Good GD&T should start with the function of the part. If the shaft is used as a drive shaft of any sorts, the the tolerance in the straightness, runout, concentricity should be a mirror of what you need for the shaft to perform the task.

Now, how does that effect the manufacture, the same way any tolerance effects the method of manufacture, the tighter the tolerance the more processing that is involved. GD & T should only clarify the design intent.

Let's take a steel shaft of most any length, without a callout for straightness, the part would most likely be produced on a lathe and from bar stock. Straightness you could expect would be within .005" total.

Runout, is measured from one diameter of a shaft to a different diameter of a shaft. Support the shaft on one or more datum diameters and place a dial indicator on the part of the shaft you want to inspect. Slowly spin the shaft and the runout is the Total amount of Indicator Movement seen (TIR).

Concentricity is used not by checking the outside diameter of the part but by caculating the center of the inspected diameter and comparing it to the datum diameter.

You asked about cost, Cheapest way is just a lathe operation for the shaft, but in you put a real smooth surface finish, or real tight straightness requirement, you could add a grinding operation to maintain the requirements, double the cost. Well, not double, but add about 1/3 the cost. Cost of the material won't change.

The same is true for a true position callout, the tighter the tolerance the more care needs to be taken. A 0.020" true position will be drilled, but a 0.003" true position would be drilled with a smaller diameter drill then bored, add a tool, add cost.

Hope this helps, let me know if you need more information.

Laby

Not to put too fine a point on this discussion, but the grinding operation itself doesn't straighten the bar, the grinding house often needs to restraighten the bar to get it straight enough to grind.

The grinding operation does improve surface finish by removing asperities. it also improves size tolerance and concentricity. It does not straighten the bar.

milo

Milo,

I was thinking a centerless grinder would straighten a part... what do you think?

How does the grinder impart sufficient force to 'unkink' the bar and put surface into compression? Surely not through the abrasive wheel. nor through the wheel that holds it against the grinding wheel. The bars generally go through a medart 2 roll straightener once or twice before grinding. That's the magic. Grinding is merely last step.

milo

Maybe I'm all messed up here, I was thinking if I had to remove .010" total and i had a bend of say .003, then it would be straight when it came out. Reason is the centerless would remove the high spots first. Any bend beyond the material removal, no question would require a straighten operation.

In that case perhaps.

I have seen many shafts come out of the centerless grinders where the kink or bow (camber) was so severe that all the removal came off the high side, leaving the low side 'untouched.'

So to your point, there may be some level where the departure from straightnessis so slight that the stock removal may be sufficent to 'correct' the straightness. but for lack of straightness exceeding that level, the departure frrom straightness exceeds the process's ability to correct.

In my experience, grinding crooked bars gave us ground crooked bars, not straight ground bars. i regret that I don't have my data, it was several promotions and several companies ago.

milo

milo

wow! I think maybe i should go back to school. Grinding does not straighten the shaft? true after heat treating you must get it close to,before you begin the final process-grinding.

If the bowed part does no recede below the lower tolerance limit and the high point does not extend beyond the upper tolerance limit then grinding can straighten the bar but only if concentricity is sufficiently accurate from end to end.

Form - Fit - Function

thanks for the reply. I really don't have the time today to comment fully on your post but i can see you make a good case: performance vs design.

Perhaps your textbook contains the answers.

Thanks Laby:

Good info. I've been an automotive designer for 20 years and have spent alot of time with machinists and in machine shops. It was very hard too get any type of info from them on how they actually stick to GD & T callouts and what process they use. You usually get a different answer everytime. Also I think they don't want us engineering types to know that they basically rely on the machine tolerance to hold dimensions so they can charge us more. LOL just kidding guys I know it's tough to stick to GD & T and too apply it properly.

Cheers to the machinists that make it work.

Just a thought: Tolerance and variation are not the same.

Tolerances come from designers who record them on prints (or other product documentation).

Variation comes from tools or processes and gets manufactured into parts.

GD&T (tolerances) tells a producer how much variation will be tolerated and thus which of their available processes can be used to produce the toleranced feature. Producers can then choose the cheapest process(es) that keep variation within tolerances.

Example: I will not re-route a part through a punch press to make some holes with a large positional tolerance if it is cheaper to make the holes on the VMC (Vertical Machining Center) that is already being used to make other features.

True Guest, I didn't mean to imply that the tolerance dictated the routing, although I have seen that, but if the machine I'm on can't hold, or generate the tolerance required, then I must re-route and add an operation, that cost money soley for the reason of the tolerance.

I take your answer to mean that if I have a loose tolerance I'm forced to go to a lesser machine... never the case, If I have a machine capable of 100x the tolerance then instead of re-routing it, I'll call one of the 6 sigma black belts and have them do a study on the feature so they can pound their chest and show everyone their math is Superior.

Most of the time, if it fails inspection, they just wait and re-inspect it on 2rd shift, then it passes.

Hi,

My thoughts on GD&T.

GD &T-->Dimensioning and Tolerance is just the limit of acceptance to the size that does not control the size and shape of the feature.

That is why GD &T comes to picture, where u can control over the shape and size. Which also indicates the functionality of the part.

GD&T also helps in instructs the manufacturer by designating datums and development of inspection gauges.

GD&T applied manufactured part will ease the assembly mismatch and also decrease the rejection at assembly stage.

Sorry guys, I'm the OP and could not spend any time on the net and have a look at the thread during the past week. (Busy in a hectic training program).

It has been a very interesting and useful info exchange (especially grinding and straightness) but my question has remains un-answered. So, probably I need to rephrase it.

First, I am not looking for basic info on GD&T. I am not asking how to determine the tolerances. Here is little more explanation on what info I need.

If the shaft dia has 0.05 tolerance it will probably machined on a CNC. If tolerance is changed to 0.02, it will still be machined on CNC. (Omit the cases where we might need to shift to grinding) Will the cost change? Why? It would be fantastic if you can explain with true, practical shop-floor examples. Also, will the machine be capable of achieving inherent 0.01 straightness tolerance? If I specify 0.001 straightness, how will it be achieved? What adjustments will the machining process need?

What I am trying to understand is how geometrical tolerances are achieved in machining processes?

In other words, what is the machine capability regards geometric tolerances? Do we have to establish it using process capability? Or can machine manufacturer provide us with this data? Is such data available in the machine's manual. (sorry, I have neither working experience with CNC, nor do I currently have an access to one). What are the ways (jigs, fixtures, toolings?) that can be used to enhance geometric tolerance capability of a machine?

For example, I would like to know a guideline like to achieve desired concentricity, the depth of final cut should be less than half the value of the desired concentricity or something similar.

In other words, I'm looking for relationship between GD&T and manufacturing processes which is very rarely addressed in detail.

I hope I have been able to specify my problem with more clarity now.

Yeah your question is a bit wishy-washy.

How long of a shaft? What is the shaft made of? What kind of machine?

I can readily hold most any reasonable tolerance to .0005" using standard tooling and time given certain parameters.

In the first thirty-years in this business, manufacturing, I worked exclusively on precision machining. The closest tolerance I was involved in was. +.0003 -.0001. It took six months to bring that baby in! Three other companies were all competing at the same time.

Automation has taken a lot the heavy lifting out of it, but when you get down to "feel", automation takes a back sit.

There are to many unknowns in your question. What's the part for, will it be heat treated, etc…

Let me try to reframe this in plain english.

The realtionship of cost to tolerance is the tighter the tolerance, the higher the cost.

WIth a wide open tolerance, you can use any machine in operating condition, standard tools, and good enough set ups. And the cycle time is fast and uptime is high because there are few issues and adjustments needed.

As the tolerance tightens, you get limited to machines in better shape, and perhaps more expensive machines with greater capability. You may need more expensive tooling, and you will need to confirm the operation is in control more often. You will also need more expensive gaging. Cycle time may increase, and machine uptinme (in the cut) will surely decline as more checks and adjustments will be required.

As the tolerance further tightens, you will have much less machine up time as your operators are forced to make many more adjustments to try to keep the process in spec. You will need better tooling and the process may require an additional Final step Such as a hone or shave or a light finish pass that will add time to the operating cycle., Time is money. Time with out machine in cut is even more money.

At the point where your process is 'just barely capable' you will add expense as any departure or deviation in the process from statistical control results in scrap for which you will incur costs but not bne paid.

Beyond that, you will need to make a "rough blank" on a less expensive and less capable machine which you will then finish on a more capable secondary machine. This will add expense by doubling setups, doubling labor, and doubling supplies and tools, as well as increasing your total time to fabricate. The fringe benefits of the second machinist become a major factor. (This is why savvy managers buy the most capable capital equipment they can, so that they can drop off parts complete without secondary, thus saving the fringe benefits and medical expense of the redundant machinist.)

Any shop that does not know its cpk for various metal removal processes by tolerance class by machine is committing suicide by flying blind when quoting. This is often the reason that they havea backlog and are late to customer, they quoted, it, took the job, figured out at that point they could n't do it as quoted and have to scab together a process to git'r done.

It has been my experience that reducing the tolerance by the last 10% can often double or triple the cost. the first 90% may only increase costs 25-30 % or less, Its the last little bit that throws you out of capability and commercial success.

Just like pollution control equipment. first 90 % is easy to eliminate. The last 10% may double or triple or more the cost to remove the pollutants.

Waste is when a customer asks for a tighter tolerance than they actually can take advantage of. Value engineering was the term that was used professionally to describe sitting down with your customer and evaluating which features were worth paying for, and which could be done without as drawn. But "value engineering" became "armed robbery" in the hands of the purchasing miscreants in detroit, whose chickens have now come home to roost.

Cockle doodle doo.

milo

Nice Long Post Milo but you said it all in your first sentence: "The relationship of cost to tolerance is the tighter the tolerance, the higher the cost."

Thank you.

I heard a rumor we'd be paid by the word when we're on topic.

Just kidding.

milo

lol

I tried voting as 'on topic' 27 times. I only got to vote once though.