Machined parts all exactly at limit of tolerance (MMC) - is there a practical reason?

[Aries6776]

I've just had a first iteration design machined. It's all within tolerance but on 6 internal diameter features they have hit the bottom of the tolerance to within 0.01mm on a range of 0 to -0.05mm and on the one external diameter they have hit the absolute max size. So my question is, they've obviously aimed to hit the minimum hole size and the maximum shaft size (unless it's some amazing coincidence on all 7 features), is there some practical reason that they've done this?

I'm a design engineer by trade and I've done a little bit of machining. I always aimed for the middle of the tolerance band by default. The assembly will still work (it's within tolerance) but I'm going to have a batch of these made and I'm wondering if I need to adjust the tolerance if they are always going to hit maximum material condition because it makes fitting a little bit more time consuming. I'm asking here just in case I'm missing something obvious before I speak with them again.

The work was done on a 3 axis CNC, not sure of the make.

 

[sfriedberg]

Speaking as a fellow engineer, set your tolerances so you don't have to do any fitting. If a transitional fit is inconvenient and you can't go to a fit with greater clearance, then add a lead-in chamfer or similar feature to make assembly less fussy. If the shop meets your specified tolerances, the parts are good, and you don't get to kvetch. :-)

 

[moonlight machine]

Speaking as a fellow engineer, set your tolerances so you don't have to do any fitting. If a transitional fit is inconvenient and you can't go to a fit with greater clearance, then add a lead-in chamfer or similar feature to make assembly less fussy. If the shop meets your specified tolerances, the parts are good, and you don't get to kvetch. :-)

I always aim to make IDs just bigger than on size within tolerance and ODs just smaller than on size within tolerance.

 

[Aries6776]

Thanks for your replies. I'm aware I can adjust the tolerances, I'm just wondering if there was a reason for them making the parts to the maximum material condition? Is it a test to see if I know what I'm doing? Or is it something amusing for them? I worked with an experienced machinist who would delight in making exactly what you put on a drawing, even though he knew it would ruin the part! It didn't happen to me but he did it to a few other junior designers. Or is it just a cautious machinist who doesn't want to risk oversizing holes or over reducing a turned shaft? Or is it a way to get me to spend more money, because I'd need remedial work to adjust the fits?

I got around the issue by just sticking some parts in the freezer and others in the microwave
I didn't want to specify tighter tolerances to keep costs down but practically I don't think it will make any difference because they have easily hit the numbers. I'm just trying to work out why they have done this so I know how to deal with them. Do I want to give them repeat business?

 

[Aries6776]

I always aim to make IDs just bigger than on size within tolerance and ODs just smaller than on size within tolerance.

Thanks, this is what I would assume someone would do by default when machining something.

 

[Clive603]

Setting tolerances and fits has always been a bit of a black art. Especially if you need "real nice" fits without grading parts for selective assembly.

Lot to be said for making first off test parts to minimum hole and maximum metal conditions to verify that the extreme pair actually assemble easily enough. Something I always tried to do.

You aren't the first person to discover that a pair of end tolerance fits that, according to the book, should work just fine are just too much faff to assemble on the bench. Time to move the limits a touch I think.

These days CNC machines are so good that calling out a 0 to - x and 0 to + y pair is asking for trouble. You will get some 0, 0 pairs that won't fit without a BFH. Always the last couple or three so no margin for a quick swopsie!

Clive

 

[guythatbrews]

Put this question to the shop that made the parts. It is entirely possible you got lucky the part is barely in tolerance instead of out of tolerance. Not all shops do good work, and some will sell non-conforming stuff with impunity.

 

[jaguar36]

Most likely its to allow for rework if something goes wrong. If the tool breaks or they messed something else up, having the most material left gives them the highest chance they can rework it and still have it meet the tolerance.

 

[Mtndew]

is there some practical reason that they've done this?

Could be.
Sometimes if a feature is a bitch to machine they will take it just into tolerance and be done with it.
Or that's just the habit of the machinist/shop that made the part for you.

But you put the tolerances on the print, if being at one end of those tolerances makes more work for you, then change the tolerance if you can and be done with it.

 

[Sam I]

How were the parts modelled (assuming you supplied 3D CAD files)?

Most models that come to me are set at one end of the limit and so this ends up being the programmed size generated from my CAD/CAM package. I would personally adjust a wear offset at the machine to account for any part variation but I'd stay pretty close to programmed size as changing the offset changes every diameter cut with that tool and can have unwanted consequences elsewhere. If I hit within .01 mm of a programmed diameter at the machine I'd be pretty happy and leave it be. If I thought there could be a problem I'd have to go in and modify the CAD model or the part program (although personally I don't like modifying the program directly as it gets overwritten should there be a change in the CAM system).

Sometimes I get a customer who supplies the models at mid limit and it saves a lot of time and effort having to modify the models. As a programmer I really appreciate it when that happens!

This only applies however if your machinist is using CAM to generate the programs for the machine.

 

[VTM]

Could be.
Sometimes if a feature is a bitch to machine they will take it just into tolerance and be done with it.
Or that's just the habit of the machinist/shop that made the part for you.

But you put the tolerances on the print, if being at one end of those tolerances makes more work for you, then change the tolerance if you can and be done with it.

It could be this. A former employee always did this. If he had .005 He'd use .0048 every time. Drove me nuts.

 

[Kingbob]

Most likely its to allow for rework if something goes wrong. If the tool breaks or they messed something else up, having the most material left gives them the highest chance they can rework it and still have it meet the tolerance.

My guess is exactly this as I am also guilty of this and do it for this exact reason. I make valve parts and often times plants during unplanned outages will authorize re-machining of parts just to get them to function until replacements can be found/made, were talking turn around times of a couple of hours or valve parts ridding on airplanes. So please don't immediately assume mischief on the part of your machine shop. I think you should accept it for what it is, a valuable learning opportunity. Move your dimensions around, adjust your tolerances and move on.

 

[cngbrick]

Asking the shop/machinist would probably get you your answer.

Ultimately, your model and drawing are tools to communicate your requirements to the machinist. The machinist has to assume that meeting the tolerances will produce a part acceptable for you, this is a contractual obligation. It's unfair to expect the machinist to guess that you expect the part to be made to the middle of the tolerance. It is your job to clearly state your requirements. You can certainly solicit advice from the machinist before establishing your tolerances if you intend to work with this machinist but don't take their advice and then use another shop unless you are upfront about the situation and fairly compensate them.

 

[GregSY]

The bottom line is you gave tolerances and they met them...they owe you no further reasons or explanations. There's a good chance their answer would be 'it just turned out that way'.

30 years ago....we had an order for a large synchronous motor for a ball mill. This was around 13,000HP 180RPM. The motor was assembled and tested fine, when it got to the jobsite it was installed...for those who don't know large plants, installing a new ball mill and motor - just the installation - is a long and expensive process. Anyway, they started the unit and right away the rotor rotated...but the shaft didn't.

Turns out the drafter had specified the ID of the rotor hub at the exact dimension of the OD of the shaft, and no one in engineering caught it. It was a good enough fit to run unloaded, but not good enough to transmit 13,000HP at 180RPM. This is about a 24" diameter, forged steel, and normally this interface is an interference fit which requires the hub to be heated and the shaft to be frozen before they are stabbed together.


Typical hub:

 

[Tonytn36]

Given the tighter tolerances it is possible that the parts measured nominal in the non-temperature controlled shop they were made in, but now in your temperature controlled place they are to edge of tolerance.

 

[BT Fabrication]

Tolerance is all up to the designer.
Most i've seen in general tolerances are plus or minus 0.005" if its nothing important.
Shafts are usually obviously tighter tolerance but all depends on the application if its a press fit or shrink fit interference needed.
The archilles heel is the tighter the tolerance is more of a pain, thus costs more $ to make if you need to hold 0.001" vs 0.0001", the extra zero will always add extra zeros to the bill.

Being on the machinist size, ID bores we all like to shoot smaller, as you can always hone or ream it out. Much harder to add material back, especially if it's a first run part. A quick hone and a polish can take off a few thousandths of an inch quickly if needing to be opened up a bit and only takes minutes.
Most of the time bringing parts back and adding material back to a shaft or bore requires the whole part to be remade at more $$ cost.


End of the day, they hit tolerance, if you have found it needs to be different, change the tolerance or sizing to match exactly what you require or communicate it to the people making the part and have it in writing communication by email etc. That way you will know its on paper and can specify what you really need, I have had customers not know, had to go back and forth a couple times for changing specs just like this as it was told to be press fit but was exact diameter of the shaft and would have been a slip fit.

 

[eKretz]

I also always shot for the mid to high side of a given tolerance on internal sizes and the mid to low side on external sizes, but I was never doing high production runs. That's on parts that were slip fit. I was targeting easy fit up and assembly for whoever had to put the parts together. As a supervisor I asked the guys under me to do the same also. See, I supervised the assembly/millwright guys too - and they would pitch a bitch if the parts didn't go together easily - whether actually in tolerance or not. That's on top of it costing the company more money as time to get the parts assembled. The other question is did the guys making the parts know that they would be assembled together? If it's a large shop the people running the parts may not even talk to each other.

However, I can understand why a shop doing very high production might make their parts to MMC to allow rework if sizes started to drift. But only if the material was very expensive or the machining took a very long time. Otherwise it's simply more efficient to throw another piece of stock in the CNC and push "Start."

Anyway, in the end, this is a matter of tolerancing. If they hit the provided target you have no grounds for complaint. If you need a different target hit, you need to provide it and pay accordingly. If you are friendly with the shop, you might be able to discuss the situation and ask if they can shift a bit on the tolerance band if possible. They may well accommodate you if you're a good customer and the parts aren't too complex. I wouldn't ask that on a first time job though, just change the tolerance to be more in line with what you'd like, as the others have already said.

 

[Mr.M]

Thanks for your replies. I'm aware I can adjust the tolerances, I'm just wondering if there was a reason for them making the parts to the maximum material condition? Is it a test to see if I know what I'm doing? Or is it something amusing for them? I worked with an experienced machinist who would delight in making exactly what you put on a drawing, even though he knew it would ruin the part! It didn't happen to me but he did it to a few other junior designers. Or is it just a cautious machinist who doesn't want to risk oversizing holes or over reducing a turned shaft? Or is it a way to get me to spend more money, because I'd need remedial work to adjust the fits?

I got around the issue by just sticking some parts in the freezer and others in the microwave
I didn't want to specify tighter tolerances to keep costs down but practically I don't think it will make any difference because they have easily hit the numbers. I'm just trying to work out why they have done this so I know how to deal with them. Do I want to give them repeat business?

This issue that is costing you more money as you say is because you have it toleranced wrong. Nothing nefarious on the machinists part.

 

[Finegrain]

I don't know if the ID's were small enough to have been reamed, but if so, the shop making the parts may have used the lower limit for the reamer sizes. I usually do that. Reamers rarely make too small of a hole, but they often make a hole that is slightly oversize. So if the hole is, say, 7.98mm +.01/-0, I'll start with a 7.98mm reamer.

.05mm is a pretty generous tolerance though, so for your parts, I personally would have used a reamer a bit bigger than the min size.

Regards.

Mike

 

[jim rozen]

Oftem problems like this can be short-stopped by a) designing so it assembles at any point in the tolereance stack-up, and b) stapling the two drawning together and putting a note saying "part 1 to be press fit assembled into part 2." Or as they say in the greeting card business, 'insert tab A into slot B.'