It has been my experience that machinist will more often than not error on the side of caution. I suspect that in this case, using a sharpie, was more of a “I’ll fix him” type of thing but in the end it probably caused no damage to the part.
What is more dangerous than “Guessing”, which again in my experience is rare, is misinterpretation. The machinist does what they think the print is saying but the print is not really saying that. The designer however said something ambiguously or with lack of clarity and the part gets scrapped.
We likely work in very different company-structural worlds. I have no dog in the part-cost vs. fitting fight (well, maybe a zero-thickness dog, but I still keep him leashed and muzzled). My job in that area is done when I submit the design summary showing more-of-this-means-less-of-that. Sometimes I even submit alternative drawings for different costing/resource planning models, and the decisions in those areas get made after I’ve closed out the project.
They are fully avoidable human errors. The typical one is when a designer adds a bunch of “+0.1” and “-0.1” tolerances in drafting in order to avoid having to do model tweaks… everything goes fine for awhile because it’s all been NCd to middle of tolerance anyway, but for whatever reason something eventually comes out at limit, and doesn’t fit anymore because the stack calculation (if done at all) contained a sign error or such. Of course, the original designer has moved on or retired by then, so no one quite knows where to start looking. Sure, tough beans and no excuses, but clients are grateful when those of us who have foresight, cushion them against such eventualities. Back in the days when CAM wasn’t a given, we always dimensioned the primary NC-coordinate view with origin at the upper right corner/int, so that all coordinates were negative-signed. It was appreciated and the good word got passed on to management, designer gets on the short-list for the next gig, win-win.
So we’ll have to agree to disagree on the general acceptability of one-sided tolerancing in the modern age. Ok, I didn’t think about the times I use those clean round numbers (basically to avoid drafting messiness on fits) when I made that statement, but in general, one-sided tolerancing only adds risks because it circumvents the model, and the default attitude should thus be to question it where it is seen. Not forbid it, but do question it.
Plus (and this was actually the main point): I think it should be an imperative to deliver a 3-D reference model with the “real” dimensions (how can these ever be “incorrect”?), so that downstream designers immediately see the true airgaps and intended interference fits, and I have never experienced a CAM programmer not appreciating a fully middle-of-tolerance model. Tool radius correction is fine on an isolated feature, but model contours having varying tolerance weighting along their runs are an unkindness.
I think that how one views a comparison of an ISO fit with an overridden dimension could be a matter of degree. If a colleague gave me a drawing with a Ø5a9 shaft spec on it, I’d send it back and say please model that true. Or if you like: what is “most correct,” 5a9, 4.8c9 or 4.7k9? Why then not 4.715js9? (These identical-but-different expressions all actually did imply discrete things to the dinosaur craftsfolk of yesteryear, but it’s easily been 10 years since I’ve met a designer or shop person who knew what those would have been)
I’m not going to respond line to line here but suffice it to say that there is no such thing as a hard and fast rule. If you’re in an industry that for some reason unilateral dimensioning is never the best design option, then never use it.
I can say without hesitation that I have run into many applications and many reasons to use unilateral tolerancing over the years.
You talk about stack ups. I simply have to disagree. I’ve checked a lot of designs over the years and I find it WAY easier to add up a bunch of round even numbers and then deal with unilateral tolerancing than to add up a bunch of odd ball numbers and then deal with the same tolerance bands in a different place.
ISO tolerances are based on base numbers typically to get a certain fit. They are set up this way so at a glance you can have an idea of what the design intent is. Moving the nominal to shy away from a +/+ or -/- tolerancing completely defeats the entire purpose of the entire practice.
Manufacturing should not dictate how something should be designed. If I designed everything the way manufacturing wanted it to make it “Easy on manufacturing” I’d end up with a seriously degraded design. There is a big difference between “doing something stupid that makes it more difficult for manufacturing” and “Designing something correctly that is hard to manufacture”. In cases where the better design is to have unilateral tolerance, that is the way it should be designed regardless of if it makes it “Harder on manufacturing”
I’ve seen WAY to many cases where designs were compromised to the point of being worthless because “Well it’s easier if you dimension it this way for purchasing” “Oh but it should be dimensioned this way to make it easier on the welding department”, “Oh and dimensioned this way for machining”, " and this way for quality". Sure manufacturing may always prefer a nominal model, but of that is not the proper way to relay design intent…to bad.
This is related to the asymmetric tolerances discussions. I have been designing a lot of plastic parts lately. They build the tool off the model, so it should be modeled to what you want. Reality, is that sometimes the part off the tool ends up outside the tolerances but it can still work. (Sometimes it was something that could have been wider tolerances to start, sometimes the mating part can compensate. Sometimes, it is accepting a cosmetic issue where the part edges don’t line up as well, but the issue is accepted rather than taking the time to fix the tool. Schedule being the most important thing for the project at that time.) I have widened my tolerances so that parts off the tool would not be rejected because they were outside tolerances, but if the tool gets rebuilt from the model, it will be at what the nominal was supposed to be.
That can be a good practice, but my argument is that if the part is designed and modeled right on the dimensions etc, then it’s up to the machine operator or fabricator to understand their limits, you can open a pretty large if manufacturing personnel changes and the new guy does it differently.
Pretty much the same thing here, we always modeled the part right on and then the shop knew what they needed to do to match the tolerances etc, since we were bought by Wyrmwood and parts started to come from their facility to ours for final finish and assembly, the parts came here way out of tolerance, now they want drawings for every step of the way, min/max on the raw material, min/max off the machines etc, this just again opens up a bigger - Understand the manufacturing process surely helps.
It is pretty easy to get the first steps taken care of using Express software already available in SOLIDWORKS.
DFMXpress will look at a few common parameters for errors directly in the UI, so the engineer can check hole diameter/depth ratio easily - or holes in a sheet metal part/distance to edge ratio.
If this works as a start, then DFM has a pro solution with a LOT more settings - available for different CAD systems as well.
For modelling the parts to mean dimensions - don’t…
Just use SOLIDWORKS CAM MBD and let the CAM software read the tolerance, and machine to the mean automatically.
So we have two pieces of software taking care of everything discussed here, and they both automate the cumbersome processes.
I still very much agree that part of the education to take on a CAD design job, is 3 months running jobs in the machine shop, to understand WHY a 10xDiameter hole could be expensive, and WHY we do not need extreme geometric tolerances to make the part LOOK good.
That would be cool. I always like to see what other people are doing. I can probably find some video’s of machines we’ve built of which we machine most of the parts for. I’ll have to walk around and see if we have anything interesting on any of the machines or in inspection.
if manufacturing personnel changes and the new guy does it differently.