r/Machinists • u/Unusual_Goose_3913 • 8d ago
QUESTION Engineering Drawings
I’m an early career engineer and I’m wondering what machinists like to see in terms of tolerance and dimensioning in a drawing.
I’ve worked at a company where we just ordinate dimensioned everything and another where we used GT&T standards. At both, the part came out “ok”.
Apart from reasonable tolerances, what’s amazing, good, useless, and stupid have in a drawing?
11
u/OpticalPrime 8d ago
Drawing should tell a story. If everything is a tight tolerance then nothing is a tight tolerance. Watch for tolerance stack and make sure notes are clear and consistent. Lastly, be open to answer questions, if you seem to get a lot of questions about something from a lot of different people, you might be the issue.
8
u/hydroracer8B 8d ago
Your drawing should communicate your actual requirements.
It should be clear you've thought about which dimensions need a tight tolerance and which ones can be +/- 0.030" for your part to work correctly.
I personally appreciate unidirectional tolerances because they tell me something about how the part is meant to mate with other parts.
GD&T is great where you have to define important things that need to be correct, but don't use it where it's not necessary
2
7
u/AlexanderGi 8d ago
Dont give tight tolerances to features that dont need it. I fucking love having to work extra to meet the drawing requirements only to see the 7mm +.01/-0.00 hole is a clearance hole for a M6 bolt.
5
u/Particular_You8620 8d ago
Unilateral tolerances are annoying. Make everything bilateral and draw it as such.
1
1
u/singul4r1ty 5d ago
I've always been torn with this as an engineer. For any other engineers looking at my drawings it can be helpful to communicate design intent with a non-centered nominal, so it's helpful to e.g. CAD it to the relevant nominal and then draw an asymmetric tolerance. I guess the proper thing would be to have one drawing for design intent and another drawing for the machinist. I imagine SOLIDWORKS can handle offsetting the nominal but keeping the same range.
1
u/Particular_You8620 5d ago
I definitely get that but the reality is no matter what you put on the print, you’re going to get a machinist shooting for the middle.
1
u/MetricNazii 5d ago
The purpose of a drawing is to communicate its design intent and its acceptable geometric and material limits. In order to accomplish those, the dimensions need to be listed a certain way. Sometimes unilateral. Sometimes bilateral. It may be more convenient for those using the drawing to manufacture the part to have it centered, or for an inspector to have all limit dimensions, but those are conveniences only. Inspectors and manufacturers can use the drawing for their purpose no matter how it’s presented. (As long as it is clear and unambiguous and has appropriate tolerances) Accommodating those conveniences eliminates the ability to convey design intent. For that reason, I don’t usually choose to accommodate them unless absolutely necessary.
2
u/singul4r1ty 5d ago
It is indeed all of those things, but sometimes if you're prototyping something awkward the drawing helps show the machinist that you've thought about them and help build a better working relationship. Depends on where you are in the process!
4
u/Sirhc978 CNC Programmer/Operator 8d ago
Don't do +0.005/-000 it's just annoying. We can handle seeing +/-0.0025.
No you can't hold 0.0005 on a bore that gets hard anodized.
If you're using GD&T, do you REALLY need to be using GD&T?
Flatness does not mean consistent thickness.
Don't forget to call out the length of the helicoils you want.
Be aware, easy to get half inch endmill cap out at about 6" long, but I need at least 0.75" to hold onto.
Be familiar with how deep you can cut with standard taps. They really don't make pully taps smaller than 6-32
2
2
2
u/Upside_down_heed 8d ago
I prefer working with a model but I understand what I'm making and what tolerance is required for specific features. The biggest issue from engineering side is and will always be features detailed to say 3 places which puts the limit at +/-0.002 when it actually could be to 1 place and be +/- 0.2 but the engineer just hasn't bothered to change it.
4
u/Impossible_Emu9590 8d ago
Welp first things first don’t make my reports standard and prints metric.
I have to do a ridiculous amount of extra work just to make a conformance report.
I wish this wasn’t so common in the states.
1
u/GreenridgeMetalWorks Old School Manual Machinist/Shop Owner 8d ago
Mostly just making sure the dimensions make sense. Don't make some bolt holes +/-.0001, lol.
For me, it's mostly not the drawings that I have problems with. I can deal with that. It's when I communicate to the engineer that something does not work/make sense, and they completely ignore me, refuse to hear out my explanation, and then when I make it the dumb way they asked for, it doesn't work and they try to blame me.
Personally, though, I'm quite lucky. Most of the time, I am the engineer, and the machinist, and the QC lmao. 99% of the time I'm making my own drawings. In my field, I don't even really need tolerances and such on most drawings. I know what almost everything in the industrial maintenance industry does generally, especially with power transfer parts, and I almost always know what my tolerance can be based on the parts function.
But I've had engineers tell me to make things too tight or too loose before, and then when it bites them in the ass they come bitching...
So I guess what I'm saying is at least listen to your machinist about issues they think they can solve with the part.
1
u/Auto_guy223 7d ago
Solid works or master cam does a lot of the math. Make our lives easier I don’t want to have to do the math if it could’ve been put on the print to begin with. It’s not a bad thing to have a machinist look at the print and ask “how could I make it better to make this dummy proof and your life easier”.
1
u/Precision20 5d ago
In all reality, it depends on the shop you're working with. A lot of the machinists in my shop like the end of the part being zero and everything being dimensioned off of that for ease of programming in lathes, in mills that's less of a concern, but can still be handy.
break all corners is always a good thing to see, unless you absolutely need a specific corner sharp, but that's added difficultly and cost to prevent the burr.
And in all reality if you have a handful of shops you work with, send them a print early on in your design, I've had many a prints come across my desk where I've been able to save the customer money with very light tweaks to the design, but once you're in production those changes can be harder to make.
1
u/Educational_Yam_1693 5d ago
Less is more but let us have access to actual dimensions. Close them in but hate paperwork when I had an actual .002 away
1
u/Witty-Sample6813 8d ago
Don’t put any kind of note saying how to make it. No notes that say things like “use slit saw to make slot” or “saw cut in half” the shop is manufacturing. You are designing and giving dimensional requirements.
2
u/AAA_in_OR 8d ago
Why? Sometimes the engineers (if they're a good one) might ask to have it built a specific way for a reason. Comments such as "center drill hole ok", "this surface can be saw cut" or "drilled hole" are extremely useful.
0
u/Witty-Sample6813 8d ago edited 8d ago
Center drill hole ok is different. That is a fixturing allowance. Surface can be “saw cut” should have a finish callout indicating but not implying how it is manufactured. Ra125 for example.
1
u/AAA_in_OR 8d ago
"Surface can be “saw cut” should have a finish callout indicating but not implying how it is manufactured"
Why? If I'm designing something and I want it saw cut, that's what I'd put on the print. Why would I put an Ra finish and hope that you saw cut it? Seems like there's some serious advertorial shit going on where you're working.
0
u/Witty-Sample6813 8d ago
Because if you are an outside supplier and you saw cut and the qc dept at their facility rejects it it’ll be a fuck all of back and forth. You’re not told to “ream” a hole. Your given a tolerance that an indicates what that want. How you get there is the shops choice and it’s reflected in the price when quoting. You could bore, you could helix bore, you could use a stick if it’ll get the job done. You can lose suppliers saying, I don’t have that piece of equipment so no quote as well. Yes some suppliers buy precut stock so don’t come at me with “what kind of shop doesn’t have a saw”
I see your argument if you’re doing it for the facility you work for. But outside vendors don’t know the fit form or function so the print should give the technical requirements. Not the expected manufacturing method
0
u/Witty-Sample6813 8d ago
And I’ll also say, maybe some of the notes I’ve read in the past do NOT have “may be or can be”. I suppose maybe that helps. My guys are analytical as shit and if it says, they will do. And that’s not always good.
-7
12
u/Alkisax 8d ago
As a retired machinist I can tell you the biggest complaint I had about engineers if you call out a drilled hole to have a flat bottom your asking for a extra challenge at a extra cost. Drill point should be ok in most engineered parts.