You model "exact". If it's 10 inches that's how you model it. Mathematical exactness isn't possible in the real world, but it is on the computer. If you model in error you negate most of the benefits of solid modeling.
Tolerances are expressed as part of the manufacturing processes to convey what's "possible", or what you can live with without violating the intended function.
"Bryan Bruder" wrote in news:z9zid.359844$ snipped-for-privacy@twister.nyroc.rr.com:
A series of "best practice" type stuff, some of which is articulated, some is not. Things such as model for symmetry, make holes and fillets as separate features rather than sketched into extruded features, cosmetic fillets last, fully define all sketches except spline sketches, Most of this is impossible to really enforce unless you have a lot of extra time on your hands to check models the way people used to check drawings. The key is to hire people you can trust to do their jobs, educate them, and then let them do it.
No. When designing plastic parts I try to design "steel safe", so that changes to the mold remove rather than add material from the mold (add rather than remove material from the part).
I model to nominal, and tolerance for manufacturing.
Depends on if it's a press fit,what I want to do with interference detection and the manufacturing method. If it will be manufactured from a paper drawing, that's one thing. If it will be machined directly from my model, that's something else. Still, overall, I model to what I wish it to be in an ideal no-tolerance world. Inspection drawings give tolerances.
Because of statistical distribution curves, it makes most sense to use symmetric tolerances. The guy at the machine is going to aim for a number, and could miss to one side or the other. No one aims for one extreme of a tolerance zone.
Do you not use any GD&T? I find it easier to reconcile the tolerances to the model if I use GD&T. So, really, I think you are asking the wrong questions.
Thanks these are exactly the opinions I want to hear.
But from a manufacturing point of view should we give the NC Programmer or Machinist using the model for tool paths something more than tolerances on a drawing? Maybe I should have called this modeling for rapid proto-typing standard. That is why I asked about MMC for tight tolerance dimensions and exact (nominal) for looser sizes.
I do NC programming directly from the solid model every day. In my situation, I always know the function of the machined features. many times, they are my own designs.
I don't know what "your" situation is, so it's hard to know how to answer. How involved is the shop with the engineering dept ? Do you typically ask their opinions on design for manufacturing issues ? Or do you throw the data over a wall ?? Does the shop have Solidworks seats, or do they usually end up working with a dumb imported solid ?
If they have Solidworks, you can apply tolerances directly to the driving dims. and they're available with a simple click. If they have to work with dumb solids, you have to provide supplemental data regarding tolerancing. That is, unless, you work closely enough that they already know what's required.
I will usually model things exactly as they will be machined. That is, if I have a hole that's a tight running fit for a .2500 shaft, I model the hole at .2510. This is also a standard reamer size. For tapped holes, I model the minor diameter. Our guys know when they see a .159 hole that it's a 10-32.
Geometric dimensioning and tolerancing is used mainly by aerospace, automotive, and defence. The reason for it, in these industries, is that parts are made by different companies all over the world. You have to have a consistent standard or things won't fit. It's a bit of an overkill for a companies internal use. In these cases, it's far more important (and cheaper) that you just understand each other.
You made some mention of geometric tolerancing for 3D models. ANSI has come up with a standard for that (can't remember the number, but we just bought the book). As it stands now, that's all it is, a book. The utimate purpose, as I understand it, is that this data will be included in a future STEP specification. Several things have to happen before it becomes usable. The specification has to be finished, and software has to be updated to support it, in both directions. As far as I know, only Unigraphics supports it now, and that only in a developmental role.
I model to "nominal" and then tolerance for a serviceable part. I think that's where tolerancing goes to hell for people. You need to understand how the part is to be used and tolerance for a usable part. The tolerances then would dictate how it is actually manufactured. Any way, that's just my opinion
I believe that there are addins that help you evaluate tolerances. I feel the proper way would be to model to nominal and then add tolerance to your feature dims. You could then use a tolerance analysis program which should show the results of combining different extremes.
Always a good point to keep in mind when possible.
BIG Ditto
Not always true - The aluminum extruder we have been dealing with always shoots for the bleeding edge of the tolerance we give him. This is to extend tool life. As the tool wears, the parts get bigger/walls get fatter. If he shoots for the middle fo the tolerance range it cuts the expected tool life in half. Not that I liked it -I gave him nominals that I wanted them to shoot for on the tool (+.003, -.012) and he disregarded them and went for the exact outer limits.
Except in the case of some hole sizes when I know the process to be used to create the hole, I invariably model to the size I want and avoid with a vengence the +.000/-.010 thing. Nobody in fabrication will try to make it near the .000, they will try to make it -.005
People who build things are not relly too interested in our design intent. They don't care and won't be graded on what put when using unilateral tolerances. Obviously this is never a problem when using bilateral tolerances. But when one uses unilateral tolerances, particularly on a linear dimension, and then makes the geometry "nominal" one introduces a disparity between model and what fabricator will make. I would suspect that the awareness of the personnel and the situation might get a good result, but generally, machinists are not concerned at all about +.005/-.000 - All that they will do is make the part .0025 off nominal or at lest try to. Let's not even get into SPC during a run if they go for the -.000 side of things, the guard band gets tight. Machinists shoot for the center of the road, and so should your model . . .
. . . Unless you don't mind designing one thing and building something geometrically different.
Also, the +.000/-.010 thing is a real nuisance if anyone is using your model to program using CNC since it can shift your whole point of reference. If they are not using your model and redrawing it based on unilateral tolerances (shame on them) then often times they will not be able to solve the geoemtry in the same way that you originally created it.
Hence: .5000 +-.010 -> Tells a fabricator to make it .5000 .4950/.5000 -> Yields a likely .4975
10.00 +.015/-.000 -> Gets you 10.0075 .5000/.5005 -> Gives .50025
10.00" +- .010 -> Gives you 10.00
Oh and I always draw turned parts as if they were in a lathe chuck and try to dimension them from the exposed end if possible . . .
Hole sizes are controlled by the tools chosen, mostly. Their centerpoint *in the model* controls their location. It's possible for an API program to read the geometry and select tools in some cases. Depends on many factors.
Surfaces, if using *your* CAD model, control the CNC programs. To the model. Don't make the programmers doubt your geometry or force them to remodel the entire (or even part of it) thing because your model cannot be trusted to be the nominal model with symmetric bilateral tolerances.
Once bitten you will never be trusted again. Nor will your firm. That adds much cost & risk.
Be very clear how you modeled things. Communicate this quite well to all,
Never allow any dimensional data thet does not fully & accurately represent the 3D model geometry. That's your product, not a
2D sheet of paper. Or it should be; the print just for annotations not otherwise well conveyed.
IF you & the shop making things are close you *may* be able to model some well-defined & known things at the minimum material condition .... as tools wear things get bigger (surfaces, holes may be a different matter) so if all the tolerance *in such cases* is on the +material side it may aid in manufacturing. But such must be clearly understood and agreed to by all involved in advance.
I have also had the fortunate scenario of designing what I programmed and building what I designed. So much can be gained if you can reduce the loss given to each interface between processes. The worst case is when there are too many interfaces and everyone has to duplicate things and nobody really understand the context for the geometry. Things descend into a "legal" type of "this is what you asked for" - this is all too common when people only do "my job" and don't know the reasons behind what they are producing. But, this is the way the world works and needs to work, particulary when things are massed produced.
Another neat thing that I have done in the past with single units is to design something, build a functional unit, tweak the design to what was built (yes sometimes even to inconsequential errors) and get on with life with the "corrected" design. This usually only works for single piece items, more like toolmaking. I have taken advantage of the SolidWorks parametrics to do this sort of backwards designing and it is the best thing on earth. Like when I square a block .030 under for whatever reason, I just throw new numbers at the design and things update, leaving me with a coherent model.
Thanks for the information on ASME Y14.41-2003, we just purchased the book.
The part that addresses what I was asking states:
Design models represent ideal geometric constructs; that is, perfect dimensionality and shape of the part geometry are assumed. Parts shall be modeled at a specified dimensional condition, for example minimum, maximum, or mean. The dimensional condition shall be specified as a general note..
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.