Modeling Standards Survey

What do most people do for solid modeling Standards?

Do you model to Maximum Material Condition?

If you model a part that is going to be 10.00" +- .010, what is the part
modeled size?

If you model a hole that is to be .5000/.5005, what is the modeled size?

If you model a part that has a length of 10.00 +.015/-.000, what will the
modeled size be?

If you model a shaft that is to be .4950/.5000, what would you model it at?

If you model a shaft that is to be .5000 +-.010, what is the part modeled
size?

Thanks for any input.

Bryan

 

Bryan,

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.


Regards

Mark

 

Just as MM's explain,toleraces let we konw what kind of part could be check
out as we can't let a part's dimension very accurent.Otherwise toleraces
express the relation of two part.As in solidworks,it stand for nothing but a
note.

 

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.

matt

 

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.

Thanks
Bryan

 

Bryan,

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.

Regards

Mark

 

Bryan,

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

Regards,
Al

 

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.

-=BAHR=-

 

Do you model to Maximum Material Condition?

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.

 

Hi Bryan,

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 . . .



Later,

SMA

 

IF you & the shop making things are close you *may* be able to

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.

Later-

SMA