What possible use is this?

[Ankana]

If I make a feature, say a ,1875in cube. and I "show dimensions" and because of manufacturing considerations I decide to change that .1875 to two a place decimal. Now my "nominal" dimension IN THE MODEL is .19. What possible use is this? Pro-E has more poorly thought out practices than any software I have ever encountered. I suppose the answer is to NEVER "show dimensions" Which is how PTC will tell you it should be done. This is just ONE of many examples of how Pro-E fails to meet expectations. How about that hole wizard!

What a P.O.S.

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[ehill]

Pro/E did exactly what you told it to do - change the accuracy of the
driving dimension to 2 places. If you want 4-place decimal accuracy,
then you need to leave the driving dimension at 4 places.



If you want to keep nominal model dimensions at their full accuracy but
show a less-accurate dimension in the drawing, then you need to create
the dimension in the drawing instead of showing the driving dimension.



Best Regards,

[tgiauque]

Um, the alternative is that you change the dimension to two places, it gets rounded off to .19 on the drawing, and the value of the dimension in the model is still .1875? So now you have a model and a drawing that don't match. Is that what you want? Which one is the "real" dimension? What do you tell your machinist who comes to you complaining that the model and drawing are different?

PTC stands for "Parametric Technology Corporation." That word "Parametric" means something important - go look it up.

[gchampoux]

I won't attempt to tell anyone why my preferred way is better than theirs.

But I do have a beef with PTC on 2 counts:

1) This behavior has changed.In older releases, Pro/E would not change the nominal when the number of decimal places changed.

2) This does not need to be a single solution situation. PTC should implement a config option to control the behavior, and allow the user to do what he/she wants, and accept the consequences thereof.

[dgschaefer]

Actually, the reality here is that this is very well thought out, you
simply don't understand it.

The software is designed to show the model dims and to have the part
model and the drawing model match. Therefore, not only will changes to
the part be reflected on the drawing, changes to part specs in the
drawing will be reflected in the part. After all, you didn't merely
change the drawing, you changed a part specification and the model
reflected that.

The drawing calls for a spec of .19, Pro|E has changed the model to
match. In your mind, 0.19 = 0.1875 = 3/16, but that's not really true
is it?

The 2 place decimal has some rather loose tolerances associated with it,
likely +/- 0.01. So, your drawing spec is that this dim can be .18-.20.
A 4 place decimal would likely have a vey tight default tolerance of
+/-0.0005 or so, meaning the dim can be 0.1870-0.1880. Very different.

As has been stated, there is a way to accomplish what you want, you just
need to understand what the software is trying to accomplish.

Doug Schaefer

[dgschaefer]

Gerry,

I've worked with Pro|E for 12 years back to Rev. 16 and I believe that
it's always worked that way.

Also, I believe there may be a config option to change that behavior,
I'm not really sure, but I seem to remember one.

Lastly, the use of created dims instead of shown will accomplish what he
wants.

Doug Schaefer

[Ankana]

I guess my point is that I can NEVER use "show dimensions" which is THE only fast way that I can populate the drawing quickly with dimensions. You can't see a problem with my designing a feature to be 5/32 long and wanting to indicate a two place decimal on the document I describe the part to a machinist.I donot want the damn thing to CHANGE my model from .15625 to.16. I'm notwanting to changethe nominal that I designed the feature. I just want the machinist to bid me a two place decimal instead of the accuracy the is associated with a five place decimal. If my machinist is using the model to create the part. I wantthe modelto BE 5/32 (.15625) and not .16.

Let's take it to an extreme, if I build a feature that is 1.625 and I round it to no decimals I'll have a two inch feature. You can't see a potential problem here that is completly avoidable?

Why round off a decimal in a model. That should ALWAYS have the highest accuacy that I MODEL it with regaurdless of what the drawing says.

Again, I ask; What possible use is this?

[Ankana]

I do understand what is hapening, I just don't see where it will be of any use. It seems that "show dimensions" should seldom be used and that is the only way that PTC has provided for us to quickly populate a drawing with dimensions. Because of how the software treats this problem, it takes away that tool altogether.

[kbryant]

Actually, Pro/E has ALWAYS changed the nominal dimension when the decimal
places changed.

<putting on=" my=" old=" geezer's=" hat=">

At the second PRO/USER conference (That's what it was before it became
PTC/USER) in 1991, I presented a paper on the topic of Production Drawings
with Pro/DETAIL & DRAFT. In that I discussed the implications of tolerances
& decimal places in drawings. The next day, we had a general session & a
long discussion of the implications of the decimal place issue. We had
people on both sides of the issue, but the bottom line was that the part &
drawing MUST match for it to be considered parametrically accurate.
Otherwise, which dimension is correct?

<removing my=" old=" geezer's=" hat=">



Thanks,

Kelly

[cfly]

Why would anyone round 1.625 to no decimal places? Rounding off a decimal
place or two is no big deal when you're left with thousandths or ten
thousandths, but the only time anyone would consider rounding to no decimal
places, thus making the accuracy one inch or more, is if the part were tens
of feet long. Your example is ridiculous.

[StephenW]

Now I think you are getting to the meat of it. It's really a tolerancing issue and not a software issue, at least that is what I see. You are trying to make the tool fit your standard tolerancing. I think that pro/e is doing the right thing based on your 1.625 dim rounded to 0 places. If the drawing says 2", then I want the model to say 2".

My solution would be to .1875±.03 (or .0300) whatever tolerance you desire. I want my nominal dimension to be machined to the number I want and then let the tolerance stretch across that.

Most of the time in this case, I just let pro/e round the number in the model too and I just make sure everything still fits like it supposed to. Usually it is in loose tolerance areas when situations come up like this anyway.

[RichSerafin]

Rich,

So you get exactly what you asked for. Why have a vendor quote on a part with 2 decimal place accuracy when you really want 3 place accuracy? What purpose does that serve?The vendors we work withneed to requote the job when you tellthem everything needs to be 3 place accuracy when the original quote was 2 place accuracy.

Rich Serafin

[BrianTaylor]

I have used shown dimensions since I got on this tool rev 17. I would
highly debate the fact with you that they should never be used. We are
moving for a paper society to a paperless model driven approach like it or
not (personally I like drawings). The model and drawing must match that
is how it has to be.

Brian L. Taylor
Sr. Draft/Design Engineer II
Mechanical Design Analysis Documentation Dept.
Raytheon Missile Systems
1151 E Hermans Road
Tucson, Arizona 85706
(520)545-9730
-

[Ankana]

Instead of discussing the issue, you attack my "EXTREME" example? Of course I would never round that number to zero place decimal. that was NOT the point!

[mpeterson]

Then design your part to the nominal as you prefer and
then add the desired tolerance in the drawing to the dimension instead
of taking the default per the number of decimal places. This might take
a little longer, but the design intent is in the model and the
machinist gets the correct nominal dimension with allowable tolerance.
Thus you can also use the shown dimensions too. By the way, go back and
use version 2000i like I am stuck with currently and see how long it
takes to dimension a drawing!!!!!! - View/Move View/Select View . . .
Modify/Any Item/Edit Text/ Select Text . . . etc, etc, etc

Mark A. Peterson
Design Engineer
Ramteq

[cfly]

Actually, your outrageous example drives home our point - if you model a
1.625" part and round the dimension to no decimal places on the drawing,
you're going to end up getting a 2" part from the shop, and it won't even
come close to matching your model. The dimensions drive the model, so if the
dimension value is changed, the model will change along with it. If you
don't want the same accuracy in your model as your drawing, you have no
choice but to use created dimensions. And yes, that does slow the process
down.

_____


Why would anyone round 1.625 to no decimal places? Rounding off a decimal
place or two is no big deal when you're left with thousandths or ten
thousandths, but the only time anyone would consider rounding to no decimal
places, thus making the accuracy one inch or more, is if the part were tens
of feet long. Your example is ridiculous.

[TimMcLellan]

Or worse. the manufacture machines the part based on the drawing/quote and
you expected them to manufacture it the model's nominal values. Are your
tolerance stack ups based on the print or the model?



Hmm.may be manufacturing some expensive paperweights.



Tim McLellan
Mobius Innovation and Development, Inc.

[Ankana]

Point taken.

I suppose there are some considerations that I had not taken into account.

Thanks for your comments

[gwalker]

I believe part of the problem we are discussing here is a fractional mindset in a decimal world (we have it where I work also). We want our parts modeled to a fractional size and dimensioned and tolerance in decimal. If you keep the model at 1.1875 and dimension the drawing to 1.19 +/- .030, the nominal is no longer centered on your desired target.

If you want to make parts from decimal dimensioned drawings, model your parts with decimal dimensions. Forget that fractions exist.

[ptc-593619]

Of course, you could always use the @O and make the dimension anything
you wanted to!

As for nominals; I once argued with an old timer that my 1 inch plus or
minus 0.25 was better than his 0.95 plus 0.3 minus 0.2, they're both two
place decimals and give the same result so why do we tend to the "pure"
number?



Richard A. Black

Lead Engineer

Eaton Corporation

16900 Aberdeen Road

Laurinburg, NC. 28353

[pfadams]

As the designer/engineer/draftsman it is your responsibility to tell
exactly what you want and the machinist should give that to you.
So if you want 1.1875" +.001-.001 tell him that and tell the program
that. If you want 1.1875 don't ask for a 2 place decimal because it can
only
be close not exact. Say what you mean and mean what you say.
To put it a little more harsh screw the computer and use your head
first. If the computer doesn't follow train it like a nasty dog and beat
it
with a stick.
phew now I feel better........................

[cfly]

But you can only do that with created dimensions.

[ehill]

It seems to me that the real problem here is trying to make a decimal dimension fit into a fractional way of thinking. If you are thinking something will be 3/16 thick, when you make this into an *exact decimal dimension* you get .1875 thick. If you then move forward thinking you want two *decimal place* accuracy shown in the drawing, you need to take a step back and realize you only actually wanted your dimension to be .19, which is a *realistic decimal representation* of 3/16. If you stop thinking in 16ths and start thinking in hundredths of an inch then this isn't an issue any longer.



If you want to think in unrounded exact fractions, use fractional dimensions and then deal with the aftermath of fractional tolerances 😄



How many users that are standardized on the metric system have an issue with the way dimensions are rounded or represented? I am guessing zero.



Best Regards,

[dgschaefer]

I can see your point, however I still think that you are asking your
machinist to read your mind.

Take your 5/32 example. What's your 2 place decimal's tolerance? Here
it's +/- 0.010". So, if my drawing says 0.16, a part of 0.17" is
acceptable. However, if what you really want is 5/32" +/- 0.01", then
0.17" is out of tolerance, the max being 0.16625".

You need to communicate to the shop what you want. Rounding dims to a
certain number of places is an expedient to allow a range of tolerances,
however it has consequences, namely it skews the nominal and therefore
the tolerance range. This was no different in the days of pencil on
velum. The only difference is that Pro|E shows you the consequences in
the part model.

I've been in your shoes before. I've ranted to the group that Pro|E
absolutely shouldn't work this way, it makes no sense! And the
community came back and basically said "Uh, yeah, it should." After
cooling down, many times I came to understand the thinking behind it.

The bottom line is now you know how the tool (Pro|E) works, now you have
to decide how you are going to use it.

Doug Schaefer

[ptc-593619]

Here's an idea - what if we all went metric? Wait, I think we've tried
that before!



Richard A. Black

Lead Engineer

Eaton Corporation

16900 Aberdeen Road

Laurinburg, NC. 28353

[ptc-726111]

I have had similar concerns in the past, and have used this method as a work

[SteveFowler]

We have been going metric one inch at a time for almost 15 years now.

Steve

WF-2 M080 FlexC

Win XP SP-2

Dell PWS 690 3GB Ram

Nvidia Quadro FX4600

[dgschaefer]

Rich,

Thanks for stirring up the pot a little. We haven't had one of these in
a while. 😄

Hey - tomorrow's Friday, who's up for a old fashioned shown vs. created
debate or Pro|E vs. SW? 😛

(Note: I am kidding.)

Doug Schaefer

[rreifsnyder]

Showing dimensions is a huge waste of time. Try creating your
dimensions. It takes far more time to redefine your sketches to end up
with the dimension you want to show, than it does to just create that
dimension in the drawing. Please don't try to tell me about design
intent in the model. A huge majority of the time, STEP or IGES files are
what is used in CAM programs. These don't translate the dimensions as
they were created, only the end geometry. Inspection using the "smart"
model requires the inspector to have the Pro/E model up, and dig through
looking for inspection dimensions. That just isn't going to happen
efficiently. There are some scanning solutions, but they are not in wide
usage.



I also have some concerns about errors that could occur with careless
use of all shown dimensions. When PTC removed redefining Scheme from the
feature redefine it allows the sketch to change while I'm trying to get
dimensions I want to show. It would be easy enough for someone to miss
the fact that the geometry changed. My other concern has to do with this
rounding issue. I understand why PTC has it behaving the way it does,
but it doesn't eliminate my concern. If I have a pattern of threaded
holes, and in making the drawing, the precision was changed to 2 place,
the holes may move. Even if I then change it back to 3 place, the holes
don't move back. The detailer may not know that the dimension was
supposed to be .1875, he will see it as .19 and it will change to .190
and if one of these holes needs to become a precision hole (a dowel or
locating sleeve, etc.) they dimension will be .1900 four place
precision, but a wrong dimension. You may call this far fetched, but
I've seen something similar happen. Drawings are still, and will
continue to be the best way to communicate certain things about a part.
The difference is that they can now be electronic (PDF).



Rob Reifsnyder

Mechanical Design Engineer/ Pro/E Librarian

L

Maritime Systems & Sensors (MS2)

497 Electronics Parkway

Liverpool, NY 13088

EP5-Quad2, Cube 281

[jflores-3]

Hey Rich,
Would you like some tea or coffee to go with all those lumps?
Seems to me like if you really want to show dimensions that are decimal equivalents of fractions but have a loose tolerance; you will need to give up the general tolerance block values.

Have you looked into showing your dimensions on the drawing with tolerance configuration turned on and using a region selectio to pick all the dimension you want to loosen the tolerance on verses the time you already investing to change the number of decimal places? May come out to be an even break.
later Jim