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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[wattsteam]

ENOUGH ALREADY!

[ksauter]

Good point. I have run into MANY instances when the model had to be precise
in order to put features where they absolutely needed to be, but putting 3
or 4 place decimals on the drawing made no sense whatsoever. When I create
features that are built on dimensions used to create other features, I want
the features to STAY WHERE I PUT THEM!!! I don't want Proe moving them just
because I don't want to put a 3 or 4 digit precision dimension on the
drawing. All this stuff about making the part and the drawing match is fine
when you're working with ONLY ONE FEATURE, but when you have dependencies
and cumulative dimensions, this behaviour can bite you in the butt.

I'm with Rich on showing dimensions. I want to slap every dimension on the
drawing as quickly as possible, KNOW that they're accurate, and change
decimal places when and where I feel like it. I hate CAD programs that
think they can tell me how to design things. I'm the designer, not the
program. It should do what I tell it to and not argue about it.

Ken Sauter

[TerryJohnson]

Technically you are ALL WRONG - so there!

According to ASME 14.5 So everyone run and tell your checkers your
formats are Jacked up!!
(inches have been this way since I don't know when..
I have a copy of 1966 and it was that way)
Metric is covered in 2.3.1 and it is DIFFERENT in 2009 than 1982 & 1994
so HEADS UP for when you adopt 2009 your
METRIC TOLERANCES will also have to "agree"

2.3.2 Inch Tolerances
Where inch dimensions are used on the drawing, the
following apply:
(a) Where unilateral tolerancing is used and either
the plus or minus value is nil, its dimension shall be
expressed with the same number of decimal places, and
the appropriate plus or minus sign.
EXAMPLE:
.500 +.005/-.000 NOT .500+.005/0

(b) Where bilateral tolerancing is used, both the plus
and minus values and the dimension have the same
number of decimal places.
EXAMPLE:
.500±.005 NOT .50±.005


(c) Where limit dimensioning is used and either the
maximum or minimum value has digits following a decimal
point, the other value has zeros added for uniformity.

[ArnoldCollett]

You can go into your drawing options and set the "draw_models_read_only" option to "YES" and then you won't be able to change a shown dimension. Then if you want to have a dimension rounded to fewer decimal places, erase the shown dimension and create a dimension to replace it. This will allow you to use shown dimensions for some locations, unless you're wanting to change every one of them.

Arnold Collett

[kdemont]

I know that I should just "forget that fractions exist", and I have certainly tried, but I just can't seem to do it for long.

So I designwith myfractional thinking brain, tolerance as appropriate for manufacturing, then recheck my design and make changesif needed to insure the new nominal sizes that I have due to rounding still fit and mate throughout the assembly.

(I'm sooo old that I didn't need to go to college. I started out as a draftsman 30 years ago, and currently work as a mechanical designer. It is highly unlikely that I will ever be an engineer.For what it's worth,some of the best designers I ever met have been, and are, even older than I am now. I have also met some very talented engineers that are only a couple years older than my oldest daughter, and others that are as old as my father.)

[nuheht]

I have used Pro/E since release 9 (about 15 years) and have used shown dimensions for all but maybe a couple dozen dimensions without having any of the problems everyone is discussing on this post. The intent for having the ability to create a dimension was for the few times a dimension can not be shown, for example: certain types of advanced surface features you may have created. I run into more problems with drawings others have created with created dimensions that I would care to bring up at this time (it is almost a daily occurance!).



SHOW your dimension as a fraction with the drawing default tolerance for fractions being ±.02. You can also SHOW it as .2075/.1675, or SHOW it as .1875 ±.0200. All this can and should be done while creating the model so that a detailer does not "create" dimensions for you that does not meet your design intentions.



Joseph A. Ordo
Joe Ordo Engineering Services
2 Butternut Lane
Mechanicsburg, PA 17050

joe_ordo@msn.com

[merrill.rosenow]

In Reply to Tim Giauque:

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?

This isn't exactly the case. Rounding only brings the answer to the closest division you specify. Lets say to 1/100th (or two decimal places). Yes, the model and the drawing would be "different," but you are rounding within tolerances. It is illogical to specify a tolerance that is less than half of the resolution of what you are using to measure. ie: specifying a tolerance of +/- 0.0025 when the dimension is in terms of 0.00 as a number does not make sense.

[ptc-1932745]

The most straightforward solution I have seen for this is on aerospace
parts. The dimensions (if noted on the drawing) are all to 4 decimal
place inch units. The drawing notes that number of digits does not
imply a tolerance, and the overall tolerance is noted, along with the
individual tolerances as needed.



This also works well when full GD&T is applied, as most dimensions
describing features can be applied as basic, and a form tolerance
applied as needed.



Christopher Gosnell

TRIGON INC.
FPD Company
124 Hidden Valley Road
McMurray, PA 15317
PH: 724.941.5540
FX: 724.941.8322
www.fpdinc.com

[BobFrindt]

Hi Chris,
For what it is worth, we do not do our drawings that way because four
place decimals are considered to be more expensive to inspect even if they
have a large tolerance band.

The logic is this........
If your dimension is .1875-.3125 that is a huge tolerance band and would
be easy to hit, BUT the inspection equipment and gages must be able to
read to FIVE decimal places to determine if the .1875 or the .3125 has
been violated and if the part is scrap or not. If your inspection
equipment and gaging is only accurate to two decimal places, you may have
a part that is at .1877 and within the tolerance limits, but you cannot
prove it. So, if you can afford that large of a tolerance band, just make
it .19-.31, use three place inspection and be done with it.
Our Pro/E models and features are built to the number of places we show on
the drawing, so the drawing and model are consistent. If the design needs
.1875, I build it that way, If the design can stand .19, then that is what
it is.

My 2 cents

Bob Frindt
Sr. Designer
Parker Hannifin Corporation
Parker Aerospace
Gas Turbine Fuel Systems Division
9200 Tyler Boulevard
Mentor, OH 44060 USA
direct (440) 954-8159
cell: (216) 990-8711
fax: (440) 954-8111
-
www.parker.com



"Chris Gosnell" <->
04/24/2009 08:41 AM
Please respond to
"Chris Gosnell" <->


To
-
cc

Subject
[proecad] - RE: What possible use is this?






The most straightforward solution I have seen for this is on aerospace
parts. The dimensions (if noted on the drawing) are all to 4 decimal
place inch units. The drawing notes that number of digits does not imply
a tolerance, and the overall tolerance is noted, along with the individual
tolerances as needed.

This also works well when full GD&T is applied, as most dimensions
describing features can be applied as basic, and a form tolerance applied
as needed.

Christopher Gosnell

TRIGON INC.
FPD Company
124 Hidden Valley Road
McMurray, PA 15317
PH: 724.941.5540
FX: 724.941.8322
www.fpdinc.com

[ocorten-2]

To end the discussion (or perhaps fuel it again):

For what I have heard, WF5 will support independent control over numbers
of digits for shown dimensions.

[TracyWillis]

Rich,

Try using a limit dimension. Set the range and decimal places to
whatever you choose. A limit dimension circumvents any issues or
conflicts that you may have with your tolerance table. When there is a
range stated in the drawing the tolerance table does not apply to that
dimension. Your part will not change. You model it with the range you
want; pro/E will calculate the "nominal" dimension and that is what is
displayed and reported when measured. Created or shown dimension is you
choice; the bottom line is you really want to keep the model and the
drawing consistent. This way all persons quoting it or machining it
will all have the data set and will know the "actual" tolerance
regardless of whether they're looking at the model or the drawing.



Tracy Willis

Designer / Drafter



Cook Urological, Inc.

11OO West Morgan Street

Spencer, IN 47460

(812) 829-4891

(812) 829-1801 (fax)



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[jamesavisengine]

Why would you make a dimension two decimal places if you want them to make it to four? It sounds like you want the nominal to be .15625, but the tolerance to be looser and cheaper. You need a reference dimension to tell the machinist what to shoot for. This is a non-standard dimensioning practice, so it will take some extra effort on your part. To take advantage of ProE's shown dimensions, you should model as built and take tolerances into account. Regardless of if the dimension is on the drawing or the part, the tolerance is still there and you should model accordingly.

James




In Reply to Rich Petty:

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?

[dgallup]

You can have your cake & eat it too. Create a relation d=3/16. Then you can change the number of decimal places to whatever your heart desires & the nominal is still .1875. But for the love of god man, get rid of the inches!

In Reply to Rich Petty:

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.

[John.Pryal]

To answer your original post, i think it is possible to do what you describe, that is, round a driven dimension without actually changing its value. There is a config option default_dec_places, but it only works for newly created dimensions. Set this option to 2 places. Make your simple cube to your .1875" size, create a new drawing & show your annotation, they will display as .19, but will not have altered your nominal size of .1875

Hope this helps

John

[dschenken]

6 years too late.

[John.Pryal]

What can i say, i have been busy