Decimal Rounding

[krichardson]

A quick question; it is my assumption that Pro/E rounds a number ending in '5' (or more) up and ending in '4' (or less) down. Can any one confirm?

i.e:

.1285 rounds to 3 places .129, .1284 rounds to 3 places .128

And I know I can test, but this got thrown at me last minute. Thanks very much in advance!

[BenLoosli]

It is a little more complex.

The round is always to an even number. This statistically averages out the round-off error so things don't grow or shrink too much. It is covered in ANSI Z210.1 spec.


.1276 will round to .128
.1285 will round to .128
.1286 will round to .129
.1294 will round to .129
.1295 will round to .130

[BenLoosli]

After some testing, it seems that PTC does not follow the standard for rounding numbers and rounds a number whose last digit is 5 up and not to the even number. If you find your assemblies tight to fit together, this is why.

So, my list below becomes:
.1276 will round to .128
.1285 will round to .129
.1286 will round to .129
.1294 will round to .129
.1295 will round to .130

[ptc-936529]

You might want to know that the way it handles driving dimensions decimal places is now different with Creo than ever before. There is now a config setting that toggles whether the dimension and the model geometry rounds when decreasing the number of digits or only the dimension rounds but the model geometry does not. Yeh go ahead and read that last sentence again, I know this has been a hot topic for some time but as more companies embrace model centric designs and Step file fabrication, I will never understand why someone would want their model not to match dimensions. OK I'm off my soapbox. On top of that based on your config settings changes how pre Creo models come into the Creo environment.

So check out the knowledge base for round_displayed_dim_values

[BenLoosli]

The new CREO setting for rounding can be confusing. I also see cases where it can be used properly.

One case would be where you design a part that is say 13/16 (.8125 modeled) but you don't need that tight of a tolerance on the drawing, so you want 0.812 (OK, Pro/E will give you 0.813) to give you default tolerance of a 3 place dimension. Do you really want the model changed to 0.813? I don't.

It is something that we all need to adapt to moving forward. There have many parts scrapped because Pro/E has changed a model dimension from the drawing side because someone didn't do the full data checking that should have been done.

[GavinBRumble]

I agree with Ben...this is a great option. It allows us to design in
fractions (everything non-metric that you buy is), but display decimal dims
on the drawing (a lot of places prefer that) without causing your model to
"move". Before, you would have had to resort to CREATED dims to achieve
this...at the risk of re-igniting the SHOWN vs CREATED argument.



When surfaces and holes centers actually line up, it makes model/design
checking oh so much easier... J



Gavin B. Rumble, PE

Solid Engineering

336-224-2312

[JWayman]

It seems like it's a great option for US users, but nothing but a nuisance for the remainder of the world that designs in metric. Maybe there should be a US standard option for Pro/E (sorry Creo) and a base standard for the rest of us. That way, we wouldn't have to worry about whether the funny fractions options were set or not.
Just a thought...


Cheers,


John

[rreifsnyder]

Be aware that I am in the process of obtaining approval to send a file in to PTC with a fairly major bug that I think has to do with rounding shown dimensions. So far I have 2 examples where a hole pattern dimension (1 table pattern, 1 direction pattern) shows as a nice even number (5.000) but the real dim. in the pattern is 4.5625. If I look at the dimension properties and uncheck the rounded dimension box, the decimal places changes to 0, and the listed nominal goes to 5 and that is why I think it is related to the rounding. If I even just go to the dim. properties and don't change ANYTHING, the dim. changes color showing that it is changed and a subsequent regen will change the ACTUAL dim in the model to 5.000.

As I said, so far I have only found it in 2 instances and they were both patterns, but I WILL use it as more fuel to my fire that ALL dims on a drawing should be created rather than shown. I don't want the drawing changing my model.

Rob Reifsnyder
Mechanical Design Engineer/ Producibility Engineer / Components Engineer / Pro/E SME / Pro/E Librarian
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