topic Dimension Rounding in Creo 2 in 3D Part & Assembly Design

Dimension Rounding in Creo 2

davehaigh — Sun, 13 Dec 2020 03:17:55 GMT

I'm coming from Wildfire 4, so I guess I may have zoned out on previous discussions about this issue.I've played around a bit in Creo 2, I'm not sure I would call what I'm seeing an enhancement. We work on some highly accurate parts, it not uncommon to use 4 digits

Dimension Rounding in Creo 2

tcooper — Thu, 26 Oct 2017 20:57:01 GMT

Brings to question of what would the value be if you set the Dim Bounds
to Upper or Lower? I do stack up analysis this way, so wonder where the
boundaries will go.

Tim P. Cooper

Lead Designer

GE Oil & Gas

North American ATO

T +1 281 878 6168

M +1 281 796 9038

F +1 281 715 4116

- <">mailto:->

www.ge.com

Dimension Rounding in Creo 2

BenLoosli — Tue, 30 Oct 2012 21:20:25 GMT

It looks like it is doing what you are telling it to do.
Nominal value 3.9375 when displayed to 3 decimal places is 9.378.

What are you expecting to see?

Thank you,

Ben H. Loosli
USEC, INC.

Dimension Rounding in Creo 2

davehaigh — Tue, 30 Oct 2012 21:32:43 GMT

Looking though the config options I think these all apply. Not really sure what all of these mean. Anyone have real world examples for these?

Round_displayed_dim_values = yes*, no
Set the default status of the Round Displayed Value checkbox for new and newly shown dimensions.

Round_prewf5_displayed_dim_val = calculated*, round all, round none
Rounds the displayed value

Default_ang_dec_places = 1*
Sets the default number of decimal places (0-13) to which to round newly created angular dimensions. Unrounded angular dimensions automatically determine the number of decimal places required to display their stored value.

Default_dec_places = 3*
Sets the default number of decimal places (0-13) to which to round newly created dimensions. Unrounded dimensions automatically determine the number of decimal places required to display their stored value.

Default_dim_num_digits_changes = yes*, no
Sets the default number of digits displayed in a dimension to the last entered value. No - The system defaults to the value specified for the configuration file option default_dec_places.

Tol_num_digits_default_driven = yes*, no
Yes - The Default check boxes in the number of digits area of the Dimension Properties dialog will be checked when a dimension is created or first shown. No - the check boxes will be unchecked when a dimension is created or first shown.

David Haigh

Dimension Rounding in Creo 2

davehaigh — Tue, 30 Oct 2012 21:58:16 GMT

Found another config option

sketcher_strngthn_to_def_dec_pl = yes*, no
yes-Rounds<">http://localhost:60200/pma/sketcher/sketcher_strngthn_to_def_dec_pl.html?queryId=13ab3a8bcdd> off the values of new dimensions and of weak dimensions when they are converted to strong dimensions.
no-Does not round<">http://localhost:60200/pma/sketcher/sketcher_strngthn_to_def_dec_pl.html?queryId=13ab3a8bcdd> off the value of new dimensions and of weak dimensions when they are converted to strong dimensions.

David Haigh

Dimension Rounding in Creo 2

dgschaefer — Wed, 31 Oct 2012 12:56:33 GMT

It's rounding the value but not changing the nominal. This is a change
from long standing behavior in Pro/E. In the past, changing the number
of decimal places of a dimension actually changed the value. As a
comparison:

Past behavior:

Entered value - .28125

Rounded value - .3

Measured value - .3

New behavior:

Entered value - .28125

Rounded value - .3

Measured value - .28125

The idea in the past was that if are saying that you can allow the part
to be made at 0.3 +/- 0.1 (the likely tolerance on a 1 place dim), that
gives a different acceptable range (0.2-0.4) compared to a nominal value
of .28125 +/- 0.1 (0.18125 - 0.38125) and the model should reflect that.

Over the years, many wanted to simply round the display leaving the
nominal alone and didn't understand why their models were changing
simply by rounding dimensions. The default behavior was flipped,
starting I think in WF5.

--

Dimension Rounding in Creo 2

BenLoosli — Wed, 31 Oct 2012 13:50:58 GMT

The old behavior has also lead to many parts being scrapped in manufacturing by producing parts outside the limits of what the engineer envisioned.
The drawing display of decimal places should NEVER change the model.
If I want to change the modeled dimension, change the model itself. The drawing may not even change, depending on the round off selected.

Companies need to decide what is the master for dimensioning and manufacturing. It can be the model or the drawing, but NOT both!
At one of my prior companies, we made the model the master since manufacturing used the engineering models for all CNC operations.
This company and my last still use the drawing as the master for production.

Thank you,

Ben H. Loosli
USEC, INC.

Dimension Rounding in Creo 2

tcooper — Thu, 26 Oct 2017 20:57:30 GMT

When I pick the feature and then edit and it says the value is 3.0, and
I show the dimension of the feature on a drawing to place the dimension
and it says 3.0, yet when I measure the feature and it measures 3.04.
That is a problem!

Tim P. Cooper

Lead Designer

GE Oil & Gas

North American ATO

T +1 281 878 6168

M +1 281 796 9038

F +1 281 715 4116

- <">mailto:->

www.ge.com

Dimension Rounding in Creo 2

BenLoosli — Thu, 26 Oct 2017 20:57:36 GMT

That is a problem, but the original poster stated that when he edits the dimension in either sketcher or in the model, it shows the full 4 decimal places.
This is what it should show. The drawing display and the measured display are being rounded. They are DISPLAY values only.

Thank you,

Ben H. Loosli
USEC, INC.

From: Cooper, Tim P (GE Oil & Gas) [

Dimension Rounding in Creo 2

cpipe — Thu, 26 Oct 2017 20:57:38 GMT

Based on my experience, there are many cases from a tool manufacturing standpoint, where the rounding is beneficial when used with a tolerance block. For example, screw clearances are often fractional size drilled holes that can have a value of 3 or more decimal places. To keep the print clear these hole sizes are shown with 2 places to match the appropriate block tolerance, but the model should still reflect the fractional size hole so the machinist/programmer can easily select the correct tool. The print is then easy to scan for critical (usually toleranced dims) and non-critical (usually 1 or 2 place non-toleranced dims) features. If the print shows a 4 place dimension and a wide open tolerance, it is confusing and requires more time to interogate. And if the model shows a non-standard, 2 place, hole size, the cost could increase because the hole might be made with a more expensive process than needed (ie machined instead of drilled).

PTC gives you both options with checkbox and the default choice can be set with your config.pro per David's post:

Round_displayed_dim_values = yes*, no
Set the default status of the Round Displayed Value checkbox for new and newly shown dimensions.

Chris Pipe<">mailto:->
Eng. Sys. Analyst
trans-matic

From: Loosli, Ben H [

Dimension Rounding in Creo 2

tcooper — Thu, 26 Oct 2017 20:57:41 GMT

So you're saying the drawing or the model dimensions do not need to
reflect the geometry because they are for display purpose only? If so
what do I not understand about parametric concept between models,
drawings and geometry?

Yes if I pick on the dimension in the model to actually edit it, it
shows the 3.01. But when just picking the feature then edit to see the
dimension it shows 3.0. With your approach I need to pick the feature,
then edit then double click the dimension to see what the actual value
is!?

Tim P. Cooper

Lead Designer

GE Oil & Gas

North American ATO

T +1 281 878 6168

M +1 281 796 9038

F +1 281 715 4116

- <">mailto:->

www.ge.com

Dimension Rounding in Creo 2

davehaigh — Thu, 26 Oct 2017 20:57:44 GMT

Let me chime back in to this conversation.

First, off I want to know how to set the behavior back to ProE 1 thru WildFire 4 behavior.

Second, looking at Tim Coopers post I decided to do a test.

1. Create a new part

2. Sketch a rectangle and don't type in values for the dimension, just drag them to what you want.

a. My case the displayed values were 337.115, 173.235

3. Drag the depth, do not type in a value

a. My case the displayed value was 216.506

4. Measure the three lengths. The displayed values were 337.115, 173.235, & 216.506.

a. [cid:image002.png@01CDB73F.C5CC5DE0]

5. Now double click on the feature to see the dimension.

a. [cid:image003.png@01CDB73F.C5CC5DE0]

6. Now double click on the dimension.

a. [cid:image004.png@01CDB740.123FBF50]

Doesn't anyone have a problem with this???????

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550

From: Cooper, Tim P (GE Oil & Gas) [

Dimension Rounding in Creo 2

dpilkey — Thu, 26 Oct 2017 20:57:46 GMT

Hello,
We do here. With simple sheetmetal parts running out to 3 decimal points is useless for us. Also, what makes it frustrating is the inability to change it permanently. If we go in and edit it to 1 decimal or no decimals it just reverts back when you open the part again. We could live with it if the changes would stick.

Donald Pilkey
CAD Leader

From: Haigh, David A. [

Dimension Rounding in Creo 2

dgschaefer — Wed, 31 Oct 2012 15:33:53 GMT

"The old behavior has also lead to many parts being scrapped in
manufacturing by producing parts outside the limits of what the engineer
envisioned."

If the engineer is rounding a dimension, the only reason to do so is to
communicate a looser tolerance by either showing it on a drawing or
through the 3D model. If he/she rounds 0.28125 to 0.3 on the print or
in the model and is surprised when it comes in at 0.4 (at the end of the
drawing's +/- 0.1 tolerance), they need to review their notes from
school. Even if the model was 0.28125, showing the dim to one place
(0.3) means they are saying it's allowed to be 0.2-0.4.

In my mind, the model ought to reflect that because changing the decimal
places is changing the design intent. If you want the nominal to remain
but to have the more generous tolerance, then call it out as such -
0.28125 +/- .1000.

This is like the old shown vs. created dimensions debate, there's no
right answer. Do what your organization is comfortable with, but you
need to understand the ramifications of each.

--

Dimension Rounding in Creo 2

BenLoosli — Thu, 26 Oct 2017 20:57:49 GMT

Absolutely NOT!
Dragging is and never has been an accurate method of getting a dimension to the precision you want. The only method to give you control is to enter the values by keyboard.

Thank you,

Ben H. Loosli
USEC, INC.

From: Haigh, David A. [

Dimension Rounding in Creo 2

cfly — Wed, 31 Oct 2012 15:44:07 GMT

I agree that rounding should change the model. If my rounding creates an
interference, I want Creo to tell me so! The defaults never should have
switched without our knowledge; there's always been the option of making it
behave the way it does now, and those who want this behavior should have
always known to change the default settings on a new installation/upgrade.
Those of us who don't have never had to change the default settings and are
justified in expecting the previous default behavior to remain the same as
it always has been.

efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef

Dimension Rounding in Creo 2

davehaigh — Wed, 31 Oct 2012 15:47:36 GMT

And another thing, In the sketcher I noticed if I select a dimension and uncheck Round Display Value from the RMB menu. I get to see the full value of the dimension. But you have to do this for each dimension.

[cid:image005.png@01CDB744.580FEBF0]

David Haigh

Dimension Rounding in Creo 2

davehaigh — Wed, 31 Oct 2012 16:14:52 GMT

Ok, So if you set the config option:
Round_displayed_dim_values no

The sketcher shows the full value for all dimensions.

If you set the config option:
Sketcher_strngthn_to_def_dec_pl yes
(the default)

When you click on the dimension and then pick Strong from the RMB menu, it will round off the dimension to the number of digits set in default_dec_places.

This means if you forget to strength any dimension, they will remain at 11 decimal places.

David Haigh

Dimension Rounding in Creo 2

dgschaefer — Wed, 31 Oct 2012 16:26:54 GMT

I'd agree that dragging isn't a robust design method; however, if the
software is going to let me do it, it ought to give me accurate data.
If it drags to a displayed 3 places (and that's my default), the
resultant geometry ought to match that 3 digit number.

--

Dimension Rounding in Creo 2

davehaigh — Wed, 31 Oct 2012 16:44:55 GMT

I opened up a call with PTC and got a response from the TSE. One of the things he sent me was this email from the PLM.