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Dimension Rounding in Creo 2

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Granite

Dimension Rounding in Creo 2

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 in inches and 3 digits in millimeters.

I entered 3.9375 in the sketcher. The sketcher shows 3.938. Finish the feature and measure, it shows 3.9375. Double click on the feature to show the dimension and it shows 3.938. double click on the number to edit it and it shows 3.9375. The drawing shows 3.938. Edit properties on the dimension and it shows this.

[cid:image002.png@01CDB6A5.678682A0]

This is different behavior than in Wildfire 4.

What config options control this behavior?

* What settings make it like I see out of the box in Creo 2

* What settings restore it to traditional ProE behavior?

Why would I want the new behavior?

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

42 REPLIES 42
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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.
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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.



--
--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Dimension Rounding in Creo 2

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.
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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) [
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Dimension Rounding in Creo 2

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 [
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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) [
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Dimension Rounding in Creo 2

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. [
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Dimension Rounding in Creo 2

"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.



--
--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Dimension Rounding in Creo 2

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. [
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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
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Dimension Rounding in Creo 2

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.



--
--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Dimension Rounding in Creo 2

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.
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Dimension Rounding in Creo 2

The first rule of Sketcher is: "You do not leave weak dimensions."

The second rule of Sketcher is: "You do NOT leave weak dimensions."



Of course, this doesn't address the issue of fractional size imperial
features, as mentioned previously...



Jonathan


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Dimension Rounding in Creo 2

In Wildfire 4 M210 with no config options (default everything) following similar steps (some 3D dragging functions are not available in Wildfire 4), I get this...
Create a new part
Create a sketch of a rectangle with an embedded sketch and don't type in values for the dimensions. Sketch shows 287.90 and 136.44.
Create an extrude feature of the sketch, accept the default depth. Dashboard shows 95.69 for depth.
Measure the lengths. The edge length shows 287.895, 136.443, and 95.6900 (notice all show 6 digits -the default).
[cid:image008.png@01CDB770.F25FB0B0]
Right click the extrude feature and select Edit.
[cid:image006.png@01CDB771.78AE51D0]

Edit the definition of the sketch and edit a dimension (this seams similar to what you describe in Creo 2.0 only buried deeper). In case the image does not show, the value is 287.895154512!
[cid:image001.png@01CDB772.0D4C6E80]

If at any time during this process, I drag the sketch of the sketched rectangle to a particular size, it will snap to a two digit dimension. I think this "snap" is the behavior you would like to see in Creo 2.0.

Have you tried changing the config value for measure_dec_places? With this set to a high number (like 10), at least the measure and edit value will produce similar results.

There are also many grid snap config options that apply when dynamically dragging geometry that might eliminate the discrepancy between what is displayed and the actual value.

This behavior does not seem to be exclusively related to Creo 2.0 as originally stated.


From: Haigh, David A. [
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Dimension Rounding in Creo 2

If you have a 9/16 hole (.5625) in a part and dimension the drawing in decimals with a standard 3 place decimal (.562) callout, do you change the hole to .562 or the display for the hole on the drawing to 4 places, .5625 or do you let the software round the display value on the drawing to .562?


Thank you,

Ben H. Loosli
USEC, INC.
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Dimension Rounding in Creo 2

If the drawing shows the hole as a 3-place decimal, the hole is going to be
made to that 3-place decimal and checked with that number and the block
tolerance. I want my models to reflect what my drawing shows so that
everything interacts the way the nominal manufacturing values would, and
what I'm telling the machinist to make is what I have in my model. If my
model doesn't match what my drawing tells the machinist to make, how can I
be sure the parts are going to fit together the way they do in the model?



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef
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RE: Dimension Rounding in Creo 2

I sent a exploder warning about models not matching the displayed dimensions 2 years ago,WF5 users please take the time to read this and educate yourself on this major hidden issue.


This is a problem that all WF5 users fail to understand because its rather hidden and PTC is not telling anyone about it. In Sept 2010 we filed the original SPR (of many) to PTC, SPR 2018798. They did a emergency build release to fix this and added the new config.pro setting outlined in issue 2 below, but PTC never changed Pro/E's default settings and they never informed the user community so the underlying problem still exists.


There are 2 big issues here 1) Decimal Display and 2) Legacy Models both caused by WF5's new default settings, I will try to explain them as short as possible.



Issue 1. Decimal Display
In WF5 with default settings if you change the number of digits in a dimensions properties box be aware that check box Round Dimension Value really is Round the Displayed Value Only not Round The Model Value. A whole number would be fine but if the value number extends past the new number of digits, the models displayed dimension will be different then the model itself.


e.g. The 22.375 value has 3 decimals places, changing the properties to 1 decimal place will cause the displayed value in the model will round to 22.4. The true size and value of the model will remain 22.375 even after a regeneration. Since the model does not match the true dimension we want to turn off the Rounded Dimension Value option. This will make the model and the displayed value both update to 22.4 after a regeneration. Be aware the dimensions properties can be changed in the drawing or in the part.


Again if you ever change a dimensions decimal place make sure you uncheck the Rounded Dimension Value option and it is OFF if it isn't off already! or else theModels Actual Size many NOT Be the Same as the displayed Value!


Pro/NC, CMM data,exported files and even the Pro/E models themselves may not match the drawing or the displayed dimension.Always uncheck the Round Dimension Value option when changing Decimal Places, very scary and potently very costly, be aware! I have no idea what PTC was thinking on this, I heard it was caused when they tried to fix another bug with sketcher digits. But really PTC the model must always match the displayed values!!


So to avoid this you need to set (for new created dims)
round_displayed_dim_values set to ROUND NONE (default CALCULATED *)


One last gotcha, if your like my company and have may users and didn't know WF5 changed the rounding on every part dimension that was saved your SOL with those saved models because all those models saved in WF5 with out the round_prewf5_displayed_dim_val set to ROUND NONE will now have part dimensions with the rounding turned on and PTC has no fix for those limbo type parts. The two config's listed are for new dimension or for pre WF5 model dimension. Also PTC hashasno way to check a model or a database to see if a displayed dimension is the same as an actual dim, all causes by this display rounding. Very Very Scary! We had to manually check all of our released drawing and newly checked in released parts between our WF5 upgrade and the date we changed these settings to ensurenodimensions had the digits changed as we use models with Pro/NC, major pain and major cost, we were lucky to catch this somewhat early.


Good Luck


Steve Burke

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Dimension Rounding in Creo 2

That's the way I feel about it too, but you wouldn't believe the number or
engineers who want to round the drawing only
and not the model!

I've seen the issue with the parts not measuring what the dimension said,
didn't realize it was weak dimensions causing it. Good thing to know.






                                                      
                                                      
                                                      
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Dimension Rounding in Creo 2

My suggestion is to always make the model match the dimension exactly.
So, if fillets are R.38, they should be .3800 not .3750.





Christopher F. Gosnell



FPD Company

124 Hidden Valley Road

McMurray, PA 15317
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Dimension Rounding in Creo 2

Ok, I've been testing things out and talking with PTC tech support. Attached is what I came up with. This is based on some helpful replies on this website and stuff I got from PTC.

I think it's a shame there is nothing about this in any of the update training materials I've seen.

To us this is a huge issue. We need to get it configured correctly.

David Haigh
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Dimension Rounding in Creo 2

Thanks David Haigh,

Your attachment most important for me is the presentation on Dimension
rounding problem identification and resolution. I'm sure a large number
of system administrators will be talking about this with the users they
support using the presentation as an aid.

From the PLM -

" the user could measure the resulting geometry and see that it was
different from the displayed dimension value and say "What the heck?"
So, in Wildfire 4.0 we decided to ..."

should have ended with the words - _generate the geometry according to
the three places shown_.

"we explicitly have a checkbox for Rounded Dim Value in the dialog as
well, so*the user knows* up-front what's going on."

Because no one else needs to know what's going on? QA, QC,
Manufacturing, Procurement, other users? The easiest method is to mark
all such dimensions with the approximate symbol automatically, not add
another check box and new config options

Dave S.
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Dimension Rounding in Creo 2

Another screwy thing about this Rounded Dimension Value you have to watch out for is Limits dimensions schemes...

[cid:image001.jpg@01CDB808.12950E60]

[cid:image002.jpg@01CDB808.12950E60]

Even though you've specified +/-.005 in the tolerances it reports no tolerance on the limit dimensions.

[cid:image003.jpg@01CDB808.12950E60]

If you turn off the Rounded Dimension it now goes back to 10 place dimensions still with no tolerances.

[cid:image004.jpg@01CDB808.12950E60]


Carpe Diem,
"Happiness equals reality minus expectations"

Michael Heath
Schlumberger Reservoir Completions
14910 Airline Rd.
Rosharon, TX 77583
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