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davehaigh13-Aquamarine
13-Aquamarine
October 30, 2012
Question

Dimension Rounding in Creo 2

  • October 30, 2012
  • 42 replies
  • 107375 views
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


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davehaigh13-AquamarineAuthor
13-Aquamarine
October 31, 2012
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) [
D
dpilkey6-Contributor
6-Contributor
October 31, 2012
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. [
D
dgschaefer21-Topaz II
21-Topaz II
October 31, 2012
"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.



--
B
23-Emerald III
BenLoosli23-Emerald III
23-Emerald III
October 31, 2012
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. [
C
cfly1-Visitor
1-Visitor
October 31, 2012
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
D
davehaigh13-AquamarineAuthor
13-Aquamarine
October 31, 2012
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
D
davehaigh13-AquamarineAuthor
13-Aquamarine
October 31, 2012
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
D
dgschaefer21-Topaz II
21-Topaz II
October 31, 2012
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.



--
D
davehaigh13-AquamarineAuthor
13-Aquamarine
October 31, 2012
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.
J
JonathanHodgson13-Aquamarine
13-Aquamarine
October 31, 2012
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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