Skip to main content
D
davehaigh13-Aquamarine
13-Aquamarine
October 30, 2012
Question

Dimension Rounding in Creo 2

  • October 30, 2012
  • 42 replies
  • 107500 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


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

42 replies

Show previous replies
G
gwalker1-Visitor
1-Visitor
October 31, 2012
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. [
B
23-Emerald III
BenLoosli23-Emerald III
23-Emerald III
October 31, 2012
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.
C
cfly1-Visitor
1-Visitor
October 31, 2012
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
S
Stephen1-Visitor
1-Visitor
October 31, 2012

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

T
TerryJohnson1-Visitor
1-Visitor
October 31, 2012
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.






                                                      
                                                      
                                                      
P
ptc-19327451-Visitor
1-Visitor
October 31, 2012
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
D
davehaigh13-AquamarineAuthor
13-Aquamarine
October 31, 2012
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
K
kimndave91-Visitor
1-Visitor
November 1, 2012
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.
M
mheath1-Visitor
1-Visitor
November 1, 2012
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
J
JWayman1-Visitor
1-Visitor
November 1, 2012
I am still back on WF2, so I have no first-hand experience of this, but, if I read it right, doesn't this go away if you make all your sketcher dimensions yellow instead of grey?
If I am right, then it doesn't seem any worse than before: It is, and always has been, asking for trouble to leave sketcher dimensions or constraints grey. Things change unpredictably if you do.
Or have I missed something?
I'd like to know, because we will be moving to a later version soon...
John
Show more replies
Terms & ConditionsAccessibility statement