cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

ACCURACY FROM RELATIVE TO ABSOLUTE CREO 7

Matteo_1987
15-Moonstone

ACCURACY FROM RELATIVE TO ABSOLUTE CREO 7

I have a client who with creo 7 cannot change from relative to absolute precision.

I tried to activate the enable_assolute_accuracy entry for it but it is no longer valid.

Do you know if there is a new entry, or how to change a model from relative to absolute?

It seems that the menu in the properties makes me change only the values but not change the method.

Hello

Thanks

5 REPLIES 5

The options to enable absolute accuracy have been removed in 7.0.  Default for new models in 7.0 is absolute accuracy (using a start part uses the defined accuracy in the start part).  Not sure why you are not being allowed to change from relative to absolute.  I am able to change accuracy of old parts.  Though most of the time complex parts tend to fail when changing to absolute.

kdirth_0-1638364668676.png

 


There is always more to learn in Creo.
LawrenceS
17-Peridot
(To:kdirth)

@kdirth

I am very interested as to the issues you have experienced, as so far I have only from other users that absolute accuracy is very stable in Creo7 and causes less failures.  What you are saying though is truely a show stopper and may put a stop to us switching to Abs accuracy for any parts at our company.  Can you elaborate on how your models are failing when going from Relative to Absolute Accuracy?

  • How complex is complex?  Bounding box size?  Size of file?  Number of features/components in the feature tree? Something else that makes it complex?
  • Did you experience these failures on parts, asms, drws or all?
  • What value for absolute accuracy did you use?  Or did you try several?  e.g. 0.0003"?  0.0001"?  Are you metric or English units?
  • If failures were in assembly mode, were the components and asm all at absolute accuracy?  Or just the asm?  Or just the asm and some of the components?
  • What build of Creo7 have you experienced this on?  e.g. we are testing Creo 7.0.7.0 right now.
  • Did you submit a case to PTC?  If so is there a ticket you can refer me to so that I can track what the exact issue is and if and what version they are correcting it on?

"When you reward an activity, you get more of it!"

The problem is only with part models and has always been a problem as far as I know.  I know I have tried it in Creo 2.0 with the same issues.  I have not submitted a case to PTC for this issue.

 

The issues I have seen are only with converting models to absolute accuracy and using inheritance features.  You do not need to convert old models to start using absolute accuracy.  Both relative and absolute models will live happily together in an assembly.

 

Absolute accuracy works very well when a part is started with absolute accuracy.  I work with a lot of contoured surfaces (for seat cushions) and complex shapes (for stamped sheetmetal and plastics).  Models tend to lose references and features fail to complete features when converting.  We just do not convert old models to absolute accuracy.

 

We are working in metric and currently use and accuracy of 0.001 mm.  I have not experienced any issues that I can attribute to absolute accuracy in creating new models except when using inheritance features. 

 

When creating a new model and trying to inherit a model made with relative accuracy, it will not work.  I always have to change the new model to relative to get an inheritance to work when the inherited model is relative.

 

Our start models have all been converted to absolute and our old models are not being converted.  There have been no issues with using both relative and absolute other than using inheritance features.  Our mold maker is much happier with the absolute models because he usually remodeled our parts to get the model quality he wanted.

 

Hope this helps.


There is always more to learn in Creo.
tbraxton
20-Turquoise
(To:LawrenceS)

I have never encountered a version dependent issue with accuracy conversion in Pro/E or Creo Parametric. I doubt any of the issues you are describing are release dependent. Converting from relative to absolute has always been fraught with failures. I have had to correct this deficiency in existing designs and often it is faster for me to rebuild the model than to attempt the conversion to absolute accuracy.

 

Some critical points regarding your issues.

 

  • Absolute accuracy has units of length (some people conceptualize this value as resolution)
  • Relative accuracy is a dimensionless parameter whose value is not fixed (it is a function of the size of the model bounds)
  • PTC has always advised the use of absolute accuracy in practice but it is was not the default setting
  • You must match absolute accuracy for data sharing features to avoid issues (Copy Geom, Merge/Inheritance etc.)
  • Using relative accuracy will likely cause problems inside and outside of Creo for tool path creation, mold cavity/core splits etc.
    • Outside of Creo it is an issue because model resolution is mismatched even with neutral file formats
  • Smaller absolute accuracy values increase model regeneration time vs more coarse values or relative accuracy

You should always use absolute accuracy for your designs.

  • The absolute accuracy should be based on actual manufacturing tolerances for your design (if tol is +/- .01 units then set accuracy to .001 units)
  • Create start parts with accuracy for manufacturing processes with different process capability for resolution (units of length)
    • For example I have start parts for MEMs devices that have length units set to 10E-6 meters with absolute accuracy set based on x-ray lithography resolutions
    • I also have start parts for injection molded plastic parts using  length units of millimeters and absolute accuracy set to .001 mm

If you are working on structural steel parts that have tolerances of  +/- 0.1" don't set the absolute accuracy to 1 nanometer. In general I have found that setting the accuracy one order of magnitude smaller than process resolution works well. 

 

tbraxton
20-Turquoise
(To:Matteo_1987)

As shown by @kdirth Creo 7 still supports relative accuracy. The config option enable_assolute_accuracy is not valid in Creo 7+. Creo 7+ uses absolute accuracy by default. If you have legacy models or start parts that use relative accuracy they are still supported.

 

You can change the accuracy by the following UI selections:

 

File->Prepare->Model Properties->Accuracy->Change

Announcements