Geometry Check

Hi folks !
I'd like to better understand the meaning of "Geometry check" info.
Anybody knows where it's possible to get info, docs, examples about it ?
Thanx in advance

Pier

 

It's a listing of geometry that isn't quite right. Sometimes it's an
accuracy issue, or strangely shaped surfaced that don't make a nice
solid, sometimes it's something else. I personally never found or
looked for a good reference on how to solve geometry checks. I just
experiment with alternate ways to make the geometry until I find one
that works without a throwing a geom check. For example, today I
imported a model and got a geometry check in the area of some raised
lettering on the part. I was unable to export it as a result. Geom
check showed me where the problem was, and I used a cut feature to
remove this lettering feature. Now it exports without a problem.

If you have any problems or errors working on the model, look at the
geometry check list.

Dave

 

Hi folks !
I'd like to better understand the meaning of "Geometry check" info.
Anybody knows where it's possible to get info, docs, examples about it ?


Causes are pretty much as Geesaman described; info is scarce, Help files have some info that might be worth considering (use interactive help on 'Info>Geom checks') but you'd spend your time more wisely cultivating a PTC modeling guru. Maybe there's a course they offer that takes you through the error resolution process. I haven't found it yet.

In my experience, the chief thing that causes geom checks is accuracy issues, especially between Pro/e and other modeling packages, when importing and exporting models. Model size, for accuracy purposes, often does not translate easily between packages and scale is accounted for differently in each.

Some things that can be done to aide this data translation, especially when we are talking about assemblies or tooling/manufacturing merged/cutout parts:
1.. Convert part accuracy to absolute (highest level) accuracy. This should be a realistic proportion/scale/ratio for comparing part accuracies. You can turn this on by setting enable_absolute_accuracy to YES in config.pro ('Tools>Options')
2.. In config.pro, set accuracy_lower_bound to something obscenely small, like .00000001
3.. Also set def_abs_accuracy to something like .00001 which will come up when you pick Absolute Accuracy in the 'Edit>Setup>Accuracy' menu as the default value.
4.. Set all parts and assembly to absolute accuracy
5.. If you want to "Open" import files directly, set the configuration option intf_in_use_template_models to YES. This buys you your default csys, planes, parameters, settings like material, units and accuracy and anything else embedded in the start part. If the start part's model units are different from the import model's, Pro/e does the conversion.
6.. Otherwise, create a new part from start part, then do 'Insert>Shared Date>From file' and select your .igs or .stp or .sat or etc part type from the drop down list.
7.. Regen everything and see if you get the geom chk again. 95% of the time I have done this, the 'geom chk' went away, Pro/MAGICALLY!
I've not seen any comprehensive references on this. If they exist, they are available privately. PTC is all about secrecy, especially in how its program works. The more you pay, the more you find out!!!!! You think if you put out for a license, you should know how the program works!?! No, there's much more to pay to get into the inner circle where they share the real knowledge.

 

Thank you for reply.
I remember to have seen in the very old ProE manual (maybe rel 13!) some
pages dedicated to geometry check, but i haven't that manual.
I generally find geometry check also if there are many rounds and it
should be useful to have some references in order to avoid these kind of
problem.
Thank you again
Bye
Pier

 

Thank you for reply.
I remember to have seen in the very old ProE manual (maybe rel 13!) some
pages dedicated to geometry check, but i haven't that manual.
I generally find geometry check also if there are many rounds and it
should be useful to have some references in order to avoid these kind of
problem.
Thank you again
Bye
Pier


I remember those manuals, as well. I've heard that they were produced as PDFs and were distributed with the documentation disks. Never could confirm this but yeah, you're right, they stopped publishing the bound editions around R20. Online, under Reference Docs, there is a "Help Topics Collection" that could be the equivalent of these docs because it seems to cover every module, including ones on feature creation, part modeling and part design with stuff on rounds and geom check. 50 Megs of PDF documents ought to be of some use.

David Jnaes