Imported Geometry fixing...

OK so I tried to get through the Suggested Technique for fixing import
features found on the PTC site found by searching on "Import Surface"...
http://www.ptc.com/cs/cs_24/howto/dtrsuf30/dtrsuf30.htm

I thought the pick "Done Sel" is gone out of Wildfire... Anyway I can't
get the directions in there to work all the way through, anyone have an
edited version?

I've got an imported STEP file that has a couple twisted surfaces and
surfaces I'd like to delete. It seems like I should be able to go into
Heal Geometry/Manual and Delete and pick a surface and it would be gone!
However, this little circular surface immediately jumps to a square when
I try to delete it. Also I can define a new surface but I'm unclear as
to whether I have manually connect up the edges of the circle. The
process of using "Isolines" and connect seems to make sense but then do
I have to run Heal Geometry/Automatic??

-D

 

Jeff - Thanks! Once you know to use THAT Delete it makes sense... but
the Suggested Technique get's you keyed into this delete from inside the
Heal Geometry/Manual menus. I deleted the surfaces, Edited one surface
boundary with Project and also delete one edge from a countour and then
recreated a surface with Surf Boundary and then it allowed me to make it
Solid. .... with the hotline helping me through it.

Sounds like they don't recommend using the Legacy mode anymore... "it's
a part of the code that hasn't been updated in a while"

-D

 

Wow... my second part could NOT be fixed even with the hotline trying to
help me. The user interface to some of these commands inside Heal
Geometry is pretty bad!...They finally ended with telling me to change
the accuracy of something... Can anyone explain this a bit more. Seems
like I have to change the outgoing system tolerance and Pro/e's??

By the way anyone else seen the Mechanica's translators are going
downhill... used to be I'd get something from almost anywhere... Now I
can create STEP or IGES files for things that look solid in Wildfire and
they say either "File Cannot be opened" or it crashes Mechanica... comon
PTC!

-D

 

: Wow... my second part could NOT be fixed even with the hotline trying to
: help me. The user interface to some of these commands inside Heal
: Geometry is pretty bad!...They finally ended with telling me to change
: the accuracy of something... Can anyone explain this a bit more. Seems
: like I have to change the outgoing system tolerance and Pro/e's??
:
: By the way anyone else seen the Mechanica's translators are going
: downhill... used to be I'd get something from almost anywhere... Now I
: can create STEP or IGES files for things that look solid in Wildfire and
: they say either "File Cannot be opened" or it crashes Mechanica... comon
: PTC!
:
Several recent messages, including those related to Mechanica, seem to bear on the
question of model accuracy. In one post, it was called aspect ratio, but means the
same thing ~ the ratio of the smallest feature size to the largest. The default
ratio, which you will see by going to 'Setup>Accuracy'. When this ratio is too
small, small holes, small surface patches, small radiuses, thin walls or thin
sheets, etc. may not be interepreted correctly. Surfaces may fail in surface
merges, parts may fail in merge cutouts, imported surfaces may fail to 'seal up'
and thus not be suitable for creating solids. Often, when these problems are
encountered, changing the accuracy ratio to a higher value (1 to 1000 or .001
instead of 1 to 100 or .01 or higher still), then regenerating, may solve the
problem. Accuracy issues are one of the more prevalent and mysterious cause of
problems in Pro/e and in exporting to and from its modules.

David Janes

 

Thanks... this did help a couple of parts... I was a little surprised to
see that it just ignores any features below a certain size... GONE! Well
I guess it's what I was trying to do manually, but it is a little scary!

I also was expecting more range on the accuracy than for .01 - .0001.
Can anyone explain relative vs. absolute accuracy? Isn't there a better
scheme than taking overall geometry diagonals to set this?

-D

 

: Accuracy is probably the most confusing and difficult to control
: 'feature' of pro-e.
:
Hear, hear!

: A search of the knowledge base found the following (among others):
:
: TPI 32869 "Detailed Information Regarding Model Accuracy"
: TPI 102316 "Determining the Accuracy of an IGES File."
: TPI 102317 "Determining the Accuracy of a STEP file."
:
And don't forget the doubly obscure 'absolute accuracy' which is absolutely the
opposite, i.e., accuracy of part with respect to assembly and the awkward
translation involved in making them equivalent.

: From my own experience, my start part has a default relative accuracy
: of .0001. The parts I design are no larger than 24 x 24 x 24 or smaller
: than 1 x 1 x 1 (approx). Yes, I have had to change the accuracy from
: time to time to create certain features.
:
: BTW, the silliest thing about accuracy is that when designing, the 'best
: practice' is to start with large features and progress to smaller
: features. But the accuracy never gets 'finer' only 'coarser' as you
: progress.

While I agree that this is silly, contradictory, obscure, etc., the main thing
that irriatates me is that the whole thing is so fundementally pointless. PTC/Proe
have all the information about features/parts/assemblies..... and computers to do
the figuring. All that's required is some programming and "my" problem (which the
PTC goofballs invented in the first place) just goes away. PTC absolves itself by
distributing TANs and advice on 'figuring' stuff. Phooi, let the computer/program
do the figuring ~ that's what they're good for. This should go on behind the
scenes, quietly, invisibly, without the silly fuss and bother, without TANs and
help files and advice, the same way it takes care of the descriptive geometry
behind spinning a part. Do I want to get involved in the descriptive geometry
calculations? No, I took the course and I'm very happy the program is doing it
quietly, in a nice taken-for-granted way, behind the screens. It ought to do the
same with 'accuracy'.

David Janes