Imported Geometry fixing...

To delete the surfaces:

Alternately, you can switch to Legacy mode (Applications menu) and Remove the surface(s) (keeps history).

I'd, after deleting the unwanted faces, make sure the edges are "clean" and create new surfaces in Standard mode. These can be "Collapsed" into the imported feature if desired (Edit Definition the import, Geometry, Collapse..).

(I think you were talking about "Delete Contour" (?). It removes the trim boundary on the surface.)

(I haven't been thru the tutorial, can't say if there are any snags in it. Are you sure you Wildfire version?)

(Edge colors indicate joined and unjoined surface edges, as well as "solid" objects.)

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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

Jeff Howard wrote:

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

meld_b wrote:

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

David Janes wrote:

Accuracy is probably the most confusing and difficult to control 'feature' of pro-e.

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."

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. I have found that for forged or cast parts with many features , draft, and large fillets, I 'hit a wall' at about 150 features.

If you import the IGES or STEP file using File|Open, the system DOES NOT use your start part, and defualts to .0012 relative accuracy. I have found that changing the accuracy after importing the data does not seem to help heal the imported geometry.

If you creat a part first, and then import the geometry using Insert|Shard Data|From File... The start part accuracy will be used, the data will import differently, and may heal.

Lastly, when import> Thanks... this did help a couple of parts... I was a little surprised to

: 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