Detailing with an imported feature

[BONES1369]

WF 2.0 / M180


I have an assembly with 6 components. 1 out of the six components is an imported feature. A part file was made, then a parasolid model was imported into the part file, and then saved with the appropriate file name. I then created an assembly file and used this part containing the imported feature. Now I am trying to detail the assembly, and when I create a drawing view, the imported feature displays every line as a solid line. The view display settings are set to, "No Hidden", and "None" for tangent edges. Anyone experience this before?


Thanks,

 

[BONES1369]

After investigating a little further, it appears the software does not recognize it as a solid. I can actualy see geometry from another part that is behind the imported part. Also, it comes in with purple lines, which means it is being treated as something other than geometry.

 

[appinmi]

If the import has "purple" lines, it means that their are gaps between surfaces, or there are missing surfaces. You will have to "repair" the imported feature to eliminate the gaps or add surfaces. (If it cannot hold "water", it cannot be made into a solid).

 

[BONES1369]

Not sure what you mean by "repair". This model is 100% accurate and needs used in its current state. As far as I can see there are no gaps, just one solid surface. Is there a more accurate way to interogate?


One other thing I noticed is that it is a shell. I created a cross section of the import and it appears that the equivalent of a shell operation has been performed.Would that have an effect?

 

[appinmi]

If the imported featurehas no gaps, right-click the feature and select "Edit definition". Then on the top tool bar, select Edit, then Feature Properties. See if it will allow you to select "Make Solid".

 

[BONES1369]

When I check the option, and click ok, it tells me this,


"WARNING: Design intent is unclear. Use "Info"/"Geom Check" menu for details."


It will not allow me to make it a solid. Here is the error that geometry check gives me,


The import geometry contains small edge(s) and imprecise vertices.
These small edges may cause inaccuracies and problems with later features.

 

[appinmi]

That means that the imported feature is "not perfect". There was probably some confusion during the translation between CAD systems. Vertexes between surfaces are not exactly aligned. Right-click on the import feature from the model tree and goto properties. On the top tool bar, select Geometry. Select "Heal", then "Zip gaps". I hope this works because the only other option is to repair it manually which takes some practice.

 

[BONES1369]

Ok, I got there in a roundabout way. When I right click I did not have a properties option, so I used edit definition. Then the Geometry menu appeared on top, and I selected heal, and then automatic (the other option was manual). Then I was prompted to pick the geometry along with some other options I just left alone. I picked the geometry and clicked done. After that another dialoge box poped up along with a bunch of little marks on the model. I just left everything alone and selected "compute", and then "accept". Once completedI was able to check the box "make solid".


I have no idea what I just did but it worked. Is there a good book / tutorial out there explaining things like this? Thanks for all your help.

 

[appinmi]

Proe has the capability to automatically "repair" imported features if the "gaps" or "overlaps" are not too severe. When you accepted all of the "default" criteria which depended on you part accuracy, that told Proe "how big" of gaps or overlaps to repair. Your part must have been pretty close because this option only works about 10% of the time.


Sorry to say that I do not know of any tutorials on this subject, I had to learn by "trial and error". I suggest if you want to practice on this, make a copy of the original part and play with the copy.


I do not have the time right now, but I will try to create and post a simple tutorial as soon as I can, that will get you started.

 

[design-engine]

I think what he is asking for is to simply dimension the import
geometry in a detail drawing. You cant do it because there is
nothing to create dims to. The solution requires a little bit of
surfacing skills. Simply project a curve onto the top portion of
you r model and update your drawing. Dimension to that endpoint
you have in the model. We do this alot with amorphic forms that
dont have one strait edge on it. I can elaborate if that did not
make since.



Can I add that I love California! I have been here for a week and I don't want to leave.



Edited by: design-engine

 

[write2bush]

the most easiest method will be to Double click on the view, Go to View Display and select yes Under :Hidden Line Removal for quilts" you will be done with the un necessary lines.

 

[msmit]

After hours of trying various things that las one just did the trick for me.

repairing the import model was impossible (it was a complicated part with many defects)
so hidden line removal for quilts just did it.

manny thanks!!!