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Since ...
1. the drawing leaves a lot to the imagination and
2. the situation allows some 'rules' to be ignored ...
you can do the quick and easy: sketcher ellipse, a point on an offset plane,
Boundary Blend between the sketch and point. It makes a nice, well behaved quilt.
The rest (extrude a 'side wall', merge, round, thicken or cap and shell) should be
routine for you.
Attached is a wildfire 2.0 model of one of the parts (I did not model the second concept). A family table could be used for both instances.
I used a combination of variable section sweep and boundary blend. After merging all the surfaces together and solidifying, the part was shelled out. There are probably other methods available for creating this part, and it has been a while since I touched Pro-E. I have been modeling in SolidWorks lately for other clients as Pro-E jobs seem less plentiful now.
I did not know a boundary blend could be done between the ellipse and the point, and I created this model before I read the above post. That is a very useful technique! However, the wall is 25mm high (normal) to the base plane before the transition occurs, and the variable section sweep in my model represents the vertical wall (zero degree angle can be modified to account for draft if needed). I could probably reduce the feature count if I use some of the suggested techniques from the previous post.
Jeff your files are always interesting for a surfacing newbie like me, one question though: of the different approaches that you shared is one "better" than the other? And how can I tell if a surface is "good" or not? Cross sections analysis with curvature plot is enough?
It's hard to say what's best. Depends on a lot of variables and, really,
needs to be addressed on a per instance basis. Normally, if I'm
concerned with quality and robustness (not likely to cause problems
with downstream features, processes, uses) I avoid creating singular /
degenerate edges and Boundary (Blend) Blobs. That particular shape is
simple and 'regular' enough that a minimally defined (two boundaries,
one G0, one G1 constraint) Boundary Blend with singularity creates a
nice, clean surface with a minimal amount of effort and care. It would
probably serve most purposes* well. OTOH, if the user knows how to
create an elliptical paraboloid, knows that it will trim to an
elliptical boundary, it's little effort to create.
* This would bug me if I had to do a finite element model. Surface
isoparms affect meshing; FEM, analysis functions and rendering.
Note the difference between upper (the BB with singularity) and
lower (swept paraboloid) halves.
You need all the analysis tools Pro/E offers. (And then some if you
really want to be particular. I use Rhino's to supplement. Better, in
general, than found in 'mcad' programs but missing some that Pro/E
provides so they complement one another.) Try to get familiar with all
of them. The ones you'll find most useful will depend on what you're
doing.
_ _ _
I was unable to open the zip files. I getthe error message Unable to install over the MSI version of the installation. Have you ever encountered this before?
I was having trouble with all of them. I went back and checked some ZIP files I had that I know I could open before and I'm getting the same message. I also checked my start programs an it appears our IT personnel may have removed Winzip for some reason. So the problem is on my end.
They can perform updates to our machines remotely. Looking at the installed programs it now appears there was an attempt to update to a newer version of Winzip. Because IT requires we have version 11.1 it looks like it corrupted the installation. I hate it when they do this mess.
I reviewed the concepts you created after I uploaded mine, and had some questions. I like the fact you could create reduce the feature count.
I noticed on the top surface you used a Var Sec Sweep (prt0001) instead of a boundary blend. I had previously thought about that scenario, but could not determine how to do it in Pro-E. SolidWorks has a feature called "boundary surface" which allows the selection of cross curves in direction 1 & 2 (X & T profile arrangement) to create the surface. I could not get the Boundary Blend in Pro-E to do this correctly, but noticed you were able to accomplish it by using the Variable Section Sweep.
Also, the 3rd concept you created (prt0003) is a much larger file size. I do not understand why it is a larger file size as the feature count is not higher than the other concepts. Overall, the models are very good, and if I needed to create a similar model in the future I would probably choose your first concept (prt0001)
Lately, I noticed you used the thicken instead of shell. Since this is similar to a sheet metal part, thicken is probably the best technique. However, when designing an injection-molded part I find that shelling usually produces a more robust part when making modifications to the part.
It has occurred to me that if this was a sheet metal part, it could be created using a forming tool (form punch) where a flat pattern could have been created.
> (prt0001) ... were able to accomplish it
> by using the Variable Section Sweep.
The key is to use the Constant Normal Direction option to keep
the (progressing) section plane parallel to the start section.
> (prt0003) is a much larger file size.
> I do not understand why it is a larger file size
? Suppressed and zipped, prt0003 is actually the smallest. Ok,
unsuppressed it's the largest ... I'm going to guess the file
sizes are related to the 'density' of the surfaces created. The
CV counts for all surfaces in the models are; prt0001 (1080), 2
(3596), 3 (5536) amd 4 (1468). (It is common to see file sizes
almost double if you change abs accuracy from .001 to .0001.
That is because spline surfaces, intersection / trim curves, etc.
densities are greater to achieve the accuracy. Here, though, they
are related to creation method.)
Regarding thickening vs. shelling; my first thought is that there
shouldn't be any difference except that the flange end trim, if it
were not perpendicular to the 'base' plane, would be different.
Both function work by creating surface normal offsets of the
original open or closed shell / quilt. The creation of 'capping'
(like the flange end) surfaces will be different and that might
explain why one works better than the other sometimes(?).
> flat pattern could have been created
You can get a decent approximation using Pro/E but it would require
some 'cheating' I believe (start with a flat oval and flange?).
I use a different method, curves by equation, boundry blend it together, it's a full ellipsoid at this point, solidify that, then solidify <trim use quilt ;-( > , extrude the flat, then shell. -- 18 features including the datums. File size before shell 149k, after shell 449k. then I can family table the other one. weird the family table version is 382k ?? Not sure how big of files you guys are talking about. I don't see a shell thickness on the print
What tool do you use to calculate the number of control vertices (CV) in the model for each part file? I assume it is located under analysis. I noticed you changed the arc into a spline (convert to spline) in the sketch mode to avoid a sharp transition after adding rounds/fillets.
In the image below, notice that using SolidWorks, I was able to create a surface using an X profile curve arrangement (direction 1 & 2). In Pro-E, the variable section sweep created a T profile curve arrangement, then was mirrored. Can a X profile curve arrangement be created in Pro-E, and if so what surface feature tool would you use?
Thanks, you made a good point. I should have stated my request more clearly. Although I do have the ISDX module, I have a concern when designing a part for another client. If my client does not have the ISDX module, then their ability to modify / edit the part will be limited. Is there another option for creating this surface without using ISDX?
PTC should roll its ISDX into the basic package without charging extra. SolidWorks ISDX equivalent is all part of the base package without paying extra. Any surface features I create in SW can be modified by another SW client, as they will have the same surfacing capabilities. I think PTC would improve its sales by not making it customers pay extra for the ISDX.
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