Sectioning in Wildfire 2.0 & other Q's

Pro/e group,

I am a newbie Pro/e user, but feel I'm catching on pretty well even though
WF2 has many changes from the WF1 primer. We've hacked our way through and
our first impression is that we like it.

I have many questions for this usenet group, but let's start with this.

1) Our primary use of cad software is aerospace design, specialing in
airfoils and ceramic cores. These require complex surfacing, contour and
cambering. Our primary way that we accomplish this is through sectioning.
Let me explain that when I use the term sectioning, there may be some
confusion with WF terminology. As an example of what I am talking about,
take a baseball bat (say 34" long) and cut a cross-section every 2" along
it's length. You now have 16 (or 17 if you started right at the edge)
variable-sized 2D 'sections' that define the final contour of the bat.

This is similar to how airfoils are defined. However, we aren't always the
ones defining them! Sometimes we get UG or CADDS files and must make our
own 'sections'. What method is used to accomplish this feat in WF2?
Example: Someone supplies you with the afore mentioned bat, but the file
does NOT contain the geometry with which they cambered to (from an .igs file
for instance). They ask you to place a variable band in certain places
along the length of the bat. Normally we take 'cuts' through the surface
geometry and end up with 2D sections spaced along the part. We then
manipulate the 2D sections (charts) and then rebuild the surfaces to the now
revised geometry (CADDS 5i, btw).

The question could be phrased: How can WF2 cut sections through specific
geometry in specific locations to return a 2D section?

Thanks,
Crew

 

Not often how they are defined, just how they are sometimes "reconstructed"
or so I've been lead to believe. But, to get back to your question <g>, you
can set up datum planes and Intersect the planes with the surfaces I'm
assuming you have. I think it might even be possible to do one and pattern
the remainder.

Now, after reading back thru your post I'm not really sure what sort of data
you are getting to work with. If it *is" surface data, wouldn't you be
better off copying, offsetting, trimming, etc. the surfaces to create
whatever you are doing than pulling a multitude of section cuts off and
creating surface from them?

Sorry if I'm completely missing the point.....

 

: >
: > This is similar to how airfoils are defined.
: > However, we aren't always the ones defining them!
: > Sometimes we get UG or CADDS files and must make our
: > own 'sections'. What method is used to accomplish this feat
: > in WF2?
:
: Not often how they are defined, just how they are sometimes "reconstructed"
: or so I've been lead to believe. But, to get back to your question <g>, you
: can set up datum planes and Intersect the planes with the surfaces I'm
: assuming you have. I think it might even be possible to do one and pattern
: the remainder.
:
: Now, after reading back thru your post I'm not really sure what sort of data
: you are getting to work with. If it *is" surface data, wouldn't you be
: better off copying, offsetting, trimming, etc. the surfaces to create
: whatever you are doing than pulling a multitude of section cuts off and
: creating surface from them?
:
I think I share Jeff's doubts. Sectioning is no problem. Go to 'Tools>Model
Sectioning' to turn your cutting planes into cross sections. Then what?

The problem comes down to a methodology for making wings with Pro/e, particularly,
surfacing. You might make a wing as a blend which is where your cross sections
might come in handy. But this is a very awkward way to do it and gives you no
control along the length of the wing which could easily result in wavy or lumpy
surfaces.

But anything beyond that and this collection of sections becomes less important.
What is more important is curves that you would constuct as trajectories for a
swept blend or for a variable section sweep. My advice would be to become fast
friends with the variable section sweep. One section, created at one of the end
points of the trajectories sweeps along them with changes to its shape being
guided by them. This makes the smoothest surface possible in Pro/e. Other
construction methods which use these long curves rather than a series of closed
cross sections are boundary blend surfaces and the nurbs type surfaces created
with ISDX. These, too, can achieve good continuity.

There are other problems, too, with the methodology you describe. Anyone familiar
with surfacing and the datum curve rigging used to hold up the surfaces could tell
you how to create curves at the intersection of a plane and your imported IGES
surface. The problem you'd immediately inherit from the surface is that Pro/e
breaks these curves at each of the surface patch boundaries. You wind up with a
heavily segmented curve. Analysis of such curves will show them to be
discontinuous. The curves, even if they could be used, would introduce this
discontinuity into the surface built on them, by whatever means it is built. But,
in truth, you wouldn't be able to use these curves for blending as blends require
sections with the same number of vertices in them. Your series of sections would
not likely have, from one to the other, the same number of segments/vertices.

So, the task at hand may not be to figure out sectioning in Pro/e but to figure
out the entire workflow and methodology, given the Pro/e tools available. And, I'd
give some serious thought to taking a surfacing/advanced surfacing course. I'm not
saying you can't "wing it", but it's not easy even with the course and a
knowledgeable instructor. It's certainly way more than I'd like to try to do using
a newsgroup.

David Janes

 

This is called "lofting" - or at least, it has been for the
past 500 years.

If this is your primary task, you might be better off looking
at some of the programs specifically oriented to creating hull
shapes, such as VX. It's cheaper, too.

 

We have been utilizing CADDS for many years and using this methodology (2D
cross-sections) have created, and sometimes recreated, seemingly perfectly
smooth surfaces that are near-perfect representations of the data received
(usually, much less than 10% of our available tolerances).

Many times, however, the sections we cut through our customer data will have
different segment amounts and, more importantly, have varying spline
degrees. We find that spline degree plays a far more important role in how
smooth the created surface will be, how well we can 'sculpt' (Cadds term for
using a surface to 'cut' or bisect another surface or solid) and certainly
how easily we can NC the finished surface. By default, a lesser degree
nspline has fewer segments anyway.

After we create all of our sections usually each must be manipulated to
reduce segments and reduce spline degrees. A 3rd degree is the simpliest
nspline (a line would be 1). Many times we get 5th and 6th degree nsplines
and greater. As you might imagine this makes the surfaces slightly wavy,
knotty and otherwise unacceptable not to mention the strain it can place on
processors and memory! After approximating the nsplines to a maximum 3rd
degree and having SIMILAR segments and knots we then create the surface.
This 'approximation' can usually be done to a tolerance of .0002 or smaller,
sometimes much smaller. Note, however, that the segments between the
sections does not have to be exactly the same and, in fact, CADDS will
usually create a surface even if the segment difference is large (say 15
segments on a 3rd degree spline compared to 92 segments on 7th degree),
however the resulting surface is admittedly ugly. Many times with all the
nsplines at 3 degrees we may have segments that range from 12 to 25, yet the
surfaces come out awesome.

Even if we place sections on our surfaces in the customer-supplied locations
(usually obtained from their print) and after manipulating the 2D splines to
the smoothest we can reasonably create the resulting surface may still not
be smooth enough. We then take intermediate sections to smooth out the
surface even though doing so may add some degree of complexity to the
surface simply because there is more controlling data.

On top of that, many times our manufacturing process calls for us to extend
the length of the airfoils, usually in both direction. In this case, we
create 'faring' sections usually utilzing the appropriate end section,
offsetting it and manipulating if necessary in order to maintain a
consistent surface. Sometimes we can simply 'extend' the surfaces to create
the next defining section, but I've never had that create a 'perfect'
section. I've always had to manipulate it to close it up or smooth it out.

Also, usually when I create the 2-d sections, it is not a closed loop, it
ends up being 6 separate entities. ID (concave/pressure), OD
(convex/suction), LE OD, LE ID, TE OD and TE ID being that the LE and TE are
split at the chord. If the airfoil is simple (i.e. relatively 'flat' and
straight) it may take only 3-5 sections to recreate it. However, if it has
a lot of twist or the interior has alot of variable surfacing (which is
common), it may take 30-50 sections to create a true representation of the
supplied data. Sometimes the sections we are looking to cut are not related
to the actual airfoil surfaces but other geometry and we simply need to be
able to take a 2D cut along the CG and 'sweep' (I believe it's called
rotational sweep on Pro/e) around the C/L of the part.

Of course, all of this is based on recreating customer-supplied data to
within 'microfarbles' (as my old boss used to say). This does not even
begin to get into what we call cambering -- the surfaces that must be
created to transcend from one surface to another and it usually requires
alot of sectioning and manipulation due to many other variables that come
into play.

To Jeff's point, sometimes the alterations we need to make to the data are
so varied that I'm not sure simply offsetting or other forms of surface
manipulation would work. There certainly aren't any appropriate tools in
CADDS for this and I doubt there would be something that would be powerful
enough on Pro/e to produce what we require.

If this type of methodology is possible in Pro/e, I'd like to know how
others accomplish it: sectioning, approximating, creating faring sections,
surfacing. If I can achieve a result as accurate without increasing
engineering time I don't mind restructuring my thinking to a different Pro/e
methodology, I just need to know where to go to be 'schooled' as they say.
I'd like to "wing it" (nice Dave...) before attending any formal schooling.

Any help on use of the tools mention by Jeff and Dave in creating these
surfaces would be appreciated. I thank you for your time gentlemen.

-Da Crew

 

At least to the best of my knowledge......

All intersection curves created in Pro/E (Pro/Surface, don't know about
ISDX) will be degree 3 max (as will be all surfaces). Control vertex, knot,
etc. count will depend on the file accuracy setting at the time the entity
is generated. (Higher degree surfaces can be imported, maintained,
exported. Curves are always converted to deg 3 max, or so it seems.)

Curve CV or knot span (I'm assuming what you are calling "segments") / count
doesn't have a direct effect on surfaces created from the curves. The
surface CV count will depend on file tolerance settings. (Just for jollies,
I created a typical leading edge curve set; 150 CV's inbd end, 15 CV's outbd
end. A Boundary Blend between the two curves with an absolute accuracy of
..001" produced a surface with 26 CV's in the U direction and nice, straight
"element" lines, gaussian curvature of 2e-7. The same surface regenerated
to an accuracy of .01" had 19 CV's and deviation from the original curves
was .002". The curves were created in Rhino and surfaces evaluated in
Rhino.)

Guess what I'm getting at is that some of the problems you describe above
shouldn't be problems in Pro.

Without seeing (and probably trying to do) what you need it's hard to offer
an opinion, but once you become more familiar with the tools available maybe
some lights will start flashing.

I don't know if you've ever tried it, but Rhinoceros is well suited to a lot
of the operations and methods you've described. I use it extensively for
curve / surface refinement.

The tools available in Pro/E are effective for things like starting with a
set of wing OML surfaces and creating ribs / formers, stringers, milled
skins, etc. I'm not sure I understand what you are doing when "cambering".
If you are altering the airfoil section or warping the airfoil... I guess
it depends on application; air transport catagory or R/C model. 8~)

=====================================

 

CADDS is known as an excellent ship building program. I'm not sure if there
is an additional module specific to ship building but we do, in fact, have a
loft command. I've been using CADDS for 5 years and have yet to use that
command. I asked some of the guys with three to four times that experience
w/it and they've never used the loft command either.

If Pro/e does not have the capabilities to perform these tasks we should
look elsewhere. We already know SW will not suit our needs but UG will,
with a much heftier price tag, of course.

I will look into the surfacing classes that Dave mentioned. Anyone know of
good surfacing manuals or books for Pro/e? What is VX?

 

Used to be called Varimetrix. Their website is not very
informative :-( Fricking marketing assholes could break
the ears off a brass donkey ...

Anyway, it's a pretty nice program. The reason I mentioned
it is that they got a large $$ infusion from a Japanese ship-
building company a while back. It is supposed to be especially
good at hull shapes. Worth a call, anyhow. And it's not too
expensive - about five grand, comparable to Pro/Foundation
except you get some machining capability for that, too.

http://www.vx.com will get you there.

 

: > "Da Crew" wrote ....
: > We have been utilizing CADDS for many years and using
: > this methodology (2D cross-sections) have created, and
: > sometimes recreated, seemingly perfectly smooth surfaces
: > that are near-perfect representations of the data received
: > (usually, much less than 10% of our available tolerances).
: >
: > Many times, however, the sections we cut through our
: > customer data will have different segment amounts and,
: > more importantly, have varying spline degrees. We find
: > that spline degree plays a far more important role in how
: > smooth the created surface will be, how well we can
: > 'sculpt' (Cadds term for using a surface to 'cut' or bisect
: > another surface or solid) and certainly how easily we
: > can NC the finished surface. By default, a lesser degree
: > nspline has fewer segments anyway.
: > >>>>>
:
: At least to the best of my knowledge......
:
: All intersection curves created in Pro/E (Pro/Surface, don't know about
: ISDX) will be degree 3 max (as will be all surfaces). Control vertex, knot,
: etc. count will depend on the file accuracy setting at the time the entity
: is generated. (Higher degree surfaces can be imported, maintained,
: exported. Curves are always converted to deg 3 max, or so it seems.)
:
: Curve CV or knot span (I'm assuming what you are calling "segments") / count
: doesn't have a direct effect on surfaces created from the curves. The
: surface CV count will depend on file tolerance settings. (Just for jollies,
: I created a typical leading edge curve set; 150 CV's inbd end, 15 CV's outbd
: end. A Boundary Blend between the two curves with an absolute accuracy of
: .001" produced a surface with 26 CV's in the U direction and nice, straight
: "element" lines, gaussian curvature of 2e-7. The same surface regenerated
: to an accuracy of .01" had 19 CV's and deviation from the original curves
: was .002". The curves were created in Rhino and surfaces evaluated in
: Rhino.)
:
: Guess what I'm getting at is that some of the problems you describe above
: shouldn't be problems in Pro.
:

Well, I'm lost and it isn't even just the highly technical discussion of wing
design and spline curves. It's the fact that I can't see, from the description of
the process, what all the futzing around is for. Normally, you'd directly use the
geometry which Pro/e imported ('Insert>Shared Data>From file') for your
manufacturing model. If you needed to modify the iges or whatever form the data
was in originally, you'd probably use one of Pro/e's built in tools for imported
surface manipulation. The shape and integrity of those surfaces and curves would
be verified using Pro/e's own very powerful surface/curve analysis tools
('Analysis>Surface Analysis>Analysis type [Gaussian, Porcupine, Normals,
Highlight, etc]). And the curve/surface would be manipulated with analysis on and
showing interactively the effect of any manipulation on the analysis.

So, where I would start with your plan to wing it, DaCrew, is with importing the
data into a Pro/e part file and doing some analysis of it. Decide from there
whether a bunch of intermediary steps is even necessary. Tools also exist in Pro/e
for splitting surfaces, extending edges, silhouette trimming and other methods of
parting halves, none of which require dividing curves at LE or TE. Think of it as
learning a new language where you can't directly translate: new vocabulary, new
systax, new thought processes. Don't immediately try to translate, just learn the
new language and see how it works to say what you want to say, get where you want
to go.

As far as resources for doing it on your own:
http://www.cadquest.com/
http://www.cadtrain.com/
http://www.frotime.com/
http://www.caddigest.com/subjects/pro_engineer/tutorials_proe.htm
http://www.proetools.com/surfaces.html
http://www.bitworm.com/detail/15669...ng_from_Solid_Modeling_to_Surface_Design.html
And, at least look for a community college with an educational license for Pro/e.
With your background, they might let you take the PTC authored surfacing course as
self study. Would be good to have this kind of background to do the above book.
One of the things a course will get you into, an essential for surface
creation/manipulation, is datum feature creation, especially curves, points and
axes.

David Janes

 

: Anyone know of good surfacing manuals or books for Pro/e?
:
Among the references listed at the end of my last post were some books (Cadquest)
and tutorials (Frotime & Cadtrain) and some freebees from CadDigest. The one book,
by Laceour, is a little advanced but puts it all together for when you're looking
past raw technique to thinking about process.

DJ

 

David,

Even if I end up utilizing a different method to construct the airfoil
surfaces, I will still need to cut sections through them for QC. So, how do
I go about creating 2D geometry using datum planes and surfaces. A previous
post mentioned that this was possible.

Thanks for the books and training links.

 

To create an intersection curve in the model; select one (or both) of the
intersecting objects, Edit / Intersect. For your particular purpose, try
just selecting the section plane and starting the command. Object selection
can be a bit tricky and if you have an inappropriate object included in the
selection set the command isn't available.

To create sections for section views; Tools / Model Sectioning. Oops, WF2
has moved it; go straight to View Manager.

If you have a maint contract there is a wealth of Suggested Technique type
articles on PTC's site. If you can't get at the Knowledge Base and are
using an eval version you might try to get your reseller to furnish some of
the more relevant ones.

Help (Global Search, in particular) is also very good.

 

:
: Thanks for the books and training links.
:

These links and resources are also the reply to your post "Machining in Pro/e". I
can't emphasize enough the resources PTC provides for learning their software that
they make available to qualified colleges through the "Universities Plus" program.
Colleges in this program have several PTC-authored courses on Pro/NC. For
information on colleges where your people can take these courses, contact Sr.
Educational Program Manager, Larry Fire.

Follow this link to the Cadtrain COACH curriculum:
http://www.cadtrain.com/coach_wildfire_curriculum.pdf

And I'm sure if you look on Amazon, you'll find one or two books on
Manufacturing/Milling.

David Janes