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
Reply to
SBC
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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 , 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.....
Reply to
Jeff Howard
: > : > 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 , 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
Reply to
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.
Reply to
hamei
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
"reconstructed"
'Tools>Model
segments/vertices.
Reply to
Da Crew
"Da Crew" wrote ....
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~)
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Reply to
Jeff Howard
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?
Reply to
Da Crew
: "Jeff Howard" wrote : > "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:
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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
Reply to
David Janes
: "Da Crew" wrote
: 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
Reply to
David Janes
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.
Reply to
SBC
"SBC" wrote....
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.
Reply to
Jeff Howard
: 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:
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And I'm sure if you look on Amazon, you'll find one or two books on Manufacturing/Milling.
David Janes
Reply to
David Janes

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