Enlarging or continueing a surface 1

[JChurch77]

I have a surface that I would like to enlarge keeping obviously the same general shape. It is a surface off of a parasolid that was imported so it is a dumb solid. When I use ENLARGE option it gives me an undesired shape. What would be the best and most efficient way to do this? Curious to see how others would attack this. See attached. Thank you.

 

[jnikolauk]

I always start with extracting the surface and then I go to edit-surface-boundary-remove trim. Beyond that I'd have to know what the surface is for and the size and the deviation you're comfortable with.

a quick "cheat" I often use when a surface gets a major twist in it is trim the surface a little short (before the edge starts to curl (often takes zooming in real close)) and then insert-surface-extension-tangential

 

[jnikolauk]

Sometimes enlarging the surface after trimming it a bit works as well.

 

[JChurch77]

Those are some options I just tried, good ideas for sure. I think I may need to construct lines off this surface though and create mesh surface to get a clean extension in this case. The geometry it creates is not desired.

 

[Toost]

I had a look at the surface and it is no pretty sight...
This simple shape is "overloaded with data", in numbers:
it is a degree 3x3 which is OK but then it has 32x60 patches which is way beyond what is reasonable for this shape. ( it is also visible when looking at the file size on disk.)
Depending on what NX licenses you have access to there are different info features and cleaning procedures that can be used.
To check the overload : Information - Object, select the face ( not the feature / body)
To see the patch boundaries Information - b surface, Show patch boundaries
( and output to listing window)

Refresh and re-run but turn on "Show poles" instead of show patch boundaries.

The problem that becomes visible when using the enlarge feature does already exist in that mass of data, imagine that you have a very small ripple in the shape and that you extend the shape in the natural directions, then that ripple will grow the farther away you go.


The proper way to proceed would in the ideal world be that you ask the supplier for a clean surface, which this is not.
In case you want to continue with this surface you need either clean the surface or build a new which is "similar but better". In this case one can create, say 4, isoparametric curves of the sheet, clean these curves( reduce the number of segments, target 1 or 2 segments) then create a thru curves sheet.

If you have the license for it, the surface can be cleaned with the Edit - surface - refit face, but you ( and your customer) need then to accept that the final shape will not be 100% identical. The question is how much deviation you can accept.

Regards,
Tomas

 

[JChurch77]

Yeah, interesting information Tomas, this shape was generated from 3D scanned data to produce a solid model. Thats probably why its a "mess". If my surface modeling experience was a bit better I would recreate this as close to the shape as possible but better. I am going to try to see what I can do to clean it up, good learning curve I imagine.

 

[jnikolauk]

Not that I usually have the luxury to ask for a better surface from the supplier but that info should come in handy

 

[cowski]

After you remove the trim (as jnikolauk suggested - also, use the 'edit a copy' option, keep the original surface for reference and deviation checking), use X-form if it is available to you. With this command you can easily change the number of patches to something reasonable. You may also be able to move poles around to get a workable extension. If you move the wrong pole or go too far, hit undo while still in the command; it will only undo your last move.

http://www.nxjournaling.com

 

[JChurch77]

X-Form is not available to me, another good idea though. Thanks.

 

[Toost]

reply regarding the "ask for better data", i have seen a few cases where "company A" buys a design from a designbureau, where the designer creates something that looks wonderful rendered but cannot be manufactured in probably any cad/cam system. I remember one case where a long discussion started about if the data from the designbureau should be reusable or not... ( My humble role was to tell if the surfaces were ok or not.)
Tomas

 

[JChurch77]

Well, I was in charge of creating these solid models. I had a physical part in my hand, had it 3D scanned and then made it at least symmetrical down centerline using bridge curves after I split it. So, with my limited surface modeling experience this is where I am at with them. I did have our cad/cam department check out the geometry and it can be cut efficiently but I do believe the surfaces could be much better and allow me to enlarge it to produce an extended surface.

 

[jnikolauk]

At this point I'd reccomend rebuilding the surface with cleaned isoparametric curves as Toost suggested. It should be reasonably close and result in a surface that can be expanded.

 

[JChurch77]

Could one of you show me how you would go about creating a new model using Isoparametric curves (4) to reconstruct this. maybe a simple surface created similar to this shape would be help for me to disect it in part navigator and pick up some pointers. I would really appreciate it, thank you.

 

[Toost]

In NX version ?

 

[JChurch77]

Im using NX 7.5 thank you....

 

[jnikolauk]

to get the curves go Insert-curve from bodies-extract...-isoparameteric curves pick your surface and enter the amount of curves and there you go. As far as simplfying the curves you could try smooth spline or any number of the spline editing operators (if you're lucky just rebuilding from the iso curves might work well enough for you) I don't have any set pattern as far as curves go. Perhaps someoene else can fill you in better.

 

[JChurch77]

Wow, much better surface created using isoparametric curves, create new clean spline from points off those then through curve mesh....very nice and close to original shape but better.

 

[Toost]

Here's how i would have proceeded.
1 inspect the original according to above, if the shape or data mass is undesirable, then:
2) remove the surface trim ( trimming of surfaces is a separate operation that can be deleted even on imported models.) Edit - Surface - Boundary - edit a copy - remove trim.
3) depending on the shape the next steps cold be different but in this case i would create isoparametric curves as seen in the attached picture.
The Iso parametric curves will have the same "math" as the underlying surface, which in this case means that the spline has 60 segments. ( =way to much)
4 ) a simple way to clean splines like these is using the "Fit Spline", Insert - curve - fit spline, then click the button "edit spline" - pick the spline and either fit to a "degree and tolerance" or "degree and segments"
In this case i would assume that i can achieve the shape using degree3 and 3 segments, - the curves are kind of flat in the ends. Note that you get "fitting errors" reported in the bottom of the menu ,- -do not press OK or apply until you find the result you desire, try different tolerances / number of segments etc and press Apply when ready.
( Zoom in on the spline, the new shape will be displayed whilst editing, and use the curvature comb to see the real shape.)
5) maybe a small manual pole edit ( double click the spline or use x-Form) is needed to change the shape in the ends of the respective spline.
6) create the surface.

 

[Toost]

should have been 2 pictures above, here's the second.

 

[Toost]