Enlarging or continueing a surface
Enlarging or continueing a surface
(OP)
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.





RE: Enlarging or continueing a surface
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
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
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
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
www.nxjournaling.com
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
Tomas
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
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.
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
RE: Enlarging or continueing a surface
While on this particular subject, it might be a good idea to remember that the scan data more than likely isn't 100% accurate due to measurement error (which is usually small, if the scan operator and machine are worthwhile) and small errors or usage of tolerance in NX for the sake of surface quality may not drastically affect the end part (when it comes to seeing the physical parts side by side). I'd keep the scan data for an envelope reference, making sure as I rebuilt the part, I was "close" to it. Granted, this is all relative to what you're trying to achieve in the end - I just watched a co-worker make minute adjustments to surfaces that resulted in an assembly being off by more than an inch (over a length of 5+ feet), but Toost has you pointed in the right direction - as well as some of the other routes pointed out to you.
For your curves, the fewest number of segments and degree values of 3 (minimum for tangency) or 5 (minimum for curvature) would be the most desired if I am recalling my Shape Studio training correctly. The combs will be invaluable, as Toost as shown. Be prepared to create, refine and recreate - maybe more than one cycle.
Tim Flater
NX Designer