I'm desiging a part for my friends small business and she wanted me to put her Logo on it. She sent me a DWG file of the logo. I imported it to my part and it automatically centered it right on the origin, which is not where i wanted it. After the most roundabout way possible I got a sketch of her logo that looks perfect and is exactely where it is supposed to be, but when I go to extrude it, NX says my input selection is invalid, but gives no reason as to how it is invalid. My process went like this:
1. Import dwg file to curves which center themselves on the origin
2. Use "copy existing geometry" to turn those curves into a sketch (uses splines)
3. Copy that sketch and pasted it on the surface where I want the logo
4. Used "scale curves" to scale that sketch down to the right size
5. Used the move command under the right click menu to move the scaled curves to the approriate location
6. Used the "copy existing geometry" command (again...) to turn those curves into a sketch again.
7. Used the auto-constrain feature to constrain the sketch.
8. After doing all of that I deleted everything except the final sketch.
I realize there are probably about 1000 ways to do that better than I did, but at my new job we use Creo and i havent used NX in a while. Maybe its the process I used, maybe not. Either way does someone have an idea of what is wrong or perhaps a more direct way to do this?
If it helps I had the same error when trying to extude a sketch with like 15 hexagons (mimicing a bee honeycomb). I cut the number of hexes in half and it worked fine.
Solved! Go to Solution.
If i guess, you have double curves and maybe other issues that came with the import.
Try to extrude area by area instead of all at once.
This is where Ryans tip comes in, when the Extrude dialog is up, you have different selection options above the graphics window, try for example "connected curves", if there are multiple curves on the same spot, the search mechanism might go back and forth on these.
There is an option in the sketch "Add existing curves" which will let the sketch "adopt non-sketch" curves.".
Instead of scaling the curves, Could you make your solid body from the sketch, then scale your solid body. Do you get the errors before you do the scale curves?
From what I've seen over the years, Autocad geometry, when imported into NX,has issues.
- curve endpoints don't match
- tangent arcs aren't tangent
When you first import the curves into a sketch,
1) Make sure the sketch is on a different layer than the curves.
2) Select the curves ONE BY ONE (single selection, no "connected curves", etc.), making sure there are no duplicates.
3) Turn off the layer with the original curves
4) ZOOM IN on the sketch, and make sure the endpoints are coincident, arcs are tangent, etc.
Then try to extrude the sketch.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
Here are a couple of exaggerated, common cases where the alert "The input section is not valid" is raised. In both cases the sketch is fully constrained, chaining selection does not identify any issues and Optimize 2d Curve does not make any corrections. In these cases you may have to resort to using Curvature Combs to detect inconsistencies. Turning on 'Stop an Intersection' may also help (though not in these rudimentary examples).
I'm going to play devil's advocate here a bit....
Why are those not allowed with Extrude but allowed with a warning that the strings self-intersect when using a Ruled Surface? The resulting surface should be close to the same as an Extrude, shouldn't it???? Seems a bit inconsistent to not allow it with a warning about the self-intersection particularly when there is a specific Customer Default that should allow it with Extrude as well as other commands.
NX 188.8.131.52 MP11 Rev. A
GM TcE v184.108.40.206
GM GPDL v11-A.3.6
I encourage that you play devil's advocate
This is actually one of two cases that the Extrude Self-intersection Customer Default does not support. They are referred to as "Y" and "a" configurations, and covered under existing ER 7305433. There is only one other feature that I could find that has a similar CD, and that is Variational Sweep.
As far as inconsistencies among remaining features, I found that Swept allows self-intersection (but warns the user once a guide is selected) but Through Curves refuses to even allow the selection. I can't explain why one works and not the other but perhaps if you open an IR with GTAC they can investigate further for you.