Problem with closed splines

[Anonymous]

I have a 2d map of a lake. The map have height curves.

I create a 3d map and use a closed splines for every meter.

The work method is:

1. I have a 2d picture in background.

2. Create a sketch on a plane.

3. Create splines that follow the height curve.

4. The spline goes around all the lake and attach were i begin. If i have luck the spline curve lightning yellow and i can use it to extrude or cut.

5. Sometimes or very often the spline will not lightning yellow when i close it and i can not use it for extrude or cut.

6. I save the file and exit.

7. Open the file again and now the closed spline curve lightning yellow?. When i try to extrude the spline it works but i get an error message. Se picture.

8. When i later try to use the extruded body, i can not use "combine and cut" tool. So the body is not ok. 

Are there any inspect tool i can use to find the problem with spline?

[Anonymous]

I can delete spline point until i make it work. The arrow show the point that create the problem. If i delete the point and create a line to close the all thing. It will work again. 

[jeff_strater]

That error message is telling you that somehow one of your spline points is no longer in the plane of the sketch.  Fusion allows you to move sketch points out of the sketch plane using the Move tool.  Did you use the Move tool at any point with this sketch?  Also, do you have "3D sketching" enabled?  If so, and if you have other model geometry in your model, the sketch tool can snap to geometry in the model that is not on the sketch plane:

For your workflow, make sure that this option is not enabled.

If you can share the design, we can take a look at it and see if we can tell what went wrong.

Another small, but helpful tip for your workflow is to use the "close spline" option in the context (right mouse) menu while a spline is active.  Choosing this will close your spline curve to the start point:

Please post or share your design if you need more help on it.

Thanks for posting!

Jeff Strater (Fusion development)

[Anonymous]

The 3d sketching is not enabled. I never use move tools on point, i click undo and create a new point because it`s faster.

This is the link to the file:

http://a360.co/1hAj4RV

It`s the same file that i have in the lower picture. Remove the last point and its working.

[Anonymous]

I still have problem to close spline. Can i sent a file so you can look at sketch?

[jeff_strater]

Thanks, @Anonymous.  Yes, we will take a look at it.  I was able to create some new splines in this design that do seem to work OK, but I am still not quite certain what the problem is with your spline.  It looks OK, but I suspect that there are some problems with it, I'm just not sure what those problems are.  Some of those points must not be exactly in the sketch plane, but I'm at a loss to explain how they got this way.  

We'll keep looking at it, though.  I apologize that we have not been able to get faster results to you.

Jeff

[jeff_strater · Accepted solution]

Thanks to @jiang_peng, who pointed out to me that the answer was right under our noses (or cursor 🙂 ).  There is a command called "Move to Sketch Plane" that will fix the spline in this case.  Here is a screencast that shows this working with your data:

Here is another screencast showing creating a new closed spline:

We are still not sure how this spline drifted from the sketch plane.  One possiblity is that I wonder about is the size of the data you are working with.  I notice that the units of this design are "meters", and the size of this design is very large.  We know that Fusion can have accuracy problems when the values get large.  Internally, Fusion stores data in centimeters, so if you have a point that is at 100m, that is internally stored as 10,000cm.  Which should be OK, but I could imagine that there may be some problems.  If you are willing to do your design as a scaled design (say 1 cm == 10 m, or something), you might have better results

Jeff

[Anonymous]

Thanks for all help and the screencast is excellent.

Yes the size is very big, Scale 1:1. When i later cut with the sketches i will get some face problem but it works. I can give you the 3d file later when i am finished.

/T