Simple loft feature failed again.

Greetings;

I wish to create a simple loft consist of two cicles profiles along an
spline guide curve as shown similuting the curve of the fingers that
will rest on this feature. Unfortunately I receive an error message
"Guide curve No. 1 is invalid. It does not intersect with section No.
1" I did constraint the center of each cicle to coincide with the
Spline endpoints. Am I still missing something here?

I also realize that there isn't a loft feature for a cut. It's only
availble for a boss. If this is the case, how would you create a loft
cut?

Does anyone have a fail-safe technic that would guaranty a success
loft?

Thanks for your time and help.

Paul

http://home.comcast.net/~wangphk/SolidWorks/Parts/Another-Loft-Failed.jpg

 

Actually there is a Loft Cut feature, it's just not on the toolbar. You can
add it by customizing your toolbar and adding the button.

Richard

 

"Guide curve No. 1 is invalid. It does not intersect with section No.

Double check that the sketch planes for the circles really DO intersect
the guide curve.
A quick check might be to try using a pierce constraint instead of a
coincident constraint. If the pierce fails you can be ceratian your
sketch plane does not intersect the guide curve, just as SWX is telling
you.
Also, measure the distance between the end of the guide curve to your
sketch plane.

I am willing to bet that the problem is exactly what SWX is saying the
problem is.

 

Thank you all for your help.

Sorry, I completely forget there is an "Insert" menu feature.

I did check the plane that I am sketching on. It is perpendicular to
the endpoints of the Guide curve. I create the sketching plane using
the Insert - References Geometry - Planes - Normal to curve and Select
the Guide curve near its endpoint.

For some reason, I don't have a Pierce constraint. All I have is
Concentric or Coincident. Am I missing something?

 

: Thank you all for your help.
:
: Sorry, I completely forget there is an "Insert" menu feature.
:
: I did check the plane that I am sketching on. It is perpendicular to
: the endpoints of the Guide curve. I create the sketching plane using
: the Insert - References Geometry - Planes - Normal to curve and Select
: the Guide curve near its endpoint.
:
: For some reason, I don't have a Pierce constraint. All I have is
: Concentric or Coincident. Am I missing something?
:
You are probably missing the pierce point. Put a point on the section sketch, then
establish a relation between the path curve and the point. You should get the
'Pierce' constaint in the list. Be sure to delete the existing concentric
relation.

David Janes

 

You could always try the 'Centerline Parameters' option instead of
Guide Curves.

Mike Wilson

 

Thanks, Mike, the "centerline parameters" works beautifully. I wish
that I know this option earlier.

Intead of inserting a sketch point to the circle circumference, I
sketch a centerline from the center of the circle to the
circumference. This allow me to have the Pierce constraint option.

Once again thank you all for your time and help.