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Finding intersection point between to curves fails

Genius
Genius

I'm attempting to create an extrusion on a face of an object and want to set the origin as an intersection of two edges.  Why is it that sometimes this works without any problems, but then I'll try it again for another extrusion and it fails (No intersection point found)?  I have attached a file showing what I'm trying to work on.  The "X" indicates the face that I'm wanting to create the extrusion on.  The two hilighted lines are the two lines I'm trying to find the intersection of.  Sometimes it works, sometimes it doesn't...  Thanks

6 REPLIES

Re: Finding intersection point between to curves fails

Siemens Phenom Siemens Phenom
Siemens Phenom

Assuming that edges are coplanar.

Menu > Insert > Datum/Point > Point. 

Set the selection filter to 'Edge'

In Point dialog, select type as 'Intersection Point' which will create the point (check associative option under settings) that you can use as a reference.

 

Re: Finding intersection point between to curves fails

Genius
Genius

OK, that was a good thing to check.  I didn't create the initial part, so I thought these two lines were coplaner, but they aren't.  While trying to set the origin, I had also tried to set it at the intersection of a line and a plane, but that didn't work, either.  The attached screenshot shows what I tried to do.  I thought I was able to get this to work before, too.  Thanks

Re: Finding intersection point between to curves fails

Siemens Phenom Siemens Phenom
Siemens Phenom

@s_hightower wrote:

OK, that was a good thing to check.  I didn't create the initial part, so I thought these two lines were coplaner, but they aren't.  While trying to set the origin, I had also tried to set it at the intersection of a line and a plane, but that didn't work, either.  The attached screenshot shows what I tried to do.  I thought I was able to get this to work before, too.  Thanks


With the same 'Point' command, you can create a point using the face as reference. Select the type as 'End Point' > Select the required edge > In 'Offset' select Offset Option as Rectangular > Now for Delta X value, use measure (Measure Distance command) with the projected distance between the end point of that edge and face.
point.PNGAnother option is to use 'Point Set' command. Create a datum axis along the edge and a datum plane along the face. With 'Point Set' command, type as 'Intersection Points' select the datum plane and datum axis which will create an intersection point.   

point1.PNG

 

 

Re: Finding intersection point between to curves fails

Genius
Genius

Thanks for the info.  One question with this.  Is there a setting that I can change that will make the plane and the edge "infinite" so that if a line or edge is perpendicular to a plane, an intersection will be found?  Right now, it seems that the surface and edge are bound by the edges in the surface and the ends of the edge.  Does that make sense?  I'm not sure if I've seen that in NX or another CAD software that I'm used to using.  Having that setting is a lot more user friendly to have instead of having to create 2 more other features than just being able to select an intersection between two infinite (not bound) objects.  Thanks

Re: Finding intersection point between to curves fails

Siemens Phenom Siemens Phenom
Siemens Phenom


Is there a setting that I can change that will make the plane and the edge "infinite" so that if a line or edge is perpendicular to a plane, an intersection will be found? 

No. Planes and axes are itself considered as infinite and in NX you can adjust the length,height of a datum plane and length of an axis by dragging its arrow tip.

 

@s_hightower: Are those options not sufficient to fulfill your purpose?

 

Re: Finding intersection point between to curves fails

Genius
Genius

I could be wrong, but I think a different CAD system that I worked with did have the option of the edge being able to be considered infinite for situations like this.  It's been awhile since I used it.  I do know that in NX I can create the axis to be co-linear with the edge and then get the intersection between the new axis and the plane  It would just be convenient if I didn't have to do the extra step of creating the new axis (instead of using the original edge).  Thanks