What is a valid section view snap point?

steve_maietta

Hello, I am drawing some plans with section views and trying to put the section views where I want them, but can only drop them where the orange box appears.  They are forced to certain points.  How can I define these points myself?  I tried adding points in a sketch, but couldn't use these points in my drawing view.

thanks for any pointers as to the behavior of the section view tool.

~Steve Maietta

brucebartlett

Steve, looks like you got a result, however my intent was to create snap points without the extra parts and a assembly by just split 1 face. 

john_mccullough

Bruce's method works well because it generates separate edges along the top edge of his model. Even though those model edges are still splines, whihc become polylines in the view, the end points of each of those polyline edges are valid associative snap points in the drawing. 

john_mccullough

A section view cutting plane line can only be associated to an end, mid, or center point on edges on specific entity types - basically only lines or arc/circles. It can be difficult to tell which edges in a view are actually line or arc entities. This is because all spline and ellipse edges in your model project to polyline edges in the drawing view on which Onshape can't create an associative reference point. Most likely the view edges you are trying to place the cutting line on are generated from curved edges (splines and ellipses) on the model. 
Currently the best work-around for this is to place the cutting plane line "in space" near the location you need it. It will not be associative to the model, but should allow you to create the section view needed.  This type of cutting plane will stay associative and move with the view. 

steve_maietta

Thanks John..
  So I tried what (I think) you meant.  I created a sketch right along my model but not actually part of it.  This sketch was 4, 2 inch line segments one after another.   (I'd like to have a section view every 2" in my drawing)  I went back to the drawing, regenerated the part and still can't snap section views to these points. Hmmmmmmm...?  What exactly does OnShape look for to find a snap point?  

(Edit - I moved the sketch so it is on the actual part, still no snapping)

~Steve
 
May be useful to be able to dimension where the section view lies, like how we dimension where lines are in sketches.

brucebartlett

Steve you could try splitting a face with a plane on the model in the the part studio at the points you want the section's, this will give you a point to pick on the drawing. Not ideal but should work, will just mean you have some extra splits across your model's face but will not change the geometry. 

steve_maietta

Bruce, I have planes running along the model and would like to use them as section snap points but it doesnt work..  Also I have a line that I drew as a sketch on the top surface of the model and put a few points on in hopes of snaggin them as snap points, no luck either..

Heres the file (Public) 

https://cad.onshape.com/documents/4a3090c111204005a035c899/w/c0478464d35e42f282b61dad/e/e1c01e32f68c409c8bc1c3b3

Hull 2 is the part and Hull Plans is the drawing..  Anyone care to give it a shot?  Create a section view every two inches?

thanks

~Steve

_Ðave_

Steve

 I split the hull @ the planes then created an assembly from those parts. With a drawing from the assembly you can create a section view at the end of each part. Here's a link. HTH

steve_maietta

Cool Dave, thanks for your time!

~Steve

brucebartlett

Steve, looks like you got a result, however my intent was to create snap points without the extra parts and a assembly by just split 1 face. 

john_mccullough

Bruce's method works well because it generates separate edges along the top edge of his model. Even though those model edges are still splines, whihc become polylines in the view, the end points of each of those polyline edges are valid associative snap points in the drawing. 

_Ðave_

@brucebartlett That works quite well, Thanks.