Dimension to a silhouette edge

[dgs]

(Asked on the SolidWorks forum, but no good answer yet, so I thought I'd try here.)

I need to create overall dims on a drawing of a complex form. Most,
if not all, of the outside edges are silhouette edges and SW won't
allow me to dimension to them. It suggests that I create a silhouette
split line to dimension to. I tried that, but the split line removes a portion of the geometry.

How can I create these dimensions?

I
know it's a bit cryptic and a part file would help, but I can't send
this customer data over, sorry. This isn't what I'm working on, but
imagine trying to create overall dims of orthographic views of these headphones:

 

[c_thompson_68]

Doug,

Here are some options that come to mind:

<ul>[*]Add points inside a 3-D sketch, and dimension to those points.[*]The split-line should work, but it breaks-up the surface which I do not like unless I am applying boundary conditions for FEA[*]Add driven dimensions in the original sketch if possible, then show annotations in drawing (similar to Pro-E)[/list]Otherwise, post a simplified example of a part type that you wish to dimension. It could also be a bug as SP 3.0 would not permit the creation of a sweep for 64-bit OS. This was corrected after I upgraded to SW 2009 SP 4.0

Chris

 

[dgs]

Not sure what SP we're running here, I may check that.

The problem with #1 is I'd still want to tie those points to the 3D geometry, is there a good way to do that?

The split line worked OK, once I redefined the sweep. The problem there is on certain geometry it was challenging to figure out the right plane and surface that will provide a vertex at the right place. And you're right, splitting the surface is an undesireable side effect.

I posted a simple model to the SW forums (linked above) if you want to look at it.

I'm surprised at how difficult this was. I've had the occasional challenge like this in Pro|E, but never this widespread.

 

[c_thompson_68]

I posted a model and response to this SolidWorks forum: https://forum.solidworks.com/thread/25536



"Look at the attached file, I think I found the solution you where
looking for. I created a split line from two intersecting sweeps (zero
twist), than coverted edge in a 3DSketch for the silhouette line.




Points
where attached to the silhouette line using a 3DSketch. I did attempt
to add points through reference geometry, but I was not able to
dimension to the points in the drawing. The point tool in SolidWorks is
not as Versatile as the DTM PT tool in Pro-E."

Regards,

Chris Thompson
www.appianwaytech.com

SolidWorks Premium 2007 & 2009
Pro-E WF 2.0 & 3.0


Edited by: c_thompson_68

 

[mjcole_ptc]

Doug,

If you don't want to split the actual model faces you can apply the split on an offset copy surface created using distance=0

Regarding the Point Tool I (3/4) heartedly agree.
You can do 21 points on curve but then you get 21 separate points with distance along curve values. Points Datums Curves and Surfaces cannot be patterned as features. I guess they are not considered worthy of that function.

Points also cannot be properly referenced from a sketch as they can in ProE (Should we change the short name to "ProW" for wildfire?)

MAny types of points can't be created. My favorite is Intersection of Axis and Plane -maybe in 2012 it'll be possible- funny that in a 3D sketch a point Axis and plane can be selected for Intersection constraint. Also intersection of circle entity or edge with plane is not possible
because there are 2 solutions an [other solution] button would be nice.

Most of the time a 3D sketch works better for points. If you want the Offset from Csys option like on Pro/E you can dimension the sketch points from Def Planes to achieve this.

Michael