Profiles of Complex Geometry

[Airmack]

I am fighting SolidWorks to create boundaries of the profiles of complex parts within a .SLDDRW file.

I have been semi-successful in being able to hide tangent edges and select SOME profile edges, which are then bilaterally offset to make the profile boundary. Unfortunately, there are some edges that are non-selectable (usually revolves or fillets).

Is there a way to generate a stable profile of a part that is selectable?

(I have looked into split lines - but it is unknown exactly where a peak will occur on the profile, thus it is unknown where to exacly place the split line. Am I on the right track looking down this path?)

 

[Theophilus]

Are you creating loft sections within the context of a drawing (instead of within a part or assembly)?

If so, I do this within a part. Insert planes where you want them, then use the Intersection Curve tool within a sketch to generate a profile where the sketch plane intersects the part. you can then offset the profile by whatever amount you need.

If this isn't what you're looking for, you may need to ellaborate.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[Airmack]

Thanks for getting back so quickly...

I'll take a step back... I am trying to create overlay templates for inspection of these complex parts on an optical comparitor. There are some profile callouts on the print that reqire me to offset them X amount, bilaterally, creating the visual boundary for inspection.

In my attempts, I have imported a view from the part file and then proceed select the outer profile edges and offset them. Some of the profile edges are non-selectable - which are usually lines derived from the edge of a fillet, revolve, or similar surface.

Perhaps the Intersection Curve Tool may be the direction to go, but I am unsure where to exactly place the intersecting planes to cross the part at crossections that will represent the physical view of the part under the comparitor- (maybe this is my discovered problem?).

 

[SBaugh]

I think you are confusing the idea of a drawing to a model. You cannot create geometry like you would within a part. How about you build a profile in a part and place that into your drawing?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Theophilus]

OK, that makes sense. Sounds like you only need the outer profile of the part from particular views. The suggestion I had may not work for what you need--it depends on the shape of your part and whether the profile can be had within a single plane. The Intersection Curve feature does a great job of converting any geometry into sketch form as long as it intersects your sketch plane.

In your case, you could probably try it and use it where you will get a true profile of your part--then offset the sketch geometry to the inside and outside--and then convert the original inner profile to construction geometry (dashed lines).

One thing you can do (again, depending on part geometry) is to extrude a surface through your part--much like a jogged section line--and use the surface (which can have multiple line segments) to generate your profiles where the surface itself intersects your part geometry. So you can deliberately make your profile accurate with this method by careful line placement to extrude your surface. From this point, select the Intersection Curve feature (even though you haven't started a sketch) and then select your extruded surface, and then the faces that intersect your extruded surface. The result will be a 3D sketch. From this point, you can offset the sketch geometry once you get into a drawing view, or use your Front, Right, or Top planes to create a 2D sketch and merely convert the sketch entities from your 3D sketch. Offset inside and out, and you'll have your needed profiles, including radiused edges.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[J-C]

What about a section view with the Surface cut only option? Then hide the parent view if you don't want to see it.

As for hiding edges and some not being selectable, trying right clicking the view locking the focus. Usually you can select them then.

Jason Capriotti
Smith & Nephew, Inc.