"Selecting" and flattening intersecting faces? 1

[cgwiita]

I have a model with intersecting pipes, and I'm having some trouble making a useful drawing so the pieces can be made. This is what I have:

What I'd like to do is "select" the visible part of the cylindrical face, with the outlines being the lines of intersection with the neighboring parts. Then, "flatten" the outline into something that would like this:

So the paper with the drawing can be wrapped around the actual pipe. Then the contour can be cut into the pipe. Is there anyway of doing this (using the intersection in the assembly)? Or will I just need to open the pipe models and cut them to the proper final shape with freehand 3d sketches?

Thanks for any help...

 

[TheTick]

You could possibly use the "Unwrap" feature in-context. Select the part to edit and you should get all of the "Part" functionality...

or...

Create the intersection curves in-context in the assembly and use those in the part file to do your unwrapping...

or...

You could copy (offset) the surfaces of the mating part in the context of the assembly to the part of interest, and cut the pipe with the surfaces...

I don't see a way to do it at the assembly level.

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[cgwiita]

Thanks Tick. That's what I figured would be the only way to do it. Unfortunately, SW doesn't want to convert the intersections between the pipes, either in the assembly or when editing the part in context. It looks like I'll have to use freehand surface-splines to draw the outline, and then "unwrap" that drawing. Unless of course, someone know how to convert the lines of intersection to a 3d sketch

 

[cgwiita]

And for that matter, even with a hand-drawn spline sketch, how would I "unwrap" it from the model? I can't think of a way to do it in the part or in a drawing...

 

[ctopher]

Or maybe use sheetmetal? Create the tube, extrude-cut the arc, flatten? I will try it myself later.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[cgwiita]

I've been trying the last hour or so with a sheet metal model, and have been running into different problems. I can sketch the contour with surface-splines, but cutting it is giving me problems. There's no way I know of the make a cut-extrude tangent over the whole surface (as in, setting the cut-extrude "direction" to be directly towards the axis). I can make a cut extrude in a planar direction (which means I can't cut the whole contour at once, I'll have to split it to three or more around the circumference) and then make planar cuts. In any case, I get an error when trying to unsuppress the flat model. I have a feeling its because the cut edges aren't parallel to the radius... is there some way to draw the contour around the body of the cylinder and then cut directly "in" towards the axis? I'd assume it would flatten fine then...

 

[CorBlimeyLimey]

Unless of course, someone know how to convert the lines of intersection to a 3d sketch

Start a 3D sketch, select the Intersection Curve, click on Convert Entities icon.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[cgwiita]

Limey--fantastic! I had tried intersection curve before and had gotten an error, I don't even remember what it was. Then I just ignored the function entirely. Tried it again and sure enough, it works fine. I've gotten the cut-extrudes to work too it appears...if all else goes well, I should have this done in an hour! Thanks everyone!