80-20 aluminum extrusion dwg import

Does anyone have any tips on importing dwgs into a sketch. I am
trying to import a dwg and extrude it. I am getting the dwg from
http://8020.net/ part number 3060.

When I import it and try to extrude it I get an error message saying I
have an open contour, no matter what the "merge points" setting I
have.

When I open the part in autocad everything looks to be a continuous
polyline yet in solidworks I get an open contour error.

Does anyone have any tips or tricks for importing a dwg into a sketch?

Thanks in advance
Troy

 

When I import it and try to extrude it I get an error message saying I

Damn those DWG's... ;-) The outer contour of the profile is not closed. Use
the Contour Select tool to find out where the contour is open (upper & lower
right corners). Zoom to the open gaps, select the endpoints and add 'Merge
Points' relation. Selection filter may be needed since the extreme zooming
can make it hard to hit the endpoints.

Hope this helps!

-h-

 

Love to help ya, but I don't download from any site that has e-mail as a

No registeration was needed at all to download DWG's.

-h-

 

Troy,

The drawings that they give you on 80/20 are junk,if you look close
lines don't even connect. I have built part of quite a few
80/20 components, let me know what you need and I will send if I have it.
For extrusions, I quartered the .dxf that they provide, repair, exutrude,
then mirror twice to come up with whole profile.

later

Andrew Grove

 

actually it is closed. i check in acad and it imports into inventor just
fine as is. it must be a problem with how solid works imports acad files.

check for youself if you have autocad. its a closed pline just like he said.

Matt

 

ok. found the problem.

the dwg has 2 arcs with very small dimensions right where solidworks looses
it.

the radius is 0.00000213

the solid works importer just ignores those arc so you end up with a gap.

i would erase them and re-close it in acad and bring it back into sw.

Matt

 

Couple options.

You could import the dwg then close the sketch. Start a new sketch and use
the dwg as a reference. Convert entities, make lines collinear and make
sure all the end point connect. Depending on the profile this could be time
consuming.

Another option I have found that works well is to open the dwg in AutoCAD.
Explode everything and then convert all lines to polylines. Save the dwg
and then import that into SolidWorks. If that doesen't close all the points
it usually gets about 90%.