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Start a sketch in an assembly, click on the edge you want then convert entities.
For a few lines it is possible, but the problem is I want convert the edges of a complex sub-assembly (with more than 1000 parts and sub assemblies). To select each edge of it is a lot of work!
The reason why I want to use a sketch is to increase speed; when we engineer a new machine, we need other sub assemblies to determine where machineparts can be located. By using a sketch of those subassemblies instead of the complete model, Solidworks doesn't need to load all the parts of those sub assemblies.
I don't understand your complete intent for creating the sketchlines, it sounds like you might want to try things like"lightweight" for all your subassemblies. This willload the geometry, but not the features behind it. If doneproperly, large assemblies will load in 15 seconds (orless) lightweighted.
Open the assembly file, right-click and edit part, open a new sketch on the part face, convert entities on that one face (which can become your top/right/front view later). Open the part template file, paste the sketch. You can select all converted edges with window in the assembly file and perform CTRL C function. to copy entities. Then, in the part file, select the face you want the sketch to appear on, insert sketch, paste the entities using CTRL V. On your 2D to 3D toolbar in you part file, you can select the sketch and then select the "extrude" button. you can use the "align sketch" button to align the sketches so that the top and right side line up, for example. If you don't select the view before pasting the sketch entities, then you have to select the "front" view button on the 2D to 3D toolbar to add certain entities to the front plane.
This sounds like alot, but is actually alot easier and faster than saving as dxf....as you mentioned earlier.
Hope this helps!
Yes, I mentioned editing a part within the assembly and then converting entities above. You actually don't have to edit a part. You can insert a sektch directly in the assembly and convert entities that way, as SolidAir has mentioned.
You could also save the assembly as a part using the Exterior faces Only or Exterior components option. That way the full 3D effect is maintained, not just a 2D profile.
Or if you really prefer the 2D approach;
Select the drawing view
Use the Edit > Copy to DWGeditor function
Paste it into DWGeditor
Copy back to the SW model.
But I prefer Charles method of using the assy model in lightweight.
To expand on what Kelvin just posted. If you *really* want toget the sketch information as lines... you can:
Open the assembly.
Save As... then select .sldprt. save it with all thegeometry
Open up the newly saved .sldprt
Start a 3D Sketch.
Press F5, then select the second option, which is"Lines"
Now do a drag-select over the entire "part", which willselect every line.
Click on "convert entities".
You will now have a 3d sketch of every edge in the oldassembly.
-I haven't actually tried this, but I'm pretty sure it willwork.
Save your original (.sldasm) this defines your limits for your machine as a (.sldprt). Then insert that (part) into you new machine (.sldasm) as an envelope.
This will give you an envelope to work inside of that is a "transparent shell" representation of your original (.sldasm) and will be very light on performance.
Charles, great thinking! However, if you have a curved surface, such as a pin diameter, the drag window select will not grab those as sketch lines to convert. Something to note.
Personally, I like the lightweight option best. Solidworks will load large assemblies quickly that way.
Thanks for your advise.
I've used lightweight, but there were too many negative issues when I used it.
I'm busy right now, but when I've more time, I'll try to save it as part and insert it as an envelope part.