Importing file from AutoCAD

[cardiomed]

I have been trying to import a file from AutoCAD to SW, the only way this is done is the "drawing" format in SW and not the "part" file or format. This, I can work on 2D as drawing in SW but cannot exit to the 3D environment which is my ultimate goal, making a 3D drawing(or part) in SW from a 2D one in AutoCAD.

Hope I was clear, thanks alot.

 

[ctopher]

AutoCAD .dwg is 2D. Either create the part in a SW model from scratch, or use the 2D to 3D function.
Under Help is "Moving from 2D to 3D".
Also look into YouTube:

http://www.youtube.com/results?search_query=solidworks+2d+to+3d&aq=0

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[49again]

When you open the .dwg file in SolidWorks, the first dialog box that pops up "Select the method to open this DWG/DXF file:"
You can select the option to "Create new SolidWorks drawing" or "Import to a new part"

Select the latter.

Steve R.

 

[cardiomed]

Thanks Steve,

That worked out! one more question if you have time, this drawing is about a 'tray'(where some components/items are supposed be placed in this tray after being manufactured). Now I have the 2D drawing of this tray imported to SW and I need to make it 3D in different depths for different components/items. The tray's material is some sort of PVC and its thickness is constant for the entire tray.

Do you think I should use the sheet metal feature to do the 3D design although its shape is sort of complex?

I'm uploading the SW 2010 version of the file in here in case you wanna have a look.

Thanks alot,

 

[MikeHalloran]

The sheet metal functionality works best for actual sheet metal parts, cut and folded from sheet. It will work less well for the sorts of things you typically do to PVC, even if you do start with it in sheet form.

Instead, try shelling a surface.



Mike Halloran
Pembroke Pines, FL, USA

 

[49again]

cardiomed -

Yeah - what Halloran said. Use a shell. But first....

You'll notice the SolidWorks sketch you've got has several heavy and thin lines. That's because you've got multiple closed loops. So, start your Extrude command, and then you can pick "regions". Pick the outer contour for the initial extrude, then for Extrude-Cuts at your different depths, turn your initial sketch to "Show" and pick from your multiple closed loops.

 

[CorBlimeyLimey]

cardiomed ... If you have (or can get) the models of the products, you would be able to use the Indent function. That would drastically decrease the design time of the tray.

http://help.solidworks.com/2010/Eng...eatures/example_of_indent_drill_packaging.htm

Here's a a more helpful video tutorial;

http://gabijack.com/2008/12/new-featured-video-indent/

 

[cardiomed]

Thank you all, good points,

The point is the software I'm working on its 'shell' feature is dis-active, I'll have to find a way.

Also, if you look at the side view of the finished tray its bottom part/surface has the elevation of 0.00 and its highest part is 1.00(in)from the bottom surface. The depth of different compartments change according the products shapes; however the thickness of the tray has to be constant. Yeah, the indent function idea would have been amazing but the 3D models of the products are not available.

 

[CorBlimeyLimey]

cardiomed ...

You have the profiles of the parts, and I assume you must know the depths and recess shapes required. That information should be enough to create simple dummy parts (multi-bodies) to be used with the Indent function.

Once created, a DT could be used to control the different configurations of the dummy parts. That in turn would create the required configs of the tray.