problem with greating dwg 2D to 3D

[emc2673]

I am in the middle of converting from Solid Edge to the world of Solid works for a job opportunity I have been practicing with Solid works but have found some problems.

I have imported a 2D .dwg profile into solid works part and I just figured I could select certain profile sketches and create a base and use the exsisting sketches as references for cutouts, etc.... It so happens that it doesn't work out that way (like Solid Edge) any advice on creating a milti dimensional profile part (I have gone through the tutorials and they proved to be no help)

also, Does SolidWorks have object snaps similar to AutoCad? such as mid point, end point???? etc.

Lastly, is there a way to create a sketch and then "project it to another plane??

Thanks in advance,

EMC

 

[Theophilus]

The 2D DWG file might be riddled with overlapping/redundant lines. SW needs non-overlapping entities from which to extrude and create features. That might be the problem you're having.

In SW, you do have some of the snap feedback. When you select a point, it's the point. You can also create associations between a midpoint of a line and a point of another line. It's just formatted differently from ACAD.

Yes, you can also project one sketch to another--check out the curves toolbar. You probably want to project a sketch, as the feature says.

If you're just starting out, I recommend doing all the tutorials completely, then picking a particular project to model and refer to the help for trouble getting what you want. For such a complex program, the help files are very well done.

Good luck.




Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[Mandrake22]

Another way to project an initial sketch to a new sketch plane: Select or create the new plane, open a sketch, click on any segment of the sketch you are wanting to project and then click the "Convert Entities" button on the sketch toobar.The selected sketch segments will then be copied (and projected) to the new plane. If you want to project the entire initial sketch to the new plane, click on the sketch entry in the feature manager and then the "Convert Entities" button.
This technique works very well when dealing with an imported 2D sketch.

 

[DHALE1]

Another way to copy sketches to sketch planes would be the copy/paste function. You can control select the lines you want from the 2d layout, and under the edit pulldown choose copy. Then set up a sketch plane, go back to the edit pulldown menu and choose paste. This will paste the sketch onto the sketch plane. You could do this in the same document, but you can also copy/paste to other documents. The copy/paste is just like word or excel. Many times I will have a imported 2-d layout open and a part model open. Then I copy lines from the layout, use control-tab to toggle to my part file, and paste the lines to a sketch. The sketch needs to be moved into the proper position. To do this I use the "modify sketch" command under the Tools pulldown menu and Sketch tools. Once the lines are moved into the position I then add relations and dimensions to the sketch, and perform the extrude, revolve, etc.

Also, if you want to use what you have, you can try the "repair sketch" command. This will clean up your sketch, so you can use it for a feature. use this before putting dimension or relations to your sketch. You can find that under the Tools pulldown menu and under sketch tools.

 

[rporter]

emc2673

I beleve what you want to use is the 2d to 3d feature to create a solid from a 3 view 2d drawing. Look in help topic 2d to 3d.

 

[stanp]

Hi
to avoid overlaping entities from .dwg to SW sketches, u can use Rhino3D V3, in which you can select duplicates (at least).

also beware of using acad splines : SW2003 dont read them...
Good luck

 

[JNR]

OK I have a different view of this issue - surprise, surprise!!

First from your description, I think you need to go through the SW tutorials and take a class. Fully understand the differences in the modelling approaches of the two systems. Never try to relate a new CADsystem to the methods used by an old one.

Second. I strongly believe it is faster, less painful and more useful in temrs of database strucuture to just 3D model the things from scratch by looking at the old prints if you have no 3D models you can convert.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There's no place like 127.0.0.1

 

[macPT]

Again, I agree with JNR 100%.

My company as many legacy data in ACad. When it's appropriate, we convert this data into SW. I've tried to use 2D to 3D tools from SW,only to quickly find out that we should create the new parts from scratch. ACad data can hide so many problems that it's more productive and safe start all over in SW.

Regards

 

[rocheey]

We've been using SW for years, but are still stuck with legacy Acad data.

One way to locate overlapping stuff in acad is to make your geometry into closed polylines...

Make a Polyline out of your boundaries, and then attempt to CLOSE it. If you see acad draw an extra line from out of the blue, it is showing you where a gap in your geometry is.
if you dont see acad drawing any extra lines, click the newly created CLOSED polyline and make sure all the entities are in there.