autocad geometry in solid edge

[fwm]

Hi

How do I bring in geometry from a .dwg file and use it in solid edge for either part of an assembly, or a part file.

Thanks.

fwm

 

[KENAT]

You mean using it to generate the sketch profile for protrusion/cutout etc?

Been a while but, back when I did it a few years back I'd open the dwg in SE draft. I'd tidy up the relevant profile a little bit, delete extraneous lines scale it if need be etc.

I'd then copy it, open up the part file and paste it onto the sketch for the relevant feature.

I'd then use the move & rotate commands and constraint commands to position it and then add any dimensions etc I needed.

These days Solid Edge has some better functionality for this kind of thing. I’d take a look at the ‘modeling parts from drawing views’ tutorial and go from there.

I suspect others here may be able to give more detail on how to do it in the new versions of Solid Edge. Knowing what version you’re on might help.

 

[fwm]

Thanks KENAT,

I'm using V19. I will look into the tutorial you mentioned, and monitor this and see if someone else has something to add.

Thanks

 

[onefjef]

Our company is making the transition to SE and have been using Autocad since R11. I use the same method KENAT uses to bring in sketch geometry. I don't believe there is a way to bring in .DWG directly to .PAR sketch.

I've become proficient at doing it this way so I haven't tried to find a better way.

One thing about ACAD geometry in SE. Sometimes tanget arcs to lines aren't recognized by SE so you have to apply a relationship to them.

Jef

 

[Wiemannironworks]

I have been suing AutoCAD and SE in conjunction with each other for th past year and a half. If I need to use a DWG file to produce a sketch for a PAR or similar SE file, I use these steps...

1. Remove all extraneous lines form the DWG file. All objects must be exploded if they are blocks and ungrouped.

2. Save the DWG file.

3. Open the DWG file suing SE and use DFT as your file type.

4. You should now have the DWG file open as a DFT file in SE.

5. Click on TOOLS in the drop down menu and select CREATE 3D. this willopen a small dialog box over the drawing, move it over so you can see what you want to use as a sketch. Then draw a selection box around the lines you want as your sketch and click FINISH in the dialog box.

6. SE will now open a PAR file and the selected lines are located on a sketching plane with in it. Clean it up, fillet out all your corners and you will have a viable sketrch from the DWG file.

NOTE: No matter how accurate your DWG file is, SE will not always connect corners and tangencies and must be manually done to the sketch before it will work as an extrusion. I work to 5 decimal places and SE still fails to completely connect the lines most of the time.

Is this what you were after?

 

[fwm]

Thanks for all the help. That is exactly what I was looking for. After further digging I found the tutorial that went through it step by step. If I get stuck on something again, I know where to come for some help.

Thanks again.

Dan