I am importing DWG file created in Autocad 2000 in to Solidworks. Is there any way to maintain the Solidworks tree? Or will I have to redraw every drawing?
Rob, you can import your AutoCAD dwg files into Solidworks drawings. Couple of notes:
Solidworks doesn't import paper-space viewports so you're not going to have a tree structure like you do with a Solidworks drawing.
The AutoCAd drawing layers will import so that you can control visibility. Layers do not work on a per-view basis in Solidworks like they do in AutoCAD paper-space viewports. (in case you didn't know, layers in AutoCAD are similar to layers in Photoshop but don't have intrinsic display order)
The goemtry will be stored in the drawing file as 2D sketch entities and will not be associative to the model
You may notice some irregularities in annotations
Drawing views won't be associative to one another (if you modify the top-view, it won't affect the front view)
Now, just about every one of us has had to devise a strategy to integrate AutoCAD drawings into a Solidworks workflow. I myself have had to do this a couple of different ways across a couple of employers and what I've found most important is establishing which file is the controling document for design changes.
If you shop-floor people are going to pull up the AutoCAD drawing in Fastlook, right or wrong, there's no point in converting that drawing to Solidworks without a compelling geometry change.
Similarly, if your checkers are anal about the differences in font and line rendering between AutoCAD and Solidworks, your better off leaving them with what they expect.
On the other hand, if your practice is take the CAD model drop it into a CAM program and press the 'go' button, then you want that model driving the drawing document and recreating the Solidworks model is the only way to ensure that relationship is preserved.
If the AutoCAD drawings are schematics or wiring diagrams or the like, then there's little to be gained by going through the trouble of converting them to Solidworks.
If the drawings are of COTS items and legacy components that aren't going to be revised, it is similarly unpractical to go through the process of importing them into Solidworks. Use the imported Pro-E parts for your assembly models and leave the AutoCAD drawings for dimensional reference. You might want to institute a policy that if a model is going to be changed, the drawing has to be recreated in Solidworks in order to prove that unchanged dimensions and design intent have been preserved.
Where I have seen the greatest need to straight out recreate the drawing in Solidworks arise is when you're unsure about the fidelity of the model to the drawing or vice versa. In our case, we had models that didn't match the AutoCAD drawings that were released and our interference and hole alignment calculations were all screwed up. If you need to prove that a model is faithful to an AutoCAD drawing, the best thing to do is recreate the AutoCAd drawing in Solidworks. In all earnestness: I would do this for any part which is used in production and has a design critical fit.
Finaly, if a part is simple: composed of a couple of features and described with only a few dimensions, it's faster just to redraw the thing than it is to mess with the import wizard.
Two bits of follow-on advice.
When you disposition your parts (redraw, import, leave as-is) explain the situation to your teammates so that they know how to regaurd the parts when they use them.
Write out your conversion plan-whether it's all-at-once, as-you-go or piece-meal and get it approved as a design guideline or SOP. The last thing you want is to have a mixed bag reliable and sketchy parts and leave it unclear which is which.
Welcome to the forum.
What version of SW are you importing into?
What exactly are you talking about when you say maintining the SW tree?
I am importing in to SW 2010. When I import these flies there is no Feature Manager Design Tree. I have Probably close to 1000 drawings in Auto Cad 2000. I need a fast efficient way to convert these. I have not been working with SW more than a couple months. Alias was my prior program. Any help would be great.
Ok, do you need to make 3D models of these drawings or are you maintaining 2D drawings.
Also I would be aware that there might be an incompatiblility issue between SW and Autocad seeing
they are not comparable versions.
3d models are in Pro E. I have been able to import most of these and make changes where needed and save as SLDDRW files. Seems to be going ok with the exception of a few. Basically everything was in ProE and Auto CAD 2000 and I am working on getting every thing in to SW.
So my main concern right now is converting these 2D drawings as best as possible. Would be a ton of work to redo every one. Rob
If you are attempting to get the .dwg files into .slddrw format, look at the API help on this command: InsertDwgOrDxfFile.
If you are looking for a fast way to just convert them then look at what Brian suggested regarding that macro.
Also since you are in 2010 take a look at the SW drawing editor. That almost mirrors Autocad in looks and commands.
Or down load the replacement to the drawing editor, Draftsight. Both of these you should be able to callup the Autocad
files directly. But with all of this said that is why I asked you in my last posting if you needed to convert these drawings to models.
You said you had Pro-E model that you have converted fairly successfully. If some of these drawings in autocad represent these Pro-E
models that you have converted into Solidworks, why not just create new drawings from those models? Then there will be the parametric
link with them.
Great advise all of you!
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