I have an assembly full of virtual parts. I really would like to export all of the sketches of these virtual parts at once into a .slddrw (that will be saved as a .dwg for use in Autocad) . I say sketches becasue in these sketches I typically have some construction lines I need copied. I currently have to manually select/copy/paste into a .slddrw
Someone please blow my mind and tell me how this is possible, because I'm all out of ideas.
Thank you Habib, but I don't think that would work the way I want. I have all my virtual parts on different planes.
Stephen
I have zero knowledge of autocad but is it possible you could export your sketches directly via an iges file?
Other than that it seems like you need a macro to traverse your tree and do it for you.
Rob Edwards wrote:
Stephen
I have zero knowledge of autocad but is it possible you could export your sketches directly via an iges file?
Other than that it seems like you need a macro to traverse your tree and do it for you.
This will export your sketches in 3D space, not flat into a 2D dwg. Not sure if your AutoCAD/AutoCAD work-alike will open IGES files.
Why would you not use your SolidWorks sldasm file and create a SolidWorks slddrw drawing?
After you create the slddrw you can Save As to a DWG. Does not even need to be a complete slddrw with dimensions; just set up the views, sections, etc that you want to export to DWG.
I am guessing you now are trying to figure out how you are going to set up your dwg file for nesting and lasering/waterjetting your parts.
You can convert the virtual part assembly file into a standard external part assembly.
What we do is make a helper assembly and drop all the parts in that we wish to laser or waterjet, etc and mate as needed to fit on the raw sheet material. I usually create a sketch on the front plane that shows raw stock size. Mate all the parts to front plane and space as needed. Create a SolidWorks drawing from the helper assembly, then File > Save As to a DXF/DWG for manufacturing.
2016 SOLIDWORKS Help - Saving Virtual Components to External Files
Hello Anna,
I see what you're saying, however I don't know if it will actually be a faster process. This is the process I have to take now once my assembly is created with my virtual parts (note, I would like to have my construction lines be transferred as well).
Step 1 - Open a new .slddrw at 1:1 scale with blank template
Step 2 - begin copying all my virtual part sketches from .sldasm file (even construction lines are copied)
Step 3 - paste in the .slddrw file I opened
Step 4 - tab back to .sldasm file, and repeat processes until all virtual part sketches are copied and pasted to .slddrw file
Step 5 - once all sketches are copied to my .slddrw file, save the file as .dwg so it can be opened in AutoCAD
Pick your poison....
What you wish to do it not stock SolidWorks behavior. Would require custom programming.
If you make a change you have to re-export & setup your dxf from scratch.
If you use a SolidWorks assembly (not virtual) you will not have to re-create your dxf file, it will update automatically in the helper sldasm/slddrw. Just save out a new dxf file for manufacturing.
You can leverage your assembly for future designs with Pack and Go to make clones with updates and not have to re-do from scratch.
Hi Stephen
I'm practising my API skills so thought I'd have a crack at this. This probably isn't exactly what you want, but I hope it's an improvement. It's probably possible to automate the whole process, but thats beyond me at the moment. Also I confess I got slightly drunk last night mid way through writing this so you'd better test it on something not important. I had a few nasty crashes, from my programming errors and I cannot guarantee I have removed all the bugs.
The nice thing about using derived sketches is that you can move them around like blocks, but they update with the part
Is there supposed to be an attachment?
I literally laughed out loud in my office when I read that
Hi Stephen
Yes you don't see it when in in-box thats all.. did you find it?
The macro works by deriving your sketches onto a single plane.
Sometimes the sketch may appear flipped, so
and adjust the sketch plane eg
All the best, hope it's helpful
Option 3 if you have no constraints
This is what I always do.
I'm not sure if it's the best or the fastest. But it is what seems to be OK for me.
My assemblies are full of virtual parts too. That's why I think we are in the same boat.
In my assembly, I add several Display States. In each Display state only one or two virtual parts are shown and the rest are hidden (It depends on my need how many parts I show in a view of drawing). Let's say DisplayState0 shows all parts and DisplayState1 shows only part1 and the rest are hidden.
Then in drawing file I drag a view and select DisplayState1 in view's property. There, I can right click the sketches in tree and select Show to show the sketches in drawing.
In the following image, Trimetric view shows DesplayState0 (all parts)
but the other view shows DisplayState1 with part1 and Sketch35 shown.
If you need all sketches, you can filter Sketch in your tree and set all of them to Show with one click.