The wording in my post was incorrect. I should have said bodies instead of features.
You can still hide the bodies and/or delete to drill down into the assembly. I believe that is what he is trying to avoid.
Will the user be sectioning your assembly? If so, saving with 'exterior faces' selected will not work either. As mentioned, you will just have an external shell, nothing more.
I believe the best approach would be as I mentioned before with the fix that Dustin added about the bodies that would not combine.
do a file, save as , then select part for file type.
sometimes takes a while.
What Greg said is true but you still need to be careful. There are 3 options when you save an assembly as a part: Exterior Faces, Exterior Components, and All Components. How much information you want to send will determine which option you select.
Regardless of the method of conversion, the features are still selectable in the FMT and can be hidden or deleted. The receiver of the file can pick through it and see the construction of the assembly.
This could take a substantial amount of time, but how about saving the assembly as a part. Then open the part and combine all bodies. Export this as an IGS for STEP file. If the receiver requires a 'native' SolidWorks file, just open the IGS and save it again as a SLDPRT.
I believe that would solve the problem. The receiver would be able to see the assembly, but would not be able to disassemble it.
2636 wrote: Regardless of the method of conversion, the features are still selectable in the FMT and can be hidden or deleted. The receiver of the file can pick through it and see the construction of the assembly. This could take a substantial amount of time, but how about saving the assembly as a part. Then open the part and combine all bodies. Export this as an IGS for STEP file. If the receiver requires a 'native' SolidWorks file, just open the IGS and save it again as a SLDPRT. I believe that would solve the problem. The receiver would be able to see the assembly, but would not be able to disassemble it.
no if you save the assembly as a part you loose the features in the tree! it is just a dumb solid body or slew of bodies. even in iges it would become a bunch of bodies.
This model is going to be brought into Revit to be part of a rendering. It doesn't look like PDF is an import option in Revit.
If the file is saved as a part and the 'exterior faces' option is selected, the result is all hollowed out solids. So even if the feature is selected and hidden the user still cannot see the interior geometry.
wat dustin suggests is right way
after u combine all then select solidbody in featurem manager tree. right click and import into new part. later u can break all links. this way u will get a single solid body which has no feature tree no history.
I guess this will work fine for ur requirement.
DUDE WHAT DO YOU WANT! Send them a jpg/tiff file of all the views you want then have them tweek the pics! anything else out of SW will be some sort of surface/wireframe data.
37332 wrote: But if I open those bodies I can still see the part grometry!
EXACTLY to the above statement! if it's graphics send jpg or tiff if they need the surfaces you have no other choice but to send iges, parasolid, step and they get the solid data...sorry!
HAVE THEM SIGN A CONFIDETCEALITY AGREEMENT!
Steve wants to turn an assembly into a single imported body to send out. I've mocked this up and it works as Tony said with the end result being ONE body. I started with 2 blocks and a cylinder in an assembly:
Save the assembly as a part file with all components option. Open the resulting part file and do a combine on all bodies until only 1 body is remaining in the part:
Save this as an IGES, STEP, Parasolid and you get the assembly as one body in a part file with NO features to drill down in or anything... just what the doctor ordered:
Yes I under stand that...BUT if the bodies do not touch.....they will still be seperate bodies.....so what he is asking isn't a simple task!
he would have to model in connection bodies for it all to become one solid body. so he may have to make some configs of his parts to make it look the way he wants in the end
also sounded like he wanted a PDF file to do the rendering which to me ment that he doesn't want to send out any type of solid/surface info to whoever is doing the rendering.
PS: I also taught SW at the VAR for 3 years and use multible every day as a model maker machinist.
Tony did say "This could take a substantial amount of time"... I'd say that is a good disclaimer. Yes, the end result is not an easy one to get to... but if you want to get there sometimes you gotta take the long and only road.
No, he is needing it to go into Revit... which he said "it doesn't look like PDF is an option" so it looks like he doesn't just want a 3D PDF but actually needs the solid body.
At this point I think this is the best approach. I've saved the exterior faces into a sldprt file and combined them into SAT file that I can send them.
Thanks for all the help everyone!
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