Drawings - How to change from Part to Assembly
Drawings - How to change from Part to Assembly
(OP)
I have come up against an issue that I cannot find a solution for.
If I create a solid part which is a flat plate with some holes in it and then create a drawing from it, all is well.
Now someone comes along and asks for some hexagon nuts to be welded over the holes, no problem I make assembly from part and give it the same file name, I then add the nuts from our standard library and mate them etc.
The problem now is that the drawing still references the original solid part and not the assembly.
I have tried to open the drawing and press the references button to link it to the assembly, but this does not work, I get a message about not being able to change form part to assembly type.
It seems to be an awful waste of time for me to have to start and create a new drawing from scratch, especially when all the dimensions are identical.
This is not just a one off, we have it quite regularly.
Please someone tell me I have missed something really obvious.
Thanks
Phil
If I create a solid part which is a flat plate with some holes in it and then create a drawing from it, all is well.
Now someone comes along and asks for some hexagon nuts to be welded over the holes, no problem I make assembly from part and give it the same file name, I then add the nuts from our standard library and mate them etc.
The problem now is that the drawing still references the original solid part and not the assembly.
I have tried to open the drawing and press the references button to link it to the assembly, but this does not work, I get a message about not being able to change form part to assembly type.
It seems to be an awful waste of time for me to have to start and create a new drawing from scratch, especially when all the dimensions are identical.
This is not just a one off, we have it quite regularly.
Please someone tell me I have missed something really obvious.
Thanks
Phil






RE: Drawings - How to change from Part to Assembly
Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP2.0, Dell M90, Intel 2 Duo Core, 2GB RAM, nVidia 2500M
http://designsmarter.typepad.com/jeffs_blog
RE: Drawings - How to change from Part to Assembly
Alternatively, you could insert a toolbox fastener into your part as a derived part and continue on your way.
I'd go the assembly route.
RE: Drawings - How to change from Part to Assembly
The creation of drawings can even be automated using the Task Scheduler.
RE: Drawings - How to change from Part to Assembly
If you have SW '06 or later it is almost as easy to add the nuts to the part as it is to add them to an assembly, especially if the holes they go on were created with a hole wizard feature. Just go to Insert->Part... and drop the nut into the part. You may have to hit the "Constraints" button on the "Move" property manager to access the mating functionality. Mate your nut in place, and then use the hole location sketch from the hole wizard feature to create a sketch-driven body pattern for the rest of the nuts. Easy as pi to 2 decimals.
RE: Drawings - How to change from Part to Assembly
However, if you decide to go this route, you could also create "with nuts" and "without nuts" configurations, and show both in the
assemblypart drawingAs stated above though, my choice would be to create a real assy and separate real assy drawing.
RE: Drawings - How to change from Part to Assembly
RE: Drawings - How to change from Part to Assembly
Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA
http://sw.fcsuper.com/index.php
RE: Drawings - How to change from Part to Assembly
Peter Stockhausen
Pollak Switching Products
RE: Drawings - How to change from Part to Assembly
RE: Drawings - How to change from Part to Assembly
Jason
UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.1 on WinXP SP2
SolidWorks 2007 SP2.1 on WinXP SP2
RE: Drawings - How to change from Part to Assembly
Are rivetted parts no longer an assembly? How about screwed-on parts? Or bolted parts where the nut is tack welded or physically secured?
Weld Nuts (or any other parts) can be removed just as rivets and screws can be removed.
What would you do if you had 50 different sheet metal parts being made at various vendors being welded together at another plant/department?
I guess it depends on how you look at it, but a plate with welded nuts is still a collection of separate parts and, IMO, might as well be treated as an assy.
And yes, I realise that SW is breaking it's own rules/guidlines by using a multi-body part as a weldment ... but at least they substitued the BOM with a Cut List.
My first choice would be an assy, my second would be a multi-body part with configs. One of the Pros and Cons of SW is that there's always more than one way to do something.
RE: Drawings - How to change from Part to Assembly
If a single drawing is needed to detail both part and assembly, why not just add a view of the assembly to the original part drawing? Surely you wouldn't use the view of the assembly to fully detail the part...
RE: Drawings - How to change from Part to Assembly
However, our division is part of an OEM automotive parts manufacturer. The finished product we sell (which is machined, handled, tested, cleaned, packaged, etc. by equipment that my division designs and builds) has scores and scores of drawings going all the way from raw material, molding, die cast, machining, welding, subassembly, process, inspection, etc. In this case it makes sense to have all manner of drawings, since each part, raw material, etc must be procured separately and brought to the correct place to be assembled, by welding or any other process.