Drawings - How to change from Part to Assembly

[pgp001]

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

 

[JMirisola]

You could simply insert the nuts into the part, thereby keeping it a part file versus creating an assembly file. While I'm not sure if the BOM would work correctly, you'd at least have the end result you're looking for.

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

 

[dgowans]

If this happens all the time you need to examine your process. On parts like this I'd get in the habit of inserting your part into an assembly, even if there are no other parts. You can still generate your drawing on the 1 piece assembly and it will look exactly the same. Then when you add weld nuts, PEMs, etc. your drawing isn't affected.

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.

 

[CorBlimeyLimey]

It should literally take just a few seconds to create an assy drawing. It's not like you would be fully dimensioning the plate, that would be done at the part level. All that's needed would be to add a BOM.

The creation of drawings can even be automated using the Task Scheduler.

 

[handleman]

Since the nuts are to be welded on I would guess that the "assembly drawing" can't be just that. He needs one drawing showing both how to fabricate the plate and the fact that there are nuts welded onto it.

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.

 

[CorBlimeyLimey]

Using a multi-body part as an assy is not recommended practice.

However, if you decide to go this route, you could also create "with nuts" and "without nuts" configurations, and show both in the assembly part drawing

As stated above though, my choice would be to create a real assy and separate real assy drawing.

 

[handleman]

True, it's not recommended to use multibody parts in place of assemblies. However, once the nuts are welded on it's not an assembly but a part. Whether or not to create two separate drawings would really depends on your industry, drawing routing, fab/machining procedures, etc. In our company, parts drawings go to the fab and/or machine shop, and assembly drawings go out to the assembly floor. If I created two separate drawings (part drawing for the plate and assembly w/BOM for adding nuts) then when I issued the two drawings one of them would go to the wrong place. The plate drawing would go to fab and the assembly drawing would go to assembly. The nuts and plate would be delivered to the assembly guy, who would look at the assembly drawing, see that the nuts were supposed to be welded on, cuss me, and carry the drawing, plate, and nuts over to the fab shop to be welded on.

 

[fcsuper]

I thought you can insert anything you want into a drawing replacing the current referenced part or assy by using the Options button on the Open screen?

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA

http://sw.fcsuper.com/index.php

 

[PeterStock]

An option for the future would be to create all of these plates as an assembly with one part (the plate). Create your drawing of that, the if there needs to be nuts added, you do not have to redo the drawing.

Peter Stockhausen
Pollak Switching Products

 

[handleman]

Nope. You can only change out files of the same type (part or assembly) from that screen. This applies both to drawings and to assemblies.

 

[J-C]

We insert weld nuts into the part file. You have to do the BOM manually though.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.1 on WinXP SP2
SolidWorks 2007 SP2.1 on WinXP SP2

 

[CorBlimeyLimey]

... once the nuts are welded on it's not an assembly but a part

Why? Because bits don't fall off when you pick it up?

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.

 

[engAlright]

As CorBlimey says we also treat weldments as assemblies since it's created from more than one part...we have seperate SLDDRW's for assems and parts.

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...

 

[handleman]

As I said, it's dependent on your industry, drawing routing procedures, fabrication/machining procedures, etc. My industry is machine design. For us, if it can't be assembled and/or non-destructively disassembled with standard hand tools then it is pretty much a part. In our case, all welding takes place in one location. In that location, nuts are stock items that are readily available. No need to order them or call them out on a BOM. For this level of complexity it wouldn't make sense for me in my case to create two drawings to be read by the same guy at the same time. Additionally, I would hav to go through the extra trouble of making sure the assembly drawing did not follow our standard routing for assembly drawings. Then I would have to explain to the assembly guy why the part he has in his hand (which he can't disassemble) is called an 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.