As Kelvin Said,
Libary Features are the way to go, Either to add bodys & features or cuts.
You setup configurations of "Standard" items and stuff, however you create custom items as well. As long as you capture those dimensions you want.
Attached is example of a Stud. I can choose the location, Weld depth & Length. However I blocked the ability to change the Stud Diameter & Hole diameter.
This can only be done at the part level.
Stud.SLDLFP.zip 66.6 KB
John,. you're going to have to clarify what you mean by samples, bodies and document.
It sounds like you're wondering if it's possible for you to make a set of features into a part, insert that part into the assembly and then be able to modify it without affecting the original.
If that's the case then there are two ways that I can think of for you to go about it.
1) make a template. No you can't insert a template into a new assembly, but you can insert a new part created from a template into an assembly. The part will-by default-come in as a virtual component and will be saved within the assembly until you tell SW to save it as an external file and the template file that you used to create the part will be unaffected. Change the dimensions, modify it, knock yourself out. New parts are placed either on a planar face of your choosing or at the assembly origin. However, all of you have to do in order to mate one of your new parts is either change the status from fixed to float or delete the inplace mate (which is there for top-down modeling) Then you can position and mate your new part the same as any other.
2) make your sample part as a regular part. Insert it into an assembly. Mate it as desired. then, right-click on the par tin the feature tree and select 'make virtual' from the context menu.
If that's no helpful, then tell us a little more about what you're trying to do.
Looking at method 2; I inserted 2 parts into an assembly, mated them, halved the length of the UB part, dragged and dropped the same UB part from the Design Library, right clicked the first UB part in the FT and the context menu displayed.
I observed that:-
1 The copy dragged from the Design Library is the half length (instant propagation back to the library).
2 I cannot see "make virtual" in the context menu. Help found no match for the string "make virtual".
Method 1 will result in a template document for each part in the assembly, plus a part document for each part in the assembly, plus the assembly document.
I was hoping for something less clumsy.
Whoops, I realise now that I need a document for each part so that they can be fabricated to different dimensions for each job.
Message was edited by: John Sutherland
John, I didn't realize you were using 2009. The ability to make an existing part a virtual part was introduced in 2010 or 2011. so method 2 is not going to work.
Method 1 will not require a different template for each part, because when you create the part using a template, you can modify it without affecting any other parts created from that template. If your screen capture is any indication, you're working with steel shapes. You would only need a template for each steel profile. Since the parts are virtual and are saved in the assembly, there isn't really any file management to speak of.
But now that I have a better idea of what you're doing, why don't you just create your frame as a weldment?
I see Weldments as pipe routing rebadged for structural tubes. If I get a tube job I will look again at it.
It seems that the best workflow will be Part Templates>Parts>Welded sub assemblies>Bolted general assemblies.
The shop likes a drawing of each part to keep it simple for the tradesmen, then a drawing of each weldment.
Given that each weld results in a part file, a folder for each weldment will keep the many files together.