Building new parts from assemblies

[MesaTactical]

I am to design some new parts that fit on a specific shotgun receiver. I have a SolidWorks solid model of the shotgun receiver, except that it is in the form of an assembly (actually a .SAT file that I can import).

It would be simple enough for me to make the required sketches for the new part using the Convert Entities tool, but I can't do a boss extrude on a new part from inside an assembly drawing.

The assembly breaks down into a number of parts files, but it's the assembly as a whole I need to mate to with the new part.

Is there a way to blend multiple parts into a single body in an assembly? Or some way to build new parts in an assembly? Or a generally accepted method for building new parts from an assembly?

 

[Theophilus]

You can create new parts within an assembly with Insert > Component > New Part. You then select a plane or flat surface to act as the anchoring plane for the part in the assembly. I recommend using the Front Plane of the Assembly, although you can use faces of parts within the assembly. You can then convert the entities of other parts within the assembly to create a new parametric part.

Check help files on this for more details.

Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[ShaggyPE]

To answer your merging of separate parts into one part file, here is your option. Open the assembly and saveas a part. You will have three choices in the form of a check box.
1. All components
2. All faces
3. Exterior Faces

You probably want the all components selection.

This will effectively create a part file of the entire shotgun. You will however lose all the associativity of the assembly to the newly created part. In other words, if you update a part in the gun assembly, it will not update in your newly created part file.

I have used this method in the past to "merge" a supplier's assembly into an off the shelf part file. I have also done the same with assemblies that my company manufacturered that were designed into a customers bigger system. I created a part file of my assembly and emailed that. They had no use for all of the parts in my assembly, and I didn't want them to have all that intellectual property anyway.

 

[MElam]

It sounds to me like you just need to follow Theophilus' advise and start with Insert > Component > New Part.

You probably created the sketch at the assembly level instead of in a new part, which would explain why you can't do a boss extrude. You need to be editing a part.